From nek5000-users at lists.mcs.anl.gov Sun Jun 1 00:48:05 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 1 Jun 2014 13:48:05 +0800 (CST) Subject: [Nek5000-users] test of the time average of turbChannel--what's wrong? In-Reply-To: References: , Message-ID: Hi,Paul: I modified this part of code in turbChannel.usr: if(icalld.eq.0) then call rzero(uavg,n) call rzero(urms,n) call rzero(vrms,n) call rzero(wrms,n) call rzero(uvms,n) atime = 0. call planar_average_s(yy ,ym1 ,w1,w2) icalld = 1 endif timel = time-0.02 !DT=0.02 dtime = time - timel atime = atime + dtime In this way, dtime=DT. I look into the code avg_all and find that it will write several files of avg fields. My question is: 1/ Is the average field file can be read into the solver when turn the 'Restart option' on, how can I accomplish this? 2/ For channel flow, I only need the file along y direction, so I need to dump the statistics into 1_D. If the answer of question is 'Yes', then I will want to output the avg fields(uavg,vavg and wavg). I find that in the avg_all subroutine, output2 and output are called, where are the two subroutine located? At 2014-06-01 12:31:52, nek5000-users at lists.mcs.anl.gov wrote: Hi Xianbei, You are correct that dtime should be equal to DT. If you look at avg_all() in navier5.f in the main nek source directory, this is what happens because timel is updated after the averaging. In the turbchannel case, this was not done - so I've now modified the .usr file to reflect this. I would suggest to simply use the avg_all code to do the time averaging and then to use those average fields to generate profiles. Thanks for pointing out the problem with the turbChannel example. Paul From:nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Saturday, May 31, 2014 10:38 PM To:nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] test of the time average of turbChannel--what's wrong? Hi Xianbei, The usr files are meant to be modified by the users, so you can adjust it to suit your needs. Paul From:nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Saturday, May 31, 2014 9:58 PM To: Nek5000 Subject: [Nek5000-users] test of the time average of turbChannel--what's wrong? Hi, all: I read about the time average method in the turbChannel.usr/userchk,here is the origin codes: if(icalld.eq.0) then call rzero(uavg,n) call rzero(urms,n) call rzero(vrms,n) call rzero(wrms,n) call rzero(uvms,n) atime = 0. timel = time call planar_average_s(yy ,ym1 ,w1,w2) icalld = 1 endif dtime = time - timel atime = atime + dtime if (atime.ne.0. .and. dtime.ne.0.) then beta = dtime/atime alpha = 1.-beta ifverbose = .false. call avg1(uavg,vx ,alpha,beta,n,'uavg',ifverbose) As seen , atime and timel is initialized by 0 and time, so when time=time+DT, dtime=DT, atime=DT, so the first average value is vx(t=DT), when time=time+2*DT, dtime=2*DT(timel is not changed, just equal to the initial value ),atime=3*DT, here question comes: this will lead to vxmean(t=2*DT)=2/3*vx(t=DT)+1/3*vx(t=2*DT), this is not what we respect. The right one is make sure that dtime=DT all the time. Also, I do a test to verify this.In order to be more reliable, the velocity isn't nomorlized by u_tau. First, calculate by 1 step and output the means.dat, so the value equal to the time=DT's #time = 2.0000000E-02 # y uup_tau Umean 0.000000000E+00 2.031155153E-02 0.000000000E+00 2.565198406E-03 2.031155153E-02 1.285886819E-02 then restart with the field from previous calculation and output the means.dat, this will output the value of time=2*DT's, #time = 4.0000000E-02 # y uup_tau Umean 0.000000000E+00 2.072569248E-02 0.000000000E+00 2.565205097E-03 2.072569248E-02 1.288671376E-02 At last, restart the calculation and run 2 steps to calculate the average of vx(time=DT) and vx(time=2*DT) #time = 4.0000000E-02 # y uup_tau Umean 0.000000000E+00 2.061649552E-02 0.000000000E+00 2.565198406E-03 2.061649552E-02 1.287524390E-02 As can be seen, the 2 step average is almost equal to the average of step 1 and step 2. So what's wrong with my understanding? Is timel alway updated to the previous time and make sure that dtime=constant? How? Can anyone help? Xianbei ?????????????? -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Sun Jun 1 04:15:00 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 1 Jun 2014 09:15:00 +0000 Subject: [Nek5000-users] Questions in AXHELM and WLAPLACIAN In-Reply-To: References: , , Message-ID: Hi Paul, gradm1 is working now, the problem was indeed that the declaration of output variables was not in a common block. Thank you ! Best regards, Emmanuel On 1 Jun 2014, at 8:49, > > wrote: Hi Emmanuel, Regarding the gradm1() crash, did you declare Tx,Ty, and Tz in a new common block of your own creation? This would be important to do. Regarding where to modify the code - the most common approach is to create a new routine (say, "subroutine make_term3") which generates the required source terms when called once per timestep from userchk. You would store these source terms in an array and then load from this array in the userq() routine, which is called point-by-point, field-by-field, by nek as needed. Regarding your earlier email about replacing axhelm, the strategy you propose would not give the desired result. My suggestion would be to look carefully at some of the FEM/SEM literature. There are a couple of JCP papers by Tomboulides & Orszag (for low Mach), my 97 JCP paper (on Schwarz, but generally on the SEM discretization), and the book High Order Methods for Incompressible Flow with Deville & Mund. Please let me know if you have further questions. Best, Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Saturday, May 31, 2014 3:47 AM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Questions in AXHELM and WLAPLACIAN Hi Paul I have some difficulties to compute a simple gradient of a variable. I think I?m confusing something. Basically I would like to modify the temperature and species equations to add a new term in order to take into account a velocity correction related to mass conservation and species diffusion coefficients. For temperature the equation is: d T /dt = term1 + term2 + term3 with term1 = - U grad (T) term2 = 1/rho Cp * grad ( lambda * grad (T)) term3 = 1/rho Cp * (rho * sum_k [Cp,k * (Y_k * D_k * grad(Y_k) - Y_k * sum_j [D_j * grad(Y_j )] ) ] ) * grad(T) and for species equation : d Y /dt = term1 + term2 + term3 with term1 = - U grad (Y) term2 = 1/rho Cp * grad ( lambda * grad (Y)) term3 = - 1/rho * grad (Y * sum_k [D_k * grad (Y_k) ] ) where D_k or D_j are the species diffusion coefficients, T the temperature and Y the species mass fraction. I am using the low-Mach number formulation and solving the equations with CVODE. Basically term1 is computed by the routine convab while term2 is computed by routine wlapacian. This is the current official nek implementation. Now I would like to add the term3, which involves some gradients of temperature or species variables. I think the simplest way is to modify the routine convab or maybe makeq.f However I tried a simple call gradm1 (Tx,Ty,Tz,T) but NEK crashes with a segmentation fault error. I tried to debug the routine gradm1, and it appears that it crashes during the loop do i=1,lxyz ux(i,e) =jacmi(i,e)*(ur(i)*rxm1(i,1,1,e) $ + us(i)*sxm1(i,1,1,e) ) uy(i,e) =jacmi(i,e)*(ur(i)*rym1(i,1,1,e) $ + us(i)*sym1(i,1,1,e) ) enddo after reaching a particular element e (in my case it crashes for element 9). So my questions are just: 1) According to the implementation of term3 in temperature and species equations, what is the best way to proceed? I have think about modifying convab or makeq but is it a good idea? 2) Is it a good idea to use gradm1? Why does it crash for a particular element? Should I pay attention to something in particular when using this routine? Thank you very much for your help ! Best regards, Emmanuel On 30 May 2014, at 10:25, nek5000-users at lists.mcs.anl.gov wrote: Hi Emmanuel, Strictly speaking, our functions are only once differentiable -- they are C0, not C1. The test functions are also in H1 (i.e., are C0) and therefor the standard Galerkin approach is to transfer one derivative to the test functions via integration by parts and thus avoid twice differentiating a function. If you just want the gradient of something, you would use gradm1 (gradient for a quantity on mesh 1). Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Thursday, May 29, 2014 7:47 PM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Questions in AXHELM and WLAPLACIAN Hi Paul, Thank you for your quick answer, this is really helpful. I still have a question concerning the computation of a gradient. Why did you construct the diffusion operator with the helmholtz routine? Why not using directly the routines gradm1 ? By the way I am not sure to understand the differences between gradm1 (navier5.f), wgradm1 (navier1.f) , gradm11 (navier2.f) and gradm11ts (navier2.f). I guess that the w letter refers to the weak formulation, but I don?t understand in which cases we need to choose a formulation instead of others. In summary, if I want to modify the temperature/passive scalar equations to add a term that contains a gradient of the solved temperature/PS variable, for example, which ?gradm? routine do I need to use? Thank you for your help ! Best regards, Emmanuel On 29 May 2014, at 20:20, nek5000-users at lists.mcs.anl.gov wrote: Hi Emmanuel, axhelm effects the weak Laplacian plus the mass matrix. Specifically, if you wanted to solve: (1) -nabla . [ h1 * nabla ] u + h2 * u = f with h1, h2, and f all functions of X=(x,y,z), the discrete form would be: (2) A(h1) u + B(h2) u = B f or (3) H u = B f where A is the (h1-dependent stiffness matrix and B(h2) is the h2-dependent mass matrix. For the SEM, B is diagonal, so B(h2) = h2*B, where we view h2 as a diagonal matrix. In Nek5000, a matrix-vector product w = Hu is effected via call axhelm (w,u,h1,h2,imesh,isd) with w,u,h1,h2 being arrarys. Here, imesh indicates if you are on the fluid mesh or thermal mesh. The fluid mesh is a subset of the thermal mesh in the case of conjugate heat transfer between a fluid and a solid. isd indicates which spatial direction is considered in axisymmetric applications where u is a component of a vector field. Notice the sign of the Laplacian in Eq. (1) -- that may help resolve your second question? (There is a sign change that ariss from the standard integration-by-parts stepin the weak form.) Paul On Thu, 29 May 2014, nek5000-users at lists.mcs.anl.gov wrote: Dear nek5000 team, Could you help me with the 2 questions below? Thank you very much ! 1) Concerning the routine ?axhelm? in hmholtz.f. If I am right, one possibility of this routine can be the discretisation of the diffusion operator. However it is not clear to me if axhelm performs: a) vdiff x Laplacian(phi) or b) grad ( vdiff x grad (phi) ) phi being the variable solved for (T or PS for example). So, is it actually a) or b) ? 2) In the routine wlaplacian in navier1.f, I am not sure to understand the consequence of the line: call sub2 (out,wrk,ntot) after the lines: call bcneusc(out,1) call axhelm(wrk,a,diff,h2,imesh,1) If I am right, this will change the sign in front of the diffusion operator, right? Because in makeq.f, I am not sure that the line call add2(bq(1,1,1,1,ifield-1),w1,ntot) will actually assemble the RHS of the transport equation : - (vtrans) x U grad (phi) + grad ( vdiff x grad (phi) ) Thank you for your help ! Best regards, Emmanuel _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jun 2 00:46:16 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 2 Jun 2014 13:46:16 +0800 (CST) Subject: [Nek5000-users] question on subroutine sem2lex Message-ID: Hi,all: In the parallel version of sem2lex, there is a part of code wrote as following: if (gllnid(eg).eq.nid) then ! element eg is on this processor eg = eg+1 le = gllel(ge) ! le is local element number do iz=1,nz1 do iy=1,ny1 do ix=1,nx1 However, ge doesn't appear anywhere except here,(le=gllel(ge)), so is this should be "le=gllel(eg)"? Or just my misunderstanding? Xianbei -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jun 2 02:57:58 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 2 Jun 2014 02:57:58 -0500 Subject: [Nek5000-users] Reg: Visit Message-ID: Hello all, I cannot view the output files from the nek5000 .fld format using VisIt. I am very new to using nek5000 code. . I tried paraview too. It didn't work. Help greatly appreciated. The following message was posted in forum but didn't find reply so had to post. error message VisIt could not read from the file "C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowmach\lowMach_test0.f* database". The generated error message was: There was an error opening C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowmach\lowMach_test0.f* database. It may be an invalid file. VisIt tried using the following file format readers to open the file: Silo Thank you, Ravi Kiran Pendyala, Graduate Research Assistant, Department of Aerospace Engineering, Mississippi State University, Email: srp265 at msstate.edu -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jun 2 03:18:51 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 02 Jun 2014 10:18:51 +0200 Subject: [Nek5000-users] Reg: Visit In-Reply-To: References: Message-ID: Hi Ravi, Did you create a metadata file ?? A meta data file is the one which helps you to open a *.fld or *.f00000 file in visit It looks like this NEK5000 version: 1.0 filetemplate: divpipe%01d.f%05d firsttimestep: 1 numtimesteps: 09 Best regards, Kamal On 02/06/2014 09:57, nek5000-users at lists.mcs.anl.gov wrote: > Hello all, > > I cannot view the output files from the nek5000 .fld format using > VisIt. I am very new to using nek5000 code. > . I tried paraview too. It didn't work. > > Help greatly appreciated. The following message was posted in forum > but didn't find reply so had to post. > > error message > VisIt could not read from the file "C:\Users\s > pendyala\AppData\Local\Programs\LLNL\VisIt > 2.7.2\lowmach\lowMach_test0.f* database". > > The generated error message was: > > There was an error opening C:\Users\s > pendyala\AppData\Local\Programs\LLNL\VisIt > 2.7.2\lowmach\lowMach_test0.f* database. It may be an invalid file. > VisIt tried using the following file format readers to open the file: Silo > > Thank you, > > > Ravi Kiran Pendyala, > Graduate Research Assistant, > Department of Aerospace Engineering, > Mississippi State University, > Email: srp265 at msstate.edu > > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jun 2 03:35:21 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 2 Jun 2014 03:35:21 -0500 Subject: [Nek5000-users] Reg: Visit In-Reply-To: References: Message-ID: No. I didn't not get a clue of working with metadata file. I read about it. Couldn't figure out how to create this. Is a a separate file or set of commands? Ravi Kiran Pendyala, > On Jun 2, 2014, at 3:18, nek5000-users at lists.mcs.anl.gov wrote: > > Hi Ravi, > > Did you create a metadata file ?? A meta data file is the one which helps you to open a *.fld or *.f00000 file in visit > > It looks like this > > > NEK5000 > version: 1.0 > filetemplate: divpipe%01d.f%05d > firsttimestep: 1 > numtimesteps: 09 > > Best regards, > Kamal > > >> On 02/06/2014 09:57, nek5000-users at lists.mcs.anl.gov wrote: >> Hello all, >> >> I cannot view the output files from the nek5000 .fld format using VisIt. I am very new to using nek5000 code. >> . I tried paraview too. It didn't work. >> >> Help greatly appreciated. The following message was posted in forum but didn't find reply so had to post. >> >> error message >> VisIt could not read from the file "C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowmach\lowMach_test0.f* database". >> >> The generated error message was: >> >> There was an error opening C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowmach\lowMach_test0.f* database. It may be an invalid file. >> VisIt tried using the following file format readers to open the file: Silo >> >> Thank you, >> >> >> Ravi Kiran Pendyala, >> Graduate Research Assistant, >> Department of Aerospace Engineering, >> Mississippi State University, >> Email: srp265 at msstate.edu >> >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jun 2 03:38:08 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 02 Jun 2014 10:38:08 +0200 Subject: [Nek5000-users] Reg: Visit In-Reply-To: References: Message-ID: Hi, Create a separate file with ' .nek5000 ' has extension and write those lines in it and open it via Visit and It should work. Best Regards, Kamal On 02/06/2014 10:35, nek5000-users at lists.mcs.anl.gov wrote: > No. I didn't not get a clue of working with metadata file. I read > about it. Couldn't figure out how to create this. Is a a separate file > or set of commands? > > Ravi Kiran Pendyala, > > > On Jun 2, 2014, at 3:18, nek5000-users at lists.mcs.anl.gov > wrote: > >> Hi Ravi, >> >> Did you create a metadata file ?? A meta data file is the one which >> helps you to open a *.fld or *.f00000 file in visit >> >> It looks like this >> >> >> NEK5000 >> version: 1.0 >> filetemplate: divpipe%01d.f%05d >> firsttimestep: 1 >> numtimesteps: 09 >> >> Best regards, >> Kamal >> >> >> On 02/06/2014 09:57, nek5000-users at lists.mcs.anl.gov wrote: >>> Hello all, >>> >>> I cannot view the output files from the nek5000 .fld format using >>> VisIt. I am very new to using nek5000 code. >>> . I tried paraview too. It didn't work. >>> >>> Help greatly appreciated. The following message was posted in forum >>> but didn't find reply so had to post. >>> >>> error message >>> VisIt could not read from the file "C:\Users\s >>> pendyala\AppData\Local\Programs\LLNL\VisIt >>> 2.7.2\lowmach\lowMach_test0.f* database". >>> >>> The generated error message was: >>> >>> There was an error opening C:\Users\s >>> pendyala\AppData\Local\Programs\LLNL\VisIt >>> 2.7.2\lowmach\lowMach_test0.f* database. It may be an invalid file. >>> VisIt tried using the following file format readers to open the >>> file: Silo >>> >>> Thank you, >>> >>> >>> Ravi Kiran Pendyala, >>> Graduate Research Assistant, >>> Department of Aerospace Engineering, >>> Mississippi State University, >>> Email: srp265 at msstate.edu >>> >>> >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jun 2 03:38:54 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 2 Jun 2014 03:38:54 -0500 Subject: [Nek5000-users] Reg: Visit In-Reply-To: References: Message-ID: Thank you for the kind and quickest response. Thanks again, Ravi Kiran Pendyala, > On Jun 2, 2014, at 3:38, nek5000-users at lists.mcs.anl.gov wrote: > > Hi, > > Create a separate file with ' .nek5000 ' has extension and write those lines in it and open it via Visit and It should work. > > Best Regards, > Kamal > >> On 02/06/2014 10:35, nek5000-users at lists.mcs.anl.gov wrote: >> No. I didn't not get a clue of working with metadata file. I read about it. Couldn't figure out how to create this. Is a a separate file or set of commands? >> >> Ravi Kiran Pendyala, >> >> >> On Jun 2, 2014, at 3:18, nek5000-users at lists.mcs.anl.gov wrote: >> >>> Hi Ravi, >>> >>> Did you create a metadata file ?? A meta data file is the one which helps you to open a *.fld or *.f00000 file in visit >>> >>> It looks like this >>> >>> >>> NEK5000 >>> version: 1.0 >>> filetemplate: divpipe%01d.f%05d >>> firsttimestep: 1 >>> numtimesteps: 09 >>> >>> Best regards, >>> Kamal >>> >>> >>> On 02/06/2014 09:57, nek5000-users at lists.mcs.anl.gov wrote: >>>> Hello all, >>>> >>>> I cannot view the output files from the nek5000 .fld format using VisIt. I am very new to using nek5000 code. >>>> . I tried paraview too. It didn't work. >>>> >>>> Help greatly appreciated. The following message was posted in forum but didn't find reply so had to post. >>>> >>>> error message >>>> VisIt could not read from the file "C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowmach\lowMach_test0.f* database". >>>> >>>> The generated error message was: >>>> >>>> There was an error opening C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowmach\lowMach_test0.f* database. It may be an invalid file. >>>> VisIt tried using the following file format readers to open the file: Silo >>>> >>>> Thank you, >>>> >>>> >>>> Ravi Kiran Pendyala, >>>> Graduate Research Assistant, >>>> Department of Aerospace Engineering, >>>> Mississippi State University, >>>> Email: srp265 at msstate.edu >>>> >>>> >>>> _______________________________________________ >>>> Nek5000-users mailing list >>>> Nek5000-users at lists.mcs.anl.gov >>>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>> >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jun 2 04:09:08 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 2 Jun 2014 04:09:08 -0500 Subject: [Nek5000-users] Reg: Visit In-Reply-To: <42328EFE-05CD-45EC-A746-BAD77726D5F7@msstate.edu> References: <42328EFE-05CD-45EC-A746-BAD77726D5F7@msstate.edu> Message-ID: Hi, I tried it. I still receive the same error though. Ravi Kiran Pendyala, Graduate Research Assistant, Department of Aerospace Engineering, Mississippi State University, Email: srp265 at msstate.edu On Mon, Jun 2, 2014 at 3:38 AM, Msu wrote: > Thank you for the kind and quickest response. > > Thanks again, > > Ravi Kiran Pendyala, > > > On Jun 2, 2014, at 3:38, nek5000-users at lists.mcs.anl.gov wrote: > > Hi, > > Create a separate file with ' .nek5000 ' has extension and write those > lines in it and open it via Visit and It should work. > > Best Regards, > Kamal > > On 02/06/2014 10:35, nek5000-users at lists.mcs.anl.gov wrote: > > No. I didn't not get a clue of working with metadata file. I read about > it. Couldn't figure out how to create this. Is a a separate file or set of > commands? > > Ravi Kiran Pendyala, > > > On Jun 2, 2014, at 3:18, nek5000-users at lists.mcs.anl.gov wrote: > > Hi Ravi, > > Did you create a metadata file ?? A meta data file is the one which helps > you to open a *.fld or *.f00000 file in visit > > It looks like this > > > NEK5000 > version: 1.0 > filetemplate: divpipe%01d.f%05d > firsttimestep: 1 > numtimesteps: 09 > > Best regards, > Kamal > > > On 02/06/2014 09:57, nek5000-users at lists.mcs.anl.gov wrote: > > Hello all, > > I cannot view the output files from the nek5000 .fld format using VisIt. > I am very new to using nek5000 code. > . I tried paraview too. It didn't work. > > Help greatly appreciated. The following message was posted in forum but > didn't find reply so had to post. > > error message > VisIt could not read from the file "C:\Users\s > pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowmach\lowMach_test0.f* > database". > > The generated error message was: > > There was an error opening C:\Users\s > pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowmach\lowMach_test0.f* > database. It may be an invalid file. > VisIt tried using the following file format readers to open the file: Silo > > Thank you, > > > Ravi Kiran Pendyala, > Graduate Research Assistant, > Department of Aerospace Engineering, > Mississippi State University, > Email: srp265 at msstate.edu > > > _______________________________________________ > Nek5000-users mailing listNek5000-users at lists.mcs.anl.govhttps://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > > _______________________________________________ > Nek5000-users mailing listNek5000-users at lists.mcs.anl.govhttps://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jun 2 07:22:55 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 2 Jun 2014 12:22:55 +0000 Subject: [Nek5000-users] question on subroutine sem2lex In-Reply-To: References: Message-ID: Hi Xianbei, It should be eg. However, note that it's really not as simple as this....You'll need to understand where your data resides, etc. I think this code example is quite dated and definitely not tested as it is not part of the standard source. Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Monday, June 02, 2014 12:46 AM To: Nek5000 Subject: [Nek5000-users] question on subroutine sem2lex Hi,all: In the parallel version of sem2lex, there is a part of code wrote as following: if (gllnid(eg).eq.nid) then ! element eg is on this processor eg = eg+1 le = gllel(ge) ! le is local element number do iz=1,nz1 do iy=1,ny1 do ix=1,nx1 However, ge doesn't appear anywhere except here,(le=gllel(ge)), so is this should be "le=gllel(eg)"? Or just my misunderstanding? Xianbei ?????????????? -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jun 2 08:05:07 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 2 Jun 2014 21:05:07 +0800 (CST) Subject: [Nek5000-users] question on subroutine sem2lex In-Reply-To: References: Message-ID: Hi,Paul: You are right. The code seems just out put the u in another ix,iy,iz,le way in spectral data, not what we expected as ix,iy,iz, where ix(max)=(nelx-1)*lx1+1. So is there any better way to output the data ready for the energy spectrum and two-point correlation already exists? Xianbei At 2014-06-02 08:22:55, nek5000-users at lists.mcs.anl.gov wrote: Hi Xianbei, It should be eg. However, note that it's really not as simple as this....You'll need to understand where your data resides, etc. I think this code example is quite dated and definitely not tested as it is not part of the standard source. Paul From:nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Monday, June 02, 2014 12:46 AM To: Nek5000 Subject: [Nek5000-users] question on subroutine sem2lex Hi,all: In the parallel version of sem2lex, there is a part of code wrote as following: if (gllnid(eg).eq.nid) then ! element eg is on this processor eg = eg+1 le = gllel(ge) ! le is local element number do iz=1,nz1 do iy=1,ny1 do ix=1,nx1 However, ge doesn't appear anywhere except here,(le=gllel(ge)), so is this should be "le=gllel(eg)"? Or just my misunderstanding? Xianbei ?????????????? -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jun 2 10:36:14 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 2 Jun 2014 08:36:14 -0700 Subject: [Nek5000-users] Reg: Visit In-Reply-To: References: <42328EFE-05CD-45EC-A746-BAD77726D5F7@msstate.edu> Message-ID: Hi Ravi, try visnek A <>.nek5000 file would be created. You would be able to read that from visit Tanmoy On Mon, Jun 2, 2014 at 2:09 AM, wrote: > Hi, > > I tried it. I still receive the same error though. > > Ravi Kiran Pendyala, > Graduate Research Assistant, > Department of Aerospace Engineering, > Mississippi State University, > Email: srp265 at msstate.edu > > > On Mon, Jun 2, 2014 at 3:38 AM, Msu wrote: > >> Thank you for the kind and quickest response. >> >> Thanks again, >> >> Ravi Kiran Pendyala, >> >> >> On Jun 2, 2014, at 3:38, nek5000-users at lists.mcs.anl.gov wrote: >> >> Hi, >> >> Create a separate file with ' .nek5000 ' has extension and write those >> lines in it and open it via Visit and It should work. >> >> Best Regards, >> Kamal >> >> On 02/06/2014 10:35, nek5000-users at lists.mcs.anl.gov wrote: >> >> No. I didn't not get a clue of working with metadata file. I read about >> it. Couldn't figure out how to create this. Is a a separate file or set of >> commands? >> >> Ravi Kiran Pendyala, >> >> >> On Jun 2, 2014, at 3:18, nek5000-users at lists.mcs.anl.gov wrote: >> >> Hi Ravi, >> >> Did you create a metadata file ?? A meta data file is the one which helps >> you to open a *.fld or *.f00000 file in visit >> >> It looks like this >> >> >> NEK5000 >> version: 1.0 >> filetemplate: divpipe%01d.f%05d >> firsttimestep: 1 >> numtimesteps: 09 >> >> Best regards, >> Kamal >> >> >> On 02/06/2014 09:57, nek5000-users at lists.mcs.anl.gov wrote: >> >> Hello all, >> >> I cannot view the output files from the nek5000 .fld format using >> VisIt. I am very new to using nek5000 code. >> . I tried paraview too. It didn't work. >> >> Help greatly appreciated. The following message was posted in forum but >> didn't find reply so had to post. >> >> error message >> VisIt could not read from the file "C:\Users\s >> pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowmach\lowMach_test0.f* >> database". >> >> The generated error message was: >> >> There was an error opening C:\Users\s >> pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowmach\lowMach_test0.f* >> database. It may be an invalid file. >> VisIt tried using the following file format readers to open the file: Silo >> >> Thank you, >> >> >> Ravi Kiran Pendyala, >> Graduate Research Assistant, >> Department of Aerospace Engineering, >> Mississippi State University, >> Email: srp265 at msstate.edu >> >> >> _______________________________________________ >> Nek5000-users mailing listNek5000-users at lists.mcs.anl.govhttps://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> >> >> >> _______________________________________________ >> Nek5000-users mailing listNek5000-users at lists.mcs.anl.govhttps://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> >> > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jun 2 11:13:58 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 2 Jun 2014 16:13:58 +0000 Subject: [Nek5000-users] question on subroutine sem2lex In-Reply-To: References: , Message-ID: Hi Xianbei, I would suggest checking out a stand-alone interpolation tool nek5_svn/trunk/tools/int_tp/README Best. Aleks ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Monday, June 02, 2014 8:05 AM To: Nek5000 Subject: Re: [Nek5000-users] question on subroutine sem2lex Hi,Paul: You are right. The code seems just out put the u in another ix,iy,iz,le way in spectral data, not what we expected as ix,iy,iz, where ix(max)=(nelx-1)*lx1+1. So is there any better way to output the data ready for the energy spectrum and two-point correlation already exists? Xianbei At 2014-06-02 08:22:55, nek5000-users at lists.mcs.anl.gov wrote: Hi Xianbei, It should be eg. However, note that it's really not as simple as this....You'll need to understand where your data resides, etc. I think this code example is quite dated and definitely not tested as it is not part of the standard source. Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Monday, June 02, 2014 12:46 AM To: Nek5000 Subject: [Nek5000-users] question on subroutine sem2lex Hi,all: In the parallel version of sem2lex, there is a part of code wrote as following: if (gllnid(eg).eq.nid) then ! element eg is on this processor eg = eg+1 le = gllel(ge) ! le is local element number do iz=1,nz1 do iy=1,ny1 do ix=1,nx1 However, ge doesn't appear anywhere except here,(le=gllel(ge)), so is this should be "le=gllel(eg)"? Or just my misunderstanding? Xianbei ?????????????? ?????????????? -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jun 2 11:42:25 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 02 Jun 2014 18:42:25 +0200 Subject: [Nek5000-users] help with meshing a torus Message-ID: Hi all, I'm trying to create a mesh for a torus (a doughnut). In order to do so I create the mesh for a straight pipe and then I bend it in usrdat2. If I assign periodic boundary conditions on the two faces of the straight pipe (that then coincide when I bend the pipe) everything works fine. If, instead, I assign E (as it should) nek stops after usrdat2 and complains about unique labels shared (I attached a log). Why? Best regards, Jacopo -------------- next part -------------- /----------------------------------------------------------\\ | _ __ ______ __ __ ______ ____ ____ ____ | | / | / // ____// //_/ / ____/ / __ \\ / __ \\ / __ \\ | | / |/ // __/ / ,< /___ \\ / / / // / / // / / / | | / /| // /___ / /| | ____/ / / /_/ // /_/ // /_/ / | | /_/ |_//_____//_/ |_|/_____/ \\____/ \\____/ \\____/ | | | |----------------------------------------------------------| | | | NEK5000: Open Source Spectral Element Solver | | COPYRIGHT (c) 2008-2010 UCHICAGO ARGONNE, LLC | | Version: 1.0rc1 / SVN r1016 | | Web: http://nek5000.mcs.anl.gov | | | \\----------------------------------------------------------/ Number of processors: 6 REAL wdsize : 8 INTEGER wdsize : 4 Beginning session: /afs/mech.kth.se/home/mech/jcanton/scratch/DNSs/tests/test3-fullTorus-myMesh/b timer accuracy: 1.1920929E-07 sec read .rea file read .re2 file byte swap: F 6.54321003 -2.93127722E+35 nelgt/nelgv/lelt: 48 48 640 lx1 /lx2 /lx3 : 8 8 8 mapping elements to processors 0 8 8 48 48 NELV 2 8 8 48 48 NELV 1 8 8 48 48 NELV 4 8 8 48 48 NELV 5 8 8 48 48 NELV 3 8 8 48 48 NELV RANK 0 IEG 25 26 27 37 38 39 41 42 element load imbalance: 0 8 8 done :: mapping elements to processors reading mesh reading curved sides reading bc for ifld 1 done :: read .re2 file 0 objects found done :: read .rea file 0.41709E-02 sec Reset the target Courant number to .5 setup mesh topology Right-handed check complete for 48 elements. OK. setvert3d: 8 7525 17893 7525 7525 call usrsetvert done :: usrsetvert gs_setup: 2526 unique labels shared pairwise times (avg, min, max): 8.15789e-06 7.98702e-06 8.32081e-06 crystal router : 1.40508e-05 1.34945e-05 1.44005e-05 all reduce : 2.36034e-05 2.35081e-05 2.36988e-05 used all_to_all method: pairwise handle bytes (avg, min, max): 36537.3 34204 38436 buffer bytes (avg, min, max): 15104 12640 17104 setupds time 1.6498E-02 seconds 0 8 7525 48 8 max multiplicity done :: setup mesh topology call usrdat Opening .rea.usr parameter file: /afs/mech.kth.se/home/mech/jcanton/scratch/DNSs/tests/test3-fullTorus-myMesh/bentPipe.rea.usr UPARAM( 1) = 0.0000 UPARAM( 2) = 200.00 UPARAM( 3) = 0.0000 UPARAM( 4) = 1.0000 UPARAM( 5) = 0.30000 UPARAM( 6) = 360.00 UPARAM( 7) = 22.500 done :: usrdat generate geometry data vol_t,vol_v: 0.78539821905070573 0.78539821905070573 done :: generate geometry data call usrdat2 writing hpts.in file done :: usrdat2 regenerate geometry data 1 vol_t,vol_v: 8.2246709170395587 8.2246709170395587 NOTE: All elements deformed , param(59) ^=0 done :: regenerate geometry data 1 verify mesh topology -2.1666666666666670 2.1666666666666670 Xrange -2.1666666666666670 2.1666666666666670 Yrange -0.50000000000000000 0.50000000000000000 Zrange done :: verify mesh topology 118 Parameters from file:/afs/mech.kth.se/home/mech/jcanton/scratch/DNSs/tests/test3-fullTorus-myMesh/bentPipe.rea 1 1.00000 P001: DENSITY 2 -10. P002: VISCOS 7 1.00000 P007: RHOCP 8 1.00000 P008: CONDUCT 11 3 P011: NSTEPS 12 5.0E-03 P012: DT 15 1 P015: IOSTEP 17 1.00000 P017: 18 0.500000E-01 P018: GRID < 0 --> # cells on screen 19 -1.00000 P019: INTYPE 20 10.0000 P020: NORDER 21 0.100000E-08 P021: DIVERGENCE 22 0.100000E-08 P022: HELMHOLTZ 24 0.100000E-01 P024: TOLREL 25 0.100000E-01 P025: TOLABS 26 1.00000 P026: COURANT/NTAU 27 3.00000 P027: TORDER 28 0.00000 P028: TORDER: mesh velocity (0: p28=p27) 56 1.00000 P056: : : 59 0.00000 P059: !=0 --> full Jac. eval. for each el. 65 1.00000 P065: #iofiles (eg, 0 or 64); <0 --> sep. dirs 66 6.00000 P066: output : <0=ascii, else binary 67 6.00000 P067: restart: <0=ascii, else binary 68 20000 P068: iastep: freq for avg_all (0=iostep) 69 50000.0 P069: : : frequency of srf dump 93 20.0000 P093: Number of previous pressure solns saved 94 9.00000 P094: start projecting velocity after p94 step 95 9.00000 P095: start projecting pressure after p95 step 99 3.00000 P099: dealiasing: <0--> off/3--> old/4--> new 102 1.00000 P102: Dump out divergence at each time step 103 0.01000 P103: weight of stabilizing filter (.01) IFTRAN = T IFFLOW = T IFHEAT = F IFSPLIT = T IFLOMACH = F IFUSERVP = F IFUSERMV = F IFSTRS = F IFCHAR = F IFCYCLIC = T IFAXIS = F IFMVBD = F IFMELT = F IFMODEL = F IFKEPS = F IFMOAB = F IFNEKNEK = F IFSYNC = T IFVCOR = T IFINTQ = F IFCWUZ = F IFSWALL = F IFGEOM = F IFSURT = F IFWCNO = F IFTMSH for field 1 = F IFADVC for field 1 = T IFNONL for field 1 = F Dealiasing enabled, lxd= 12 Estimated eigenvalues EIGAA = 3.6402682899481458 EIGGA = 109272.77145407666 EIGAE = 0.52560023437753967 EIGAS = 1.2032085561497324E-002 EIGGE = 109272.77145407666 EIGGS = 2.0000000000000000 verify mesh topology -2.1666666666666670 2.1666666666666670 Xrange -2.1666666666666670 2.1666666666666670 Yrange -0.50000000000000000 0.50000000000000000 Zrange done :: verify mesh topology E-solver strategy: 0 itr mg_nx: 1 3 7 mg_ny: 1 3 7 mg_nz: 1 3 7 call usrsetvert done :: usrsetvert gs_setup: 60 unique labels shared pairwise times (avg, min, max): 7.93139e-06 7.9155e-06 8.01086e-06 crystal router : 3.53654e-06 3.38554e-06 3.71933e-06 all reduce : 3.52065e-06 3.48091e-06 3.60012e-06 used all_to_all method: allreduce handle bytes (avg, min, max): 1902.67 1756 2028 buffer bytes (avg, min, max): 960 960 960 setupds time 7.7677E-04 seconds 1 2 85 48 setvert3d: 4 1189 1573 1189 1189 call usrsetvert done :: usrsetvert gs_setup: 482 unique labels shared pairwise times (avg, min, max): 5.97239e-06 5.6982e-06 6.10352e-06 crystal router : 5.74589e-06 5.6982e-06 5.79357e-06 all reduce : 9.81887e-06 9.5129e-06 1.01089e-05 used all_to_all method: crystal router handle bytes (avg, min, max): 25184 18812 28900 buffer bytes (avg, min, max): 5962.67 5344 6288 setupds time 1.3289E-03 seconds 2 4 1189 48 setvert3d: 4 1189 1573 1189 1189 call usrsetvert done :: usrsetvert gs_setup: 482 unique labels shared pairwise times (avg, min, max): 4.24385e-06 4.19617e-06 4.29153e-06 crystal router : 3.89814e-06 3.60012e-06 4.19617e-06 all reduce : 9.02017e-06 8.89301e-06 9.08375e-06 used all_to_all method: crystal router handle bytes (avg, min, max): 25184 18812 28900 buffer bytes (avg, min, max): 5962.67 5344 6288 setupds time 1.2860E-03 seconds 3 4 1189 48 setvert3d: 6 3669 6741 3669 3669 call usrsetvert done :: usrsetvert gs_setup: 1304 unique labels shared pairwise times (avg, min, max): 4.52201e-06 4.41074e-06 4.60148e-06 crystal router : 6.65188e-06 6.29425e-06 7.10487e-06 all reduce : 1.50323e-05 1.48058e-05 1.53065e-05 used all_to_all method: pairwise handle bytes (avg, min, max): 19598.7 18332 20628 buffer bytes (avg, min, max): 8149.33 6816 9200 setupds time 2.0061E-03 seconds 4 6 3669 48 Error in generalev, info= 7 6 -1 Error in generalev, info= 7 6 -1 Error in generalev, info= 7 6 -1 Matrix: 0 aa 6 6 6 0 aa 3.29462E+00 -1.92870E+00 0.00000E+00 0.00000E+00 0.00000E+00 0.00000E+00 Error in generalev, info= 12 6 -6 0 aa -1.92870E+00 3.42641E+00 -1.92870E+00 2.81394E-01 -6.58924E-02 0.00000E+00 0 aa 0.00000E+00 -1.92870E+00 3.29462E+00 -1.64731E+00 2.81394E-01 0.00000E+00 Error in generalev, info= 12 6 -6 0 aa 0.00000E+00 2.81394E-01 -1.64731E+00 3.29462E+00 -1.92870E+00 0.00000E+00 0 aa 0.00000E+00 -6.58924E-02 2.81394E-01 -1.92870E+00 Infinity -Infinity 0 aa 0.00000E+00 0.00000E+00 0.00000E+00 0.00000E+00 -Infinity Infinity Matrix: 0 bb 6 6 6 0 bb 1.05391E+00 0.00000E+00 0.00000E+00 0.00000E+00 0.00000E+00 0.00000E+00 0 bb 0.00000E+00 4.21563E-01 0.00000E+00 0.00000E+00 0.00000E+00 0.00000E+00 0 bb 0.00000E+00 0.00000E+00 1.05391E+00 0.00000E+00 0.00000E+00 0.00000E+00 0 bb 0.00000E+00 0.00000E+00 0.00000E+00 1.05391E+00 0.00000E+00 0.00000E+00 0 bb 0.00000E+00 0.00000E+00 0.00000E+00 0.00000E+00 2.10781E-01 0.00000E+00 0 bb 0.00000E+00 0.00000E+00 0.00000E+00 0.00000E+00 0.00000E+00 0.00000E+00 Matrix: 0 Aeig 6 6 6 0 Aeig 3.29462E+00 -1.92870E+00 0.00000E+00 0.00000E+00 0.00000E+00 0.00000E+00 0 Aeig -1.92870E+00 3.42641E+00 -1.92870E+00 2.81394E-01 -6.58924E-02 0.00000E+00 0 Aeig 0.00000E+00 -1.92870E+00 3.29462E+00 -1.64731E+00 2.81394E-01 0.00000E+00 0 Aeig 0.00000E+00 2.81394E-01 -1.64731E+00 3.29462E+00 -1.92870E+00 0.00000E+00 0 Aeig 0.00000E+00 -6.58924E-02 2.81394E-01 -1.92870E+00 Infinity -Infinity 0 Aeig 0.00000E+00 0.00000E+00 0.00000E+00 0.00000E+00 -Infinity Infinity Matrix: 0 Deig 1 6 6 0 Deig 2.81185E-01 1.10907E+00 2.47769E+00 3.98175E+00 1.00403E+01 1.11847E+01 Error in generalev, info= 12 6 -6 call exitt: dying ... backtrace(): obtained 12 stack frames. nek5000(print_stack_+0x1a) [0x509cfa] nek5000(exitt_+0x24b) [0x5cbcbb] nek5000(generalev_+0x172) [0x4a5d22] nek5000(hsmg_setup_fast1d_+0xfb) [0x4d038b] nek5000(hsmg_setup_fast_+0x5d7) [0x4d0a47] nek5000(hsmg_setup_fdm_+0x10d) [0x4d0d1d] nek5000(hsmg_setup_+0x3f) [0x4d1e1f] nek5000(set_overlap_+0x1ae) [0x4f5ffe] nek5000(nek_init_+0x82d) [0x421b0d] nek5000(main+0x24) [0x41e294] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xfd) [0x7f954e52bead] nek5000() [0x41e2d9] total elapsed time : 6.08048E-02 sec total solver time incl. I/O : 0.00000E+00 sec time/timestep : 0.00000E+00 sec CPU seconds/timestep/gridpt : 0.00000E+00 sec From nek5000-users at lists.mcs.anl.gov Mon Jun 2 12:43:02 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 2 Jun 2014 19:43:02 +0200 Subject: [Nek5000-users] Checking convergence to steady solution In-Reply-To: References: Message-ID: On Sat, May 31, 2014 at 9:22 PM, wrote: > call opsub2(uo,vo,wo,vx,vy,vz) > call normvc(H1,SEMI,L2,LINF,uo,vo,wo) > residu = L2/dt > call opcopy(uo,vo,wo,vx,vy,vz) > Thanks Kamal. This was also useful http://lists.mcs.anl.gov/pipermail/nek5000-users/2010-June/000681.html Best praveen -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jun 2 13:17:30 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 2 Jun 2014 18:17:30 +0000 Subject: [Nek5000-users] help with meshing a torus In-Reply-To: References: Message-ID: Jacopo, I would just use P bcs --- things will work fine. With E, you need to be careful about how the connectivity graph is generated (which is actually done by genmap). I've used your approach for tori in the past and it is ok. Paul ________________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Monday, June 02, 2014 11:42 AM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] help with meshing a torus Hi all, I'm trying to create a mesh for a torus (a doughnut). In order to do so I create the mesh for a straight pipe and then I bend it in usrdat2. If I assign periodic boundary conditions on the two faces of the straight pipe (that then coincide when I bend the pipe) everything works fine. If, instead, I assign E (as it should) nek stops after usrdat2 and complains about unique labels shared (I attached a log). Why? Best regards, Jacopo From nek5000-users at lists.mcs.anl.gov Mon Jun 2 13:39:20 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 2 Jun 2014 20:39:20 +0200 Subject: [Nek5000-users] help with meshing a torus In-Reply-To: References: Message-ID: Thanks Paul, I will follow your suggestion. Best regards, Jacopo On 2 Jun 2014, at 20:17, nek5000-users at lists.mcs.anl.gov wrote: > > Jacopo, > > I would just use P bcs --- things will work fine. > > With E, you need to be careful about how the connectivity graph > is generated (which is actually done by genmap). > > I've used your approach for tori in the past and it is ok. > > Paul > > ________________________________________ > From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > Sent: Monday, June 02, 2014 11:42 AM > To: nek5000-users at lists.mcs.anl.gov > Subject: [Nek5000-users] help with meshing a torus > > Hi all, > > I'm trying to create a mesh for a torus (a doughnut). > In order to do so I create the mesh for a straight pipe and then I bend > it in usrdat2. > > If I assign periodic boundary conditions on the two faces of the > straight pipe (that then coincide when I bend the pipe) everything works > fine. > If, instead, I assign E (as it should) nek stops after usrdat2 and > complains about unique labels shared (I attached a log). Why? > > > Best regards, > Jacopo > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Mon Jun 2 14:55:20 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 2 Jun 2014 14:55:20 -0500 Subject: [Nek5000-users] Reg: Visit In-Reply-To: References: <42328EFE-05CD-45EC-A746-BAD77726D5F7@msstate.edu> Message-ID: I have my nek5000 program on linux system. For post processing I take the data files on to my windows system where I have my VisIt tool. Is this problem for not being able to read the files. visnek also didn't help. I did this. start VisIt and use File->Open As? and then select Nek5000 reader as the reader to use to open the files. Thanks for your patience. ERROR: VisIt could not read from the file "C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowMach_test0.f00001.nek5000". The generated error message was: There was an error opening C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowMach_test0.f00001.nek5000. It may be an invalid file. VisIt tried using the following file format readers to open the file: Nek5000 The following error(s) may be helpful in identifying the problem: When attempting to use "Nek", the file matched the general format expected by the reader but eventually encountered this error: "Could not open file C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowMach_test0.f000010.f00001, which should exist according to header file C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowMach_test0.f00001.nek5000.". Ravi Kiran Pendyala, Graduate Research Assistant, Department of Aerospace Engineering, Mississippi State University, Email: srp265 at msstate.edu On Mon, Jun 2, 2014 at 10:36 AM, wrote: > Hi Ravi, > > try visnek > A <>.nek5000 file would be created. You would be able to read that from > visit > > Tanmoy > > > On Mon, Jun 2, 2014 at 2:09 AM, wrote: > >> Hi, >> >> I tried it. I still receive the same error though. >> >> Ravi Kiran Pendyala, >> Graduate Research Assistant, >> Department of Aerospace Engineering, >> Mississippi State University, >> Email: srp265 at msstate.edu >> >> >> On Mon, Jun 2, 2014 at 3:38 AM, Msu wrote: >> >>> Thank you for the kind and quickest response. >>> >>> Thanks again, >>> >>> Ravi Kiran Pendyala, >>> >>> >>> On Jun 2, 2014, at 3:38, nek5000-users at lists.mcs.anl.gov wrote: >>> >>> Hi, >>> >>> Create a separate file with ' .nek5000 ' has extension and write those >>> lines in it and open it via Visit and It should work. >>> >>> Best Regards, >>> Kamal >>> >>> On 02/06/2014 10:35, nek5000-users at lists.mcs.anl.gov wrote: >>> >>> No. I didn't not get a clue of working with metadata file. I read about >>> it. Couldn't figure out how to create this. Is a a separate file or set of >>> commands? >>> >>> Ravi Kiran Pendyala, >>> >>> >>> On Jun 2, 2014, at 3:18, nek5000-users at lists.mcs.anl.gov wrote: >>> >>> Hi Ravi, >>> >>> Did you create a metadata file ?? A meta data file is the one which >>> helps you to open a *.fld or *.f00000 file in visit >>> >>> It looks like this >>> >>> >>> NEK5000 >>> version: 1.0 >>> filetemplate: divpipe%01d.f%05d >>> firsttimestep: 1 >>> numtimesteps: 09 >>> >>> Best regards, >>> Kamal >>> >>> >>> On 02/06/2014 09:57, nek5000-users at lists.mcs.anl.gov wrote: >>> >>> Hello all, >>> >>> I cannot view the output files from the nek5000 .fld format using >>> VisIt. I am very new to using nek5000 code. >>> . I tried paraview too. It didn't work. >>> >>> Help greatly appreciated. The following message was posted in forum >>> but didn't find reply so had to post. >>> >>> error message >>> VisIt could not read from the file "C:\Users\s >>> pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowmach\lowMach_test0.f* >>> database". >>> >>> The generated error message was: >>> >>> There was an error opening C:\Users\s >>> pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowmach\lowMach_test0.f* >>> database. It may be an invalid file. >>> VisIt tried using the following file format readers to open the file: >>> Silo >>> >>> Thank you, >>> >>> >>> Ravi Kiran Pendyala, >>> Graduate Research Assistant, >>> Department of Aerospace Engineering, >>> Mississippi State University, >>> Email: srp265 at msstate.edu >>> >>> >>> _______________________________________________ >>> Nek5000-users mailing listNek5000-users at lists.mcs.anl.govhttps://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>> >>> >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>> >>> >>> >>> _______________________________________________ >>> Nek5000-users mailing listNek5000-users at lists.mcs.anl.govhttps://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>> >>> >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>> >>> >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> >> > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jun 2 15:15:32 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 2 Jun 2014 20:15:32 +0000 Subject: [Nek5000-users] Reg: Visit In-Reply-To: References: <42328EFE-05CD-45EC-A746-BAD77726D5F7@msstate.edu> , Message-ID: Hi Ravi and Tanmoy, Actually you need to provide a case name for visnek script since it creates the following template echo 'filetemplate: '$base'%01d.f%05d' > $base.nek5000 Thus you should try visnek lowMach_test and not 'visnek lowMach_test0.f00001' (ANother alternative, before running nek with scripts tools/scripts/nek*, delete 'rm SESSION.NAME' from them and just type visnek so it can look up for the case name in the SESSION.NAME file) Aleks ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Monday, June 02, 2014 2:55 PM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Reg: Visit I have my nek5000 program on linux system. For post processing I take the data files on to my windows system where I have my VisIt tool. Is this problem for not being able to read the files. visnek also didn't help. I did this. start VisIt and use File->Open As? and then select Nek5000 reader as the reader to use to open the files. Thanks for your patience. ERROR: VisIt could not read from the file "C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowMach_test0.f00001.nek5000". The generated error message was: There was an error opening C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowMach_test0.f00001.nek5000. It may be an invalid file. VisIt tried using the following file format readers to open the file: Nek5000 The following error(s) may be helpful in identifying the problem: When attempting to use "Nek", the file matched the general format expected by the reader but eventually encountered this error: "Could not open file C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowMach_test0.f000010.f00001, which should exist according to header file C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowMach_test0.f00001.nek5000.". Ravi Kiran Pendyala, Graduate Research Assistant, Department of Aerospace Engineering, Mississippi State University, Email: srp265 at msstate.edu On Mon, Jun 2, 2014 at 10:36 AM, > wrote: Hi Ravi, try visnek A <>.nek5000 file would be created. You would be able to read that from visit Tanmoy On Mon, Jun 2, 2014 at 2:09 AM, > wrote: Hi, I tried it. I still receive the same error though. Ravi Kiran Pendyala, Graduate Research Assistant, Department of Aerospace Engineering, Mississippi State University, Email: srp265 at msstate.edu On Mon, Jun 2, 2014 at 3:38 AM, Msu > wrote: Thank you for the kind and quickest response. Thanks again, Ravi Kiran Pendyala, On Jun 2, 2014, at 3:38, nek5000-users at lists.mcs.anl.gov wrote: Hi, Create a separate file with ' .nek5000 ' has extension and write those lines in it and open it via Visit and It should work. Best Regards, Kamal On 02/06/2014 10:35, nek5000-users at lists.mcs.anl.gov wrote: No. I didn't not get a clue of working with metadata file. I read about it. Couldn't figure out how to create this. Is a a separate file or set of commands? Ravi Kiran Pendyala, On Jun 2, 2014, at 3:18, nek5000-users at lists.mcs.anl.gov wrote: Hi Ravi, Did you create a metadata file ?? A meta data file is the one which helps you to open a *.fld or *.f00000 file in visit It looks like this NEK5000 version: 1.0 filetemplate: divpipe%01d.f%05d firsttimestep: 1 numtimesteps: 09 Best regards, Kamal On 02/06/2014 09:57, nek5000-users at lists.mcs.anl.gov wrote: Hello all, I cannot view the output files from the nek5000 .fld format using VisIt. I am very new to using nek5000 code. . I tried paraview too. It didn't work. Help greatly appreciated. The following message was posted in forum but didn't find reply so had to post. error message VisIt could not read from the file "C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowmach\lowMach_test0.f* database". The generated error message was: There was an error opening C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowmach\lowMach_test0.f* database. It may be an invalid file. VisIt tried using the following file format readers to open the file: Silo Thank you, Ravi Kiran Pendyala, Graduate Research Assistant, Department of Aerospace Engineering, Mississippi State University, Email: srp265 at msstate.edu _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jun 2 18:21:45 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 2 Jun 2014 18:21:45 -0500 Subject: [Nek5000-users] Reg: Visit In-Reply-To: References: <42328EFE-05CD-45EC-A746-BAD77726D5F7@msstate.edu> Message-ID: I get error even now. I modified the way you suggested, but still I get error. I typed 'visnek lowMach_test'. I get below message in my terminal. Also one may need to correct for an endian by inserting the first line "endian big" or "endian little" in case of, e.g., files transfered from other systems Total 10 file(s) are in the generated file lowMach_test.nek5000 ... Done! But when I try to view the files I get the error again. Ravi Kiran Pendyala, Graduate Research Assistant, Department of Aerospace Engineering, Mississippi State University, Email: srp265 at msstate.edu On Mon, Jun 2, 2014 at 3:15 PM, wrote: > Hi Ravi and Tanmoy, > > Actually you need to provide a case name for visnek script since it > creates the following template > > echo 'filetemplate: '$base'%01d.f%05d' > $base.nek5000 > > Thus you should try > > visnek lowMach_test > > and not 'visnek lowMach_test0.f00001' > > (ANother alternative, before running nek with scripts tools/scripts/nek*, > delete 'rm SESSION.NAME' from them and just type visnek so it can look up > for the case name in the SESSION.NAME file) > > Aleks > > > > > > > ------------------------------ > *From:* nek5000-users-bounces at lists.mcs.anl.gov [ > nek5000-users-bounces at lists.mcs.anl.gov] on behalf of > nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > *Sent:* Monday, June 02, 2014 2:55 PM > *To:* nek5000-users at lists.mcs.anl.gov > *Subject:* Re: [Nek5000-users] Reg: Visit > > I have my nek5000 program on linux system. For post processing I take > the data files on to my windows system where I have my VisIt tool. Is this > problem for not being able to read the files. visnek also didn't help. I > did this. start VisIt and use File->Open As? and then select Nek5000 reader > as the reader to use to open the files. Thanks for your patience. > > ERROR: > > > > VisIt could not read from the file "C:\Users\s > pendyala\AppData\Local\Programs\LLNL\VisIt > 2.7.2\lowMach_test0.f00001.nek5000". > > > The generated error message was: > > > There was an error opening C:\Users\s > pendyala\AppData\Local\Programs\LLNL\VisIt > 2.7.2\lowMach_test0.f00001.nek5000. It may be an invalid file. VisIt tried > using the following file format readers to open the file: Nek5000 > > > The following error(s) may be helpful in identifying the problem: > > When attempting to use "Nek", the file matched the general format expected > by the reader but eventually encountered this error: "Could not open file > C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt > 2.7.2\lowMach_test0.f000010.f00001, which should exist according to header > file C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt > 2.7.2\lowMach_test0.f00001.nek5000.". > > > > Ravi Kiran Pendyala, > Graduate Research Assistant, > Department of Aerospace Engineering, > Mississippi State University, > Email: srp265 at msstate.edu > > > On Mon, Jun 2, 2014 at 10:36 AM, wrote: > >> Hi Ravi, >> >> try visnek >> A <>.nek5000 file would be created. You would be able to read that from >> visit >> >> Tanmoy >> >> >> On Mon, Jun 2, 2014 at 2:09 AM, wrote: >> >>> Hi, >>> >>> I tried it. I still receive the same error though. >>> >>> Ravi Kiran Pendyala, >>> Graduate Research Assistant, >>> Department of Aerospace Engineering, >>> Mississippi State University, >>> Email: srp265 at msstate.edu >>> >>> >>> On Mon, Jun 2, 2014 at 3:38 AM, Msu wrote: >>> >>>> Thank you for the kind and quickest response. >>>> >>>> Thanks again, >>>> >>>> Ravi Kiran Pendyala, >>>> >>>> >>>> On Jun 2, 2014, at 3:38, nek5000-users at lists.mcs.anl.gov wrote: >>>> >>>> Hi, >>>> >>>> Create a separate file with ' .nek5000 ' has extension and write those >>>> lines in it and open it via Visit and It should work. >>>> >>>> Best Regards, >>>> Kamal >>>> >>>> On 02/06/2014 10:35, nek5000-users at lists.mcs.anl.gov wrote: >>>> >>>> No. I didn't not get a clue of working with metadata file. I read about >>>> it. Couldn't figure out how to create this. Is a a separate file or set of >>>> commands? >>>> >>>> Ravi Kiran Pendyala, >>>> >>>> >>>> On Jun 2, 2014, at 3:18, nek5000-users at lists.mcs.anl.gov wrote: >>>> >>>> Hi Ravi, >>>> >>>> Did you create a metadata file ?? A meta data file is the one which >>>> helps you to open a *.fld or *.f00000 file in visit >>>> >>>> It looks like this >>>> >>>> >>>> NEK5000 >>>> version: 1.0 >>>> filetemplate: divpipe%01d.f%05d >>>> firsttimestep: 1 >>>> numtimesteps: 09 >>>> >>>> Best regards, >>>> Kamal >>>> >>>> >>>> On 02/06/2014 09:57, nek5000-users at lists.mcs.anl.gov wrote: >>>> >>>> Hello all, >>>> >>>> I cannot view the output files from the nek5000 .fld format using >>>> VisIt. I am very new to using nek5000 code. >>>> . I tried paraview too. It didn't work. >>>> >>>> Help greatly appreciated. The following message was posted in forum >>>> but didn't find reply so had to post. >>>> >>>> error message >>>> VisIt could not read from the file "C:\Users\s >>>> pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowmach\lowMach_test0.f* >>>> database". >>>> >>>> The generated error message was: >>>> >>>> There was an error opening C:\Users\s >>>> pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowmach\lowMach_test0.f* >>>> database. It may be an invalid file. >>>> VisIt tried using the following file format readers to open the file: >>>> Silo >>>> >>>> Thank you, >>>> >>>> >>>> Ravi Kiran Pendyala, >>>> Graduate Research Assistant, >>>> Department of Aerospace Engineering, >>>> Mississippi State University, >>>> Email: srp265 at msstate.edu >>>> >>>> >>>> _______________________________________________ >>>> Nek5000-users mailing listNek5000-users at lists.mcs.anl.govhttps://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>>> >>>> >>>> _______________________________________________ >>>> Nek5000-users mailing list >>>> Nek5000-users at lists.mcs.anl.gov >>>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>>> >>>> >>>> >>>> _______________________________________________ >>>> Nek5000-users mailing listNek5000-users at lists.mcs.anl.govhttps://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>>> >>>> >>>> _______________________________________________ >>>> Nek5000-users mailing list >>>> Nek5000-users at lists.mcs.anl.gov >>>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>>> >>>> >>> >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>> >>> >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> >> > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jun 2 19:13:05 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 3 Jun 2014 00:13:05 +0000 Subject: [Nek5000-users] Reg: Visit In-Reply-To: References: <42328EFE-05CD-45EC-A746-BAD77726D5F7@msstate.edu> , Message-ID: Hi Ravi, What error are you getting? It should not be the same error you reported earlier: VisIt could not read from the file "C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowMach_test0.f00001.nek5000". since you are presumably opening lowMach_test.nek5000 instead, right? Aleks ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Monday, June 02, 2014 6:21 PM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Reg: Visit I get error even now. I modified the way you suggested, but still I get error. I typed 'visnek lowMach_test'. I get below message in my terminal. Also one may need to correct for an endian by inserting the first line "endian big" or "endian little" in case of, e.g., files transfered from other systems Total 10 file(s) are in the generated file lowMach_test.nek5000 ... Done! But when I try to view the files I get the error again. Ravi Kiran Pendyala, Graduate Research Assistant, Department of Aerospace Engineering, Mississippi State University, Email: srp265 at msstate.edu On Mon, Jun 2, 2014 at 3:15 PM, > wrote: Hi Ravi and Tanmoy, Actually you need to provide a case name for visnek script since it creates the following template echo 'filetemplate: '$base'%01d.f%05d' > $base.nek5000 Thus you should try visnek lowMach_test and not 'visnek lowMach_test0.f00001' (ANother alternative, before running nek with scripts tools/scripts/nek*, delete 'rm SESSION.NAME' from them and just type visnek so it can look up for the case name in the SESSION.NAME file) Aleks ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Monday, June 02, 2014 2:55 PM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Reg: Visit I have my nek5000 program on linux system. For post processing I take the data files on to my windows system where I have my VisIt tool. Is this problem for not being able to read the files. visnek also didn't help. I did this. start VisIt and use File->Open As? and then select Nek5000 reader as the reader to use to open the files. Thanks for your patience. ERROR: VisIt could not read from the file "C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowMach_test0.f00001.nek5000". The generated error message was: There was an error opening C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowMach_test0.f00001.nek5000. It may be an invalid file. VisIt tried using the following file format readers to open the file: Nek5000 The following error(s) may be helpful in identifying the problem: When attempting to use "Nek", the file matched the general format expected by the reader but eventually encountered this error: "Could not open file C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowMach_test0.f000010.f00001, which should exist according to header file C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowMach_test0.f00001.nek5000.". Ravi Kiran Pendyala, Graduate Research Assistant, Department of Aerospace Engineering, Mississippi State University, Email: srp265 at msstate.edu On Mon, Jun 2, 2014 at 10:36 AM, > wrote: Hi Ravi, try visnek A <>.nek5000 file would be created. You would be able to read that from visit Tanmoy On Mon, Jun 2, 2014 at 2:09 AM, > wrote: Hi, I tried it. I still receive the same error though. Ravi Kiran Pendyala, Graduate Research Assistant, Department of Aerospace Engineering, Mississippi State University, Email: srp265 at msstate.edu On Mon, Jun 2, 2014 at 3:38 AM, Msu > wrote: Thank you for the kind and quickest response. Thanks again, Ravi Kiran Pendyala, On Jun 2, 2014, at 3:38, nek5000-users at lists.mcs.anl.gov wrote: Hi, Create a separate file with ' .nek5000 ' has extension and write those lines in it and open it via Visit and It should work. Best Regards, Kamal On 02/06/2014 10:35, nek5000-users at lists.mcs.anl.gov wrote: No. I didn't not get a clue of working with metadata file. I read about it. Couldn't figure out how to create this. Is a a separate file or set of commands? Ravi Kiran Pendyala, On Jun 2, 2014, at 3:18, nek5000-users at lists.mcs.anl.gov wrote: Hi Ravi, Did you create a metadata file ?? A meta data file is the one which helps you to open a *.fld or *.f00000 file in visit It looks like this NEK5000 version: 1.0 filetemplate: divpipe%01d.f%05d firsttimestep: 1 numtimesteps: 09 Best regards, Kamal On 02/06/2014 09:57, nek5000-users at lists.mcs.anl.gov wrote: Hello all, I cannot view the output files from the nek5000 .fld format using VisIt. I am very new to using nek5000 code. . I tried paraview too. It didn't work. Help greatly appreciated. The following message was posted in forum but didn't find reply so had to post. error message VisIt could not read from the file "C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowmach\lowMach_test0.f* database". The generated error message was: There was an error opening C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowmach\lowMach_test0.f* database. It may be an invalid file. VisIt tried using the following file format readers to open the file: Silo Thank you, Ravi Kiran Pendyala, Graduate Research Assistant, Department of Aerospace Engineering, Mississippi State University, Email: srp265 at msstate.edu _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jun 2 19:28:39 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 2 Jun 2014 19:28:39 -0500 Subject: [Nek5000-users] [PossibleSpam] Re: Reg: Visit In-Reply-To: References: <42328EFE-05CD-45EC-A746-BAD77726D5F7@msstate.edu> Message-ID: Hi Aleks, The error is different apparently. Following is error: VisIt could not read from the file "C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowMach_test.nek5000". The generated error message was: There was an error opening C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowMach_test.nek5000. It may be an invalid file. VisIt tried using the following file format readers to open the file: Nek5000 Thanks, Ravi Kiran Pendyala, On Mon, Jun 2, 2014 at 7:13 PM, wrote: > Hi Ravi, > > What error are you getting? It should not be the same error you reported > earlier: > > > VisIt could not read from the file "C:\Users\s > pendyala\AppData\Local\Programs\LLNL\VisIt > 2.7.2\lowMach_test0.f00001.nek5000". > > since you are presumably opening lowMach_test.nek5000 instead, right? > > Aleks > > ------------------------------ > *From:* nek5000-users-bounces at lists.mcs.anl.gov [ > nek5000-users-bounces at lists.mcs.anl.gov] on behalf of > nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > *Sent:* Monday, June 02, 2014 6:21 PM > > *To:* nek5000-users at lists.mcs.anl.gov > *Subject:* Re: [Nek5000-users] Reg: Visit > > I get error even now. I modified the way you suggested, but still I > get error. I typed 'visnek lowMach_test'. I get below message in my > terminal. > > Also one may need to correct for an endian by inserting the first line > "endian big" or "endian little" in case of, e.g., files transfered from > other systems > > > Total 10 file(s) are in the generated file lowMach_test.nek5000 ... Done! > > But when I try to view the files > > > I get the error again. > > Ravi Kiran Pendyala, > Graduate Research Assistant, > Department of Aerospace Engineering, > Mississippi State University, > Email: srp265 at msstate.edu > > > On Mon, Jun 2, 2014 at 3:15 PM, wrote: > >> Hi Ravi and Tanmoy, >> >> Actually you need to provide a case name for visnek script since it >> creates the following template >> >> echo 'filetemplate: '$base'%01d.f%05d' > $base.nek5000 >> >> Thus you should try >> >> visnek lowMach_test >> >> and not 'visnek lowMach_test0.f00001' >> >> (ANother alternative, before running nek with scripts tools/scripts/nek*, >> delete 'rm SESSION.NAME' from them and just type visnek so it can look >> up for the case name in the SESSION.NAME file) >> >> Aleks >> >> >> >> >> >> >> ------------------------------ >> *From:* nek5000-users-bounces at lists.mcs.anl.gov [ >> nek5000-users-bounces at lists.mcs.anl.gov] on behalf of >> nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] >> *Sent:* Monday, June 02, 2014 2:55 PM >> *To:* nek5000-users at lists.mcs.anl.gov >> *Subject:* Re: [Nek5000-users] Reg: Visit >> >> I have my nek5000 program on linux system. For post processing I take >> the data files on to my windows system where I have my VisIt tool. Is this >> problem for not being able to read the files. visnek also didn't help. I >> did this. start VisIt and use File->Open As? and then select Nek5000 reader >> as the reader to use to open the files. Thanks for your patience. >> >> ERROR: >> >> >> >> VisIt could not read from the file "C:\Users\s >> pendyala\AppData\Local\Programs\LLNL\VisIt >> 2.7.2\lowMach_test0.f00001.nek5000". >> >> >> The generated error message was: >> >> >> There was an error opening C:\Users\s >> pendyala\AppData\Local\Programs\LLNL\VisIt >> 2.7.2\lowMach_test0.f00001.nek5000. It may be an invalid file. VisIt tried >> using the following file format readers to open the file: Nek5000 >> >> >> The following error(s) may be helpful in identifying the problem: >> >> When attempting to use "Nek", the file matched the general format >> expected by the reader but eventually encountered this error: "Could not >> open file C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt >> 2.7.2\lowMach_test0.f000010.f00001, which should exist according to header >> file C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt >> 2.7.2\lowMach_test0.f00001.nek5000.". >> >> >> >> Ravi Kiran Pendyala, >> Graduate Research Assistant, >> Department of Aerospace Engineering, >> Mississippi State University, >> Email: srp265 at msstate.edu >> >> >> On Mon, Jun 2, 2014 at 10:36 AM, wrote: >> >>> Hi Ravi, >>> >>> try visnek >>> A <>.nek5000 file would be created. You would be able to read that from >>> visit >>> >>> Tanmoy >>> >>> >>> On Mon, Jun 2, 2014 at 2:09 AM, wrote: >>> >>>> Hi, >>>> >>>> I tried it. I still receive the same error though. >>>> >>>> Ravi Kiran Pendyala, >>>> Graduate Research Assistant, >>>> Department of Aerospace Engineering, >>>> Mississippi State University, >>>> Email: srp265 at msstate.edu >>>> >>>> >>>> On Mon, Jun 2, 2014 at 3:38 AM, Msu wrote: >>>> >>>>> Thank you for the kind and quickest response. >>>>> >>>>> Thanks again, >>>>> >>>>> Ravi Kiran Pendyala, >>>>> >>>>> >>>>> On Jun 2, 2014, at 3:38, nek5000-users at lists.mcs.anl.gov wrote: >>>>> >>>>> Hi, >>>>> >>>>> Create a separate file with ' .nek5000 ' has extension and write those >>>>> lines in it and open it via Visit and It should work. >>>>> >>>>> Best Regards, >>>>> Kamal >>>>> >>>>> On 02/06/2014 10:35, nek5000-users at lists.mcs.anl.gov wrote: >>>>> >>>>> No. I didn't not get a clue of working with metadata file. I read >>>>> about it. Couldn't figure out how to create this. Is a a separate file or >>>>> set of commands? >>>>> >>>>> Ravi Kiran Pendyala, >>>>> >>>>> >>>>> On Jun 2, 2014, at 3:18, nek5000-users at lists.mcs.anl.gov wrote: >>>>> >>>>> Hi Ravi, >>>>> >>>>> Did you create a metadata file ?? A meta data file is the one which >>>>> helps you to open a *.fld or *.f00000 file in visit >>>>> >>>>> It looks like this >>>>> >>>>> >>>>> NEK5000 >>>>> version: 1.0 >>>>> filetemplate: divpipe%01d.f%05d >>>>> firsttimestep: 1 >>>>> numtimesteps: 09 >>>>> >>>>> Best regards, >>>>> Kamal >>>>> >>>>> >>>>> On 02/06/2014 09:57, nek5000-users at lists.mcs.anl.gov wrote: >>>>> >>>>> Hello all, >>>>> >>>>> I cannot view the output files from the nek5000 .fld format using >>>>> VisIt. I am very new to using nek5000 code. >>>>> . I tried paraview too. It didn't work. >>>>> >>>>> Help greatly appreciated. The following message was posted in forum >>>>> but didn't find reply so had to post. >>>>> >>>>> error message >>>>> VisIt could not read from the file "C:\Users\s >>>>> pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowmach\lowMach_test0.f* >>>>> database". >>>>> >>>>> The generated error message was: >>>>> >>>>> There was an error opening C:\Users\s >>>>> pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowmach\lowMach_test0.f* >>>>> database. It may be an invalid file. >>>>> VisIt tried using the following file format readers to open the file: >>>>> Silo >>>>> >>>>> Thank you, >>>>> >>>>> >>>>> Ravi Kiran Pendyala, >>>>> Graduate Research Assistant, >>>>> Department of Aerospace Engineering, >>>>> Mississippi State University, >>>>> Email: srp265 at msstate.edu >>>>> >>>>> >>>>> _______________________________________________ >>>>> Nek5000-users mailing listNek5000-users at lists.mcs.anl.govhttps://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>>>> >>>>> >>>>> _______________________________________________ >>>>> Nek5000-users mailing list >>>>> Nek5000-users at lists.mcs.anl.gov >>>>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>>>> >>>>> >>>>> >>>>> _______________________________________________ >>>>> Nek5000-users mailing listNek5000-users at lists.mcs.anl.govhttps://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>>>> >>>>> >>>>> _______________________________________________ >>>>> Nek5000-users mailing list >>>>> Nek5000-users at lists.mcs.anl.gov >>>>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>>>> >>>>> >>>> >>>> _______________________________________________ >>>> Nek5000-users mailing list >>>> Nek5000-users at lists.mcs.anl.gov >>>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>>> >>>> >>> >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>> >>> >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> >> > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jun 2 19:57:30 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 3 Jun 2014 08:57:30 +0800 (CST) Subject: [Nek5000-users] question on subroutine sem2lex In-Reply-To: References: , Message-ID: Hi,Aleks: Thank you for your suggestion. Xianbei At 2014-06-03 00:13:58, nek5000-users at lists.mcs.anl.gov wrote: Hi Xianbei, I would suggest checking out a stand-alone interpolation tool nek5_svn/trunk/tools/int_tp/README Best. Aleks From:nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Monday, June 02, 2014 8:05 AM To: Nek5000 Subject: Re: [Nek5000-users] question on subroutine sem2lex Hi,Paul: You are right. The code seems just out put the u in another ix,iy,iz,le way in spectral data, not what we expected as ix,iy,iz, where ix(max)=(nelx-1)*lx1+1. So is there any better way to output the data ready for the energy spectrum and two-point correlation already exists? Xianbei At 2014-06-02 08:22:55, nek5000-users at lists.mcs.anl.gov wrote: Hi Xianbei, It should be eg. However, note that it's really not as simple as this....You'll need to understand where your data resides, etc. I think this code example is quite dated and definitely not tested as it is not part of the standard source. Paul From:nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Monday, June 02, 2014 12:46 AM To: Nek5000 Subject: [Nek5000-users] question on subroutine sem2lex Hi,all: In the parallel version of sem2lex, there is a part of code wrote as following: if (gllnid(eg).eq.nid) then ! element eg is on this processor eg = eg+1 le = gllel(ge) ! le is local element number do iz=1,nz1 do iy=1,ny1 do ix=1,nx1 However, ge doesn't appear anywhere except here,(le=gllel(ge)), so is this should be "le=gllel(eg)"? Or just my misunderstanding? Xianbei ?????????????? ?????????????? -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Jun 3 02:52:19 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 3 Jun 2014 07:52:19 +0000 Subject: [Nek5000-users] size of arrays and declaration of variables Message-ID: Hi Nek team, I have a question concerning the size of arrays. I took the routine convab for example. TA, such as T, BQ or VTRANS, have a size of lt=lx1*ly1*lz1*lelt. So why in the call of col2 or subcol3 the parameter n, which should be the size of the arrays cited above, is actually ntot=nx1*ny1*nz1*nelfld(ifield) ? 1) I guess that there is a reason for that, but I don?t understand this mismatch of size of arrays. Moreover, ntot refers to the number of nodes on a CPU and LT refers to the total number of node in the full domain, right? 2) I?m not expert in F77 but could you confirm me that there is no difference between the declaration: TA (LX1,LY1,LZ1,LELT) and TA(LT) with LT=LX1*LY1*LZ1*LELT ? I mean, an argument such as TA(1,1,1,1) will pass the whole array of TA ? Thank you ! subroutine convab C--------------------------------------------------------------- C C Eulerian scheme, add convection term to forcing function C at current time step. C C--------------------------------------------------------------- include 'SIZE' include 'SOLN' include 'MASS' include ?TSTEP' COMMON /SCRUZ/ TA (LX1,LY1,LZ1,LELT) C NEL = NELFLD(IFIELD) NTOT1 = NX1*NY1*NZ1*NEL CALL CONVOP (TA,T(1,1,1,1,IFIELD-1)) CALL COL2 (TA,VTRANS(1,1,1,1,IFIELD),NTOT1) CALL SUBCOL3 (BQ(1,1,1,1,IFIELD-1),BM1,TA,NTOT1) Best regards, Emmanuel -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Jun 3 03:51:11 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 3 Jun 2014 08:51:11 +0000 Subject: [Nek5000-users] size of arrays and declaration of variables In-Reply-To: References: Message-ID: Hi Emmanuel, f77 passes arrays by address -- i.e., it passes a pointer to the element of the array listed, or to the first one if no array index is indicated in the call. There is no concept of passing a whole array or just part of one --- you simply pass the pointer to the first element of the array, e.g., as in "call blah(ta)" or to some other element of the array "call blah(ta(1,1,1,e))" which, in this case, would pass the pointer to the e-th element of ta. Moreover, in f77, the declaration real x(3,4) implies that x(2,k) comes immediately after x(1,k) in memory (whereas x(k,3) is _not_ next to x(k,2).) Common usage in Nek is therefore to view the block x(1,1,1,e),x(2,1,1,e),...,x(lx1,ly1,lz1,e) as an "element" All of these variables are adjacent in memory, assuming that the array index sizes are (lx1,ly1,lz1) for the first three indices. Given that they are adjacent, we can pass one element at a time to a routine (but really, we're just passing a pointer to the "e"th block) via integer e do e=1,nelv call blah(x(1,1,1,e)) enddo In a case where we operate on an entire field, i.e., all elements, it suffices to just pass the pointer to the whole array, as in: n=nx1*ny1*nz1*nelv call rzero(x,n) Note that it's critical that each element be completely full - i.e., that we use all the memory locations in the x(i,j,k) locacations. That way, we are always accessing adjacent memory locations and have unit-stride addressing (see, e.g., Deville,Fischer,Mund chapter 8 or google the topic). However, we _don't_ have to fill up all the elements. If we want to declare 10 elements and use only the first 5, that's ok (though it takes more memory, which may or may not be an issue). With this approach we have the flexibility of running the same executable with different processor counts. Consider the following scenario: We have nelg=80 elements in a mesh and we declare lelt=10. We can run on: 8 processors, lelt=10, nelt=10 16 processors, lelt=10, nelt= 5 32 processors, lelt=10, nelt= 2 or 3 etc. Note that, in the 32 processor case, not all processors have the same value of nelt. However, they must have the same value of lelt because they are running the same executable and nek uses static (i.e., declared at compile-time) memory allocation. Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Tuesday, June 03, 2014 2:52 AM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] size of arrays and declaration of variables Hi Nek team, I have a question concerning the size of arrays. I took the routine convab for example. TA, such as T, BQ or VTRANS, have a size of lt=lx1*ly1*lz1*lelt. So why in the call of col2 or subcol3 the parameter n, which should be the size of the arrays cited above, is actually ntot=nx1*ny1*nz1*nelfld(ifield) ? 1) I guess that there is a reason for that, but I don?t understand this mismatch of size of arrays. Moreover, ntot refers to the number of nodes on a CPU and LT refers to the total number of node in the full domain, right? 2) I?m not expert in F77 but could you confirm me that there is no difference between the declaration: TA (LX1,LY1,LZ1,LELT) and TA(LT) with LT=LX1*LY1*LZ1*LELT ? I mean, an argument such as TA(1,1,1,1) will pass the whole array of TA ? Thank you ! subroutine convab C--------------------------------------------------------------- C C Eulerian scheme, add convection term to forcing function C at current time step. C C--------------------------------------------------------------- include 'SIZE' include 'SOLN' include 'MASS' include ?TSTEP' COMMON /SCRUZ/ TA (LX1,LY1,LZ1,LELT) C NEL = NELFLD(IFIELD) NTOT1 = NX1*NY1*NZ1*NEL CALL CONVOP (TA,T(1,1,1,1,IFIELD-1)) CALL COL2 (TA,VTRANS(1,1,1,1,IFIELD),NTOT1) CALL SUBCOL3 (BQ(1,1,1,1,IFIELD-1),BM1,TA,NTOT1) Best regards, Emmanuel -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Jun 3 04:08:38 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 03 Jun 2014 11:08:38 +0200 Subject: [Nek5000-users] Pn-pn formulation Message-ID: Hi Neks, I found that in the turbulence channel example, (Pn-Pn) formulation is used instead of (Pn-Pn-2) is there a reason behind to choose that formulation for the channel flow (SEM) ??. Could some one please tell me what difference does it make. Thanks in advance Best Regards, Kamal From nek5000-users at lists.mcs.anl.gov Tue Jun 3 04:17:12 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 3 Jun 2014 09:17:12 +0000 Subject: [Nek5000-users] Pn-pn formulation In-Reply-To: References: Message-ID: Hi Kamal, For LES, the extra resolution in the pressure that the PnPn formulation has tends to yield better results. Paul ________________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Tuesday, June 03, 2014 4:08 AM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] Pn-pn formulation Hi Neks, I found that in the turbulence channel example, (Pn-Pn) formulation is used instead of (Pn-Pn-2) is there a reason behind to choose that formulation for the channel flow (SEM) ??. Could some one please tell me what difference does it make. Thanks in advance Best Regards, Kamal _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Tue Jun 3 04:20:21 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 03 Jun 2014 11:20:21 +0200 Subject: [Nek5000-users] Pn-pn formulation In-Reply-To: References: Message-ID: Hi paul, Thanks for reply. Is it good to maintain Pn- Pn for DNS too ?? Regards, Kamal On 03/06/2014 11:17, nek5000-users at lists.mcs.anl.gov wrote: > Hi Kamal, > > For LES, the extra resolution in the pressure that the PnPn formulation > has tends to yield better results. > > Paul > > ________________________________________ > From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > Sent: Tuesday, June 03, 2014 4:08 AM > To: nek5000-users at lists.mcs.anl.gov > Subject: [Nek5000-users] Pn-pn formulation > > Hi Neks, > > I found that in the turbulence channel example, (Pn-Pn) formulation is > used instead of (Pn-Pn-2) is there a reason behind to choose that > formulation for the channel flow (SEM) ??. Could some one please tell me > what difference does it make. > > Thanks in advance > > Best Regards, > Kamal > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Tue Jun 3 04:21:32 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 3 Jun 2014 09:21:32 +0000 Subject: [Nek5000-users] Pn-pn formulation In-Reply-To: References: , Message-ID: Yes, but it starts to become less critical -- both formulations have exponential convergence. So, once you're resolved, they are pretty much the same. ________________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Tuesday, June 03, 2014 4:20 AM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Pn-pn formulation Hi paul, Thanks for reply. Is it good to maintain Pn- Pn for DNS too ?? Regards, Kamal On 03/06/2014 11:17, nek5000-users at lists.mcs.anl.gov wrote: > Hi Kamal, > > For LES, the extra resolution in the pressure that the PnPn formulation > has tends to yield better results. > > Paul > > ________________________________________ > From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > Sent: Tuesday, June 03, 2014 4:08 AM > To: nek5000-users at lists.mcs.anl.gov > Subject: [Nek5000-users] Pn-pn formulation > > Hi Neks, > > I found that in the turbulence channel example, (Pn-Pn) formulation is > used instead of (Pn-Pn-2) is there a reason behind to choose that > formulation for the channel flow (SEM) ??. Could some one please tell me > what difference does it make. > > Thanks in advance > > Best Regards, > Kamal > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Tue Jun 3 07:17:04 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 3 Jun 2014 12:17:04 +0000 Subject: [Nek5000-users] Reg: Visit In-Reply-To: References: <42328EFE-05CD-45EC-A746-BAD77726D5F7@msstate.edu> , , Message-ID: Thanks, Ravi, I would try a Nek run with ASCII dump (p66<0 in .rea) to check whether formatting of the files is an issue. Aleks ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Monday, June 02, 2014 7:13 PM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Reg: Visit Hi Ravi, What error are you getting? It should not be the same error you reported earlier: VisIt could not read from the file "C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowMach_test0.f00001.nek5000". since you are presumably opening lowMach_test.nek5000 instead, right? Aleks ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Monday, June 02, 2014 6:21 PM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Reg: Visit I get error even now. I modified the way you suggested, but still I get error. I typed 'visnek lowMach_test'. I get below message in my terminal. Also one may need to correct for an endian by inserting the first line "endian big" or "endian little" in case of, e.g., files transfered from other systems Total 10 file(s) are in the generated file lowMach_test.nek5000 ... Done! But when I try to view the files I get the error again. Ravi Kiran Pendyala, Graduate Research Assistant, Department of Aerospace Engineering, Mississippi State University, Email: srp265 at msstate.edu On Mon, Jun 2, 2014 at 3:15 PM, > wrote: Hi Ravi and Tanmoy, Actually you need to provide a case name for visnek script since it creates the following template echo 'filetemplate: '$base'%01d.f%05d' > $base.nek5000 Thus you should try visnek lowMach_test and not 'visnek lowMach_test0.f00001' (ANother alternative, before running nek with scripts tools/scripts/nek*, delete 'rm SESSION.NAME' from them and just type visnek so it can look up for the case name in the SESSION.NAME file) Aleks ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Monday, June 02, 2014 2:55 PM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Reg: Visit I have my nek5000 program on linux system. For post processing I take the data files on to my windows system where I have my VisIt tool. Is this problem for not being able to read the files. visnek also didn't help. I did this. start VisIt and use File->Open As? and then select Nek5000 reader as the reader to use to open the files. Thanks for your patience. ERROR: VisIt could not read from the file "C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowMach_test0.f00001.nek5000". The generated error message was: There was an error opening C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowMach_test0.f00001.nek5000. It may be an invalid file. VisIt tried using the following file format readers to open the file: Nek5000 The following error(s) may be helpful in identifying the problem: When attempting to use "Nek", the file matched the general format expected by the reader but eventually encountered this error: "Could not open file C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowMach_test0.f000010.f00001, which should exist according to header file C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowMach_test0.f00001.nek5000.". Ravi Kiran Pendyala, Graduate Research Assistant, Department of Aerospace Engineering, Mississippi State University, Email: srp265 at msstate.edu On Mon, Jun 2, 2014 at 10:36 AM, > wrote: Hi Ravi, try visnek A <>.nek5000 file would be created. You would be able to read that from visit Tanmoy On Mon, Jun 2, 2014 at 2:09 AM, > wrote: Hi, I tried it. I still receive the same error though. Ravi Kiran Pendyala, Graduate Research Assistant, Department of Aerospace Engineering, Mississippi State University, Email: srp265 at msstate.edu On Mon, Jun 2, 2014 at 3:38 AM, Msu > wrote: Thank you for the kind and quickest response. Thanks again, Ravi Kiran Pendyala, On Jun 2, 2014, at 3:38, nek5000-users at lists.mcs.anl.gov wrote: Hi, Create a separate file with ' .nek5000 ' has extension and write those lines in it and open it via Visit and It should work. Best Regards, Kamal On 02/06/2014 10:35, nek5000-users at lists.mcs.anl.gov wrote: No. I didn't not get a clue of working with metadata file. I read about it. Couldn't figure out how to create this. Is a a separate file or set of commands? Ravi Kiran Pendyala, On Jun 2, 2014, at 3:18, nek5000-users at lists.mcs.anl.gov wrote: Hi Ravi, Did you create a metadata file ?? A meta data file is the one which helps you to open a *.fld or *.f00000 file in visit It looks like this NEK5000 version: 1.0 filetemplate: divpipe%01d.f%05d firsttimestep: 1 numtimesteps: 09 Best regards, Kamal On 02/06/2014 09:57, nek5000-users at lists.mcs.anl.gov wrote: Hello all, I cannot view the output files from the nek5000 .fld format using VisIt. I am very new to using nek5000 code. . I tried paraview too. It didn't work. Help greatly appreciated. The following message was posted in forum but didn't find reply so had to post. error message VisIt could not read from the file "C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowmach\lowMach_test0.f* database". The generated error message was: There was an error opening C:\Users\s pendyala\AppData\Local\Programs\LLNL\VisIt 2.7.2\lowmach\lowMach_test0.f* database. It may be an invalid file. VisIt tried using the following file format readers to open the file: Silo Thank you, Ravi Kiran Pendyala, Graduate Research Assistant, Department of Aerospace Engineering, Mississippi State University, Email: srp265 at msstate.edu _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Jun 4 09:34:03 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 4 Jun 2014 22:34:03 +0800 (CST) Subject: [Nek5000-users] How to run Nek5000 in cluster based on mpich? Message-ID: Hi,all: I have just built a small cluster of computers, based on mpich.I have tested the capability of this cluster, each node can be called freely. Now I want to do my simulation in it, however, I don't know how to run Nek. As known, on only 1 computer, one can do like this: nekmpi XXX X or nekbmpi XXX X while this is not the case in the cluster! I believe most of you have tried this, I'll appreciate if anyone can give me some advice. Best regards Xianbei -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Jun 4 10:20:52 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 4 Jun 2014 15:20:52 +0000 Subject: [Nek5000-users] How to run Nek5000 in cluster based on mpich? In-Reply-To: References: Message-ID: Hi Xianbei, Have a look at the nekbmpi script and modify to match the job submission procedure on your cluster. Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Wednesday, June 04, 2014 9:34 AM To: Nek5000 Subject: [Nek5000-users] How to run Nek5000 in cluster based on mpich? Hi,all: I have just built a small cluster of computers, based on mpich.I have tested the capability of this cluster, each node can be called freely. Now I want to do my simulation in it, however, I don't know how to run Nek. As known, on only 1 computer, one can do like this: nekmpi XXX X or nekbmpi XXX X while this is not the case in the cluster! I believe most of you have tried this, I'll appreciate if anyone can give me some advice. Best regards Xianbei ?????????????? -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Jun 4 21:23:51 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 5 Jun 2014 10:23:51 +0800 (CST) Subject: [Nek5000-users] How to run Nek5000 in cluster based on mpich? In-Reply-To: References: Message-ID: Hi, Paul: I read the nekbmpi file and find this: mpiexec -np $2 ./nek5000 > $1.log.$2 & so the nek5000 is executed by mpi. In mpich, the common way to run a executable program can be run as : mpiexec -n XX ./nek5000 However, when I type this: mpiexec -n 32 ./nek5000 > turbChannel.log & error returns like: Fortran runtime error: File './NEK.rea' does not exist Best reguards Xianbei At 2014-06-04 11:20:52, nek5000-users at lists.mcs.anl.gov wrote: Hi Xianbei, Have a look at the nekbmpi script and modify to match the job submission procedure on your cluster. Paul From:nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Wednesday, June 04, 2014 9:34 AM To: Nek5000 Subject: [Nek5000-users] How to run Nek5000 in cluster based on mpich? Hi,all: I have just built a small cluster of computers, based on mpich.I have tested the capability of this cluster, each node can be called freely. Now I want to do my simulation in it, however, I don't know how to run Nek. As known, on only 1 computer, one can do like this: nekmpi XXX X or nekbmpi XXX X while this is not the case in the cluster! I believe most of you have tried this, I'll appreciate if anyone can give me some advice. Best regards Xianbei ?????????????? -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Jun 4 21:30:54 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 5 Jun 2014 02:30:54 +0000 Subject: [Nek5000-users] How to run Nek5000 in cluster based on mpich? In-Reply-To: References: , Message-ID: Hi Xianbei, You need to be certain to use the full script, but change the mpiexec command to reflect what is on your system. The script sets up some default files that nek5000 will be looking for when it starts (specifically, SESSION.NAME) Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Wednesday, June 04, 2014 9:23 PM To: Nek5000 Subject: Re: [Nek5000-users] How to run Nek5000 in cluster based on mpich? Hi, Paul: I read the nekbmpi file and find this: mpiexec -np $2 ./nek5000 > $1.log.$2 & so the nek5000 is executed by mpi. In mpich, the common way to run a executable program can be run as : mpiexec -n XX ./nek5000 However, when I type this: mpiexec -n 32 ./nek5000 > turbChannel.log & error returns like: Fortran runtime error: File './NEK.rea' does not exist Best reguards Xianbei At 2014-06-04 11:20:52, nek5000-users at lists.mcs.anl.gov wrote: Hi Xianbei, Have a look at the nekbmpi script and modify to match the job submission procedure on your cluster. Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Wednesday, June 04, 2014 9:34 AM To: Nek5000 Subject: [Nek5000-users] How to run Nek5000 in cluster based on mpich? Hi,all: I have just built a small cluster of computers, based on mpich.I have tested the capability of this cluster, each node can be called freely. Now I want to do my simulation in it, however, I don't know how to run Nek. As known, on only 1 computer, one can do like this: nekmpi XXX X or nekbmpi XXX X while this is not the case in the cluster! I believe most of you have tried this, I'll appreciate if anyone can give me some advice. Best regards Xianbei ?????????????? ?????????????? -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Jun 4 21:44:17 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 5 Jun 2014 02:44:17 +0000 Subject: [Nek5000-users] weak derivative, dssum and binvm1 in cvode_driver Message-ID: Dear Nek team, I have a quick question: in cvode_driver.f, in the routine fcvfun, do all the derivatives must be in weak formulation (using wgradm1) when constructing the right hand side term ydot? Because at the end of the routine fcvfun, dssum and multiplication by binvm1 are applied to the right hand side term ydot. It?s also not clear to me if I need to apply dssum and binvm1 for each derivative term appearing in my equation (in other terms, each time after calling wgradm1), or if I need to apply dssum and binvm1 only to the whole RHS term ydot ? I?m afraid of inconsistency if apply twice dssum and binvm1: one during the construction of operators and one on the final ydot term. Thank you for you help ! Best regards, Emmanuel -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Jun 4 23:41:09 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 5 Jun 2014 12:41:09 +0800 (CST) Subject: [Nek5000-users] How to run Nek5000 in cluster based on mpich? In-Reply-To: References: Message-ID: Hi,Paul: I change this line: mpiexec -np $2 ./nek5000 > $1.log.$2 & to mpiexec -n $2 ./nek5000 > $1.log.$2 & in nekbmpi and then changed the name to 'runnek' in each node Then type ./runnek xxx 48 While the error still exsits. Xianbei At 2014-06-04 11:20:52, nek5000-users at lists.mcs.anl.gov wrote: Hi Xianbei, Have a look at the nekbmpi script and modify to match the job submission procedure on your cluster. Paul From:nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Wednesday, June 04, 2014 9:34 AM To: Nek5000 Subject: [Nek5000-users] How to run Nek5000 in cluster based on mpich? Hi,all: I have just built a small cluster of computers, based on mpich.I have tested the capability of this cluster, each node can be called freely. Now I want to do my simulation in it, however, I don't know how to run Nek. As known, on only 1 computer, one can do like this: nekmpi XXX X or nekbmpi XXX X while this is not the case in the cluster! I believe most of you have tried this, I'll appreciate if anyone can give me some advice. Best regards Xianbei ?????????????? -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Jun 4 23:57:27 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 5 Jun 2014 04:57:27 +0000 Subject: [Nek5000-users] How to run Nek5000 in cluster based on mpich? In-Reply-To: References: Message-ID: Hi all, I just would like to bring my experience because I had a similar problem. In my case it appears that the mpiexec command takes some times to be executed, and it is not fully completed after the end of instruction ?sleep 2? . So the command rm -f SESSION.NAME is executed before full execution of mpiexec. Consequently, nek can?t find the session file and it searches for nek.rea, which doesn?t exist. In my case the problem appears for a cpu number > to 4. I just added some more seconds to the sleeping time and everything works fine now. "Sleep 5" is reasonable in my case to be able to launch nek on 24 cpus. Hope that helps ! Best regards, Emmanuel On 5 Jun 2014, at 14:11, > > wrote: Hi,Paul: I change this line: mpiexec -np $2 ./nek5000 > $1.log.$2 & to mpiexec -n $2 ./nek5000 > $1.log.$2 & in nekbmpi and then changed the name to 'runnek' in each node Then type ./runnek xxx 48 While the error still exsits. Xianbei At 2014-06-04 11:20:52, nek5000-users at lists.mcs.anl.gov wrote: Hi Xianbei, Have a look at the nekbmpi script and modify to match the job submission procedure on your cluster. Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Wednesday, June 04, 2014 9:34 AM To: Nek5000 Subject: [Nek5000-users] How to run Nek5000 in cluster based on mpich? Hi,all: I have just built a small cluster of computers, based on mpich.I have tested the capability of this cluster, each node can be called freely. Now I want to do my simulation in it, however, I don't know how to run Nek. As known, on only 1 computer, one can do like this: nekmpi XXX X or nekbmpi XXX X while this is not the case in the cluster! I believe most of you have tried this, I'll appreciate if anyone can give me some advice. Best regards Xianbei ?????????????? ?????????????? _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Jun 5 00:04:00 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 5 Jun 2014 13:04:00 +0800 (CST) Subject: [Nek5000-users] How to run Nek5000 in cluster based on mpich? In-Reply-To: References: Message-ID: Hi, Emmanuel: Thank you for your suggestion. So you mean the way running the script is right like this: ./runnek xxx 48 right? I'll try it. Xianbei At 2014-06-05 12:57:27, nek5000-users at lists.mcs.anl.gov wrote: Hi all, I just would like to bring my experience because I had a similar problem. In my case it appears that the mpiexec command takes some times to be executed, and it is not fully completed after the end of instruction ?sleep 2? . So the command rm -f SESSION.NAME is executed before full execution of mpiexec. Consequently, nek can?t find the session file and it searches for nek.rea, which doesn?t exist. In my case the problem appears for a cpu number > to 4. I just added some more seconds to the sleeping time and everything works fine now. "Sleep 5" is reasonable in my case to be able to launch nek on 24 cpus. Hope that helps ! Best regards, Emmanuel On 5 Jun 2014, at 14:11, wrote: Hi,Paul: I change this line: mpiexec -np $2 ./nek5000 > $1.log.$2 & to mpiexec -n $2 ./nek5000 > $1.log.$2 & in nekbmpi and then changed the name to 'runnek' in each node Then type ./runnek xxx 48 While the error still exsits. Xianbei At 2014-06-04 11:20:52, nek5000-users at lists.mcs.anl.gov wrote: Hi Xianbei, Have a look at the nekbmpi script and modify to match the job submission procedure on your cluster. Paul From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Wednesday, June 04, 2014 9:34 AM To: Nek5000 Subject: [Nek5000-users] How to run Nek5000 in cluster based on mpich? Hi,all: I have just built a small cluster of computers, based on mpich.I have tested the capability of this cluster, each node can be called freely. Now I want to do my simulation in it, however, I don't know how to run Nek. As known, on only 1 computer, one can do like this: nekmpi XXX X or nekbmpi XXX X while this is not the case in the cluster! I believe most of you have tried this, I'll appreciate if anyone can give me some advice. Best regards Xianbei ?????????????? ?????????????? _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Jun 5 00:28:00 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 5 Jun 2014 13:28:00 +0800 (CST) Subject: [Nek5000-users] How to run Nek5000 in cluster based on mpich? In-Reply-To: References: Message-ID: Hi, Emmanuel: I try your method, while even if I change sleep to 10 sec, it still has the same error. Can you make it more clear about how you managed to run in different nodes? I mean how to setup and run, what's different with the common case? Best reguards Xianbei At 2014-06-05 12:57:27, nek5000-users at lists.mcs.anl.gov wrote: Hi all, I just would like to bring my experience because I had a similar problem. In my case it appears that the mpiexec command takes some times to be executed, and it is not fully completed after the end of instruction ?sleep 2? . So the command rm -f SESSION.NAME is executed before full execution of mpiexec. Consequently, nek can?t find the session file and it searches for nek.rea, which doesn?t exist. In my case the problem appears for a cpu number > to 4. I just added some more seconds to the sleeping time and everything works fine now. "Sleep 5" is reasonable in my case to be able to launch nek on 24 cpus. Hope that helps ! Best regards, Emmanuel On 5 Jun 2014, at 14:11, wrote: Hi,Paul: I change this line: mpiexec -np $2 ./nek5000 > $1.log.$2 & to mpiexec -n $2 ./nek5000 > $1.log.$2 & in nekbmpi and then changed the name to 'runnek' in each node Then type ./runnek xxx 48 While the error still exsits. Xianbei At 2014-06-04 11:20:52, nek5000-users at lists.mcs.anl.gov wrote: Hi Xianbei, Have a look at the nekbmpi script and modify to match the job submission procedure on your cluster. Paul From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Wednesday, June 04, 2014 9:34 AM To: Nek5000 Subject: [Nek5000-users] How to run Nek5000 in cluster based on mpich? Hi,all: I have just built a small cluster of computers, based on mpich.I have tested the capability of this cluster, each node can be called freely. Now I want to do my simulation in it, however, I don't know how to run Nek. As known, on only 1 computer, one can do like this: nekmpi XXX X or nekbmpi XXX X while this is not the case in the cluster! I believe most of you have tried this, I'll appreciate if anyone can give me some advice. Best regards Xianbei ?????????????? ?????????????? _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Jun 5 00:35:31 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 5 Jun 2014 05:35:31 +0000 Subject: [Nek5000-users] How to run Nek5000 in cluster based on mpich? In-Reply-To: References: Message-ID: I?m just launching the code as explained in the ?quick start? chapter of the user manual. On my computer I had a problem with the sleeping time specified in the nek script. This problem is specific to my machine, but the description of your problem reminded me it. However I don?t know if it is really related ! Good luck ! Best regards, Emmanuel On 5 Jun 2014, at 14:58, > > wrote: Hi, Emmanuel: I try your method, while even if I change sleep to 10 sec, it still has the same error. Can you make it more clear about how you managed to run in different nodes? I mean how to setup and run, what's different with the common case? Best reguards Xianbei At 2014-06-05 12:57:27, nek5000-users at lists.mcs.anl.gov wrote: Hi all, I just would like to bring my experience because I had a similar problem. In my case it appears that the mpiexec command takes some times to be executed, and it is not fully completed after the end of instruction ?sleep 2? . So the command rm -f SESSION.NAME is executed before full execution of mpiexec. Consequently, nek can?t find the session file and it searches for nek.rea, which doesn?t exist. In my case the problem appears for a cpu number > to 4. I just added some more seconds to the sleeping time and everything works fine now. "Sleep 5" is reasonable in my case to be able to launch nek on 24 cpus. Hope that helps ! Best regards, Emmanuel On 5 Jun 2014, at 14:11, > > wrote: Hi,Paul: I change this line: mpiexec -np $2 ./nek5000 > $1.log.$2 & to mpiexec -n $2 ./nek5000 > $1.log.$2 & in nekbmpi and then changed the name to 'runnek' in each node Then type ./runnek xxx 48 While the error still exsits. Xianbei At 2014-06-04 11:20:52, nek5000-users at lists.mcs.anl.gov wrote: Hi Xianbei, Have a look at the nekbmpi script and modify to match the job submission procedure on your cluster. Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Wednesday, June 04, 2014 9:34 AM To: Nek5000 Subject: [Nek5000-users] How to run Nek5000 in cluster based on mpich? Hi,all: I have just built a small cluster of computers, based on mpich.I have tested the capability of this cluster, each node can be called freely. Now I want to do my simulation in it, however, I don't know how to run Nek. As known, on only 1 computer, one can do like this: nekmpi XXX X or nekbmpi XXX X while this is not the case in the cluster! I believe most of you have tried this, I'll appreciate if anyone can give me some advice. Best regards Xianbei ?????????????? ?????????????? _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users ?????????????? _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Jun 5 00:41:37 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 5 Jun 2014 13:41:37 +0800 (CST) Subject: [Nek5000-users] How to run Nek5000 in cluster based on mpich? In-Reply-To: References: Message-ID: I see, maybe the problem is specific to my machine too, my god. Thank you for your help. Xianbei At 2014-06-05 01:35:31, nek5000-users at lists.mcs.anl.gov wrote: I?m just launching the code as explained in the ?quick start? chapter of the user manual. On my computer I had a problem with the sleeping time specified in the nek script. This problem is specific to my machine, but the description of your problem reminded me it. However I don?t know if it is really related ! Good luck ! Best regards, Emmanuel On 5 Jun 2014, at 14:58, wrote: Hi, Emmanuel: I try your method, while even if I change sleep to 10 sec, it still has the same error. Can you make it more clear about how you managed to run in different nodes? I mean how to setup and run, what's different with the common case? Best reguards Xianbei At 2014-06-05 12:57:27, nek5000-users at lists.mcs.anl.gov wrote: Hi all, I just would like to bring my experience because I had a similar problem. In my case it appears that the mpiexec command takes some times to be executed, and it is not fully completed after the end of instruction ?sleep 2? . So the command rm -f SESSION.NAME is executed before full execution of mpiexec. Consequently, nek can?t find the session file and it searches for nek.rea, which doesn?t exist. In my case the problem appears for a cpu number > to 4. I just added some more seconds to the sleeping time and everything works fine now. "Sleep 5" is reasonable in my case to be able to launch nek on 24 cpus. Hope that helps ! Best regards, Emmanuel On 5 Jun 2014, at 14:11, wrote: Hi,Paul: I change this line: mpiexec -np $2 ./nek5000 > $1.log.$2 & to mpiexec -n $2 ./nek5000 > $1.log.$2 & in nekbmpi and then changed the name to 'runnek' in each node Then type ./runnek xxx 48 While the error still exsits. Xianbei At 2014-06-04 11:20:52, nek5000-users at lists.mcs.anl.gov wrote: Hi Xianbei, Have a look at the nekbmpi script and modify to match the job submission procedure on your cluster. Paul From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Wednesday, June 04, 2014 9:34 AM To: Nek5000 Subject: [Nek5000-users] How to run Nek5000 in cluster based on mpich? Hi,all: I have just built a small cluster of computers, based on mpich.I have tested the capability of this cluster, each node can be called freely. Now I want to do my simulation in it, however, I don't know how to run Nek. As known, on only 1 computer, one can do like this: nekmpi XXX X or nekbmpi XXX X while this is not the case in the cluster! I believe most of you have tried this, I'll appreciate if anyone can give me some advice. Best regards Xianbei ?????????????? ?????????????? _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users ?????????????? _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Jun 5 02:20:55 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 5 Jun 2014 07:20:55 +0000 Subject: [Nek5000-users] weak derivative, dssum and binvm1 in cvode_driver In-Reply-To: References: Message-ID: I?m adding another quick question: why in the routine makeq, under the cvode statement, there are these following 2 lines: call col2(bq,bintm1,ntot) call col2(bq,bm1,ntot) I?m not sure to understand why we are multiplying bq by the inverse of the mass matrix (bintm1) and just after multiplying it back by the mass matrix (bm1). Moreover, after leaving the makeq routine, fctfun will multiplying again ydot=bq/vtrans by the inverse of the mass matrix. Why all of these operations? Thank you for your help ! Best regards, Emmanuel On 5 Jun 2014, at 12:14, > > wrote: Dear Nek team, I have a quick question: in cvode_driver.f, in the routine fcvfun, do all the derivatives must be in weak formulation (using wgradm1) when constructing the right hand side term ydot? Because at the end of the routine fcvfun, dssum and multiplication by binvm1 are applied to the right hand side term ydot. It?s also not clear to me if I need to apply dssum and binvm1 for each derivative term appearing in my equation (in other terms, each time after calling wgradm1), or if I need to apply dssum and binvm1 only to the whole RHS term ydot ? I?m afraid of inconsistency if apply twice dssum and binvm1: one during the construction of operators and one on the final ydot term. Thank you for you help ! Best regards, Emmanuel _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Jun 5 02:38:32 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 05 Jun 2014 09:38:32 +0200 Subject: [Nek5000-users] weak derivative, dssum and binvm1 in cvode_driver In-Reply-To: Message-ID: Hi Emmanuel >From what I recall: CVODE solves the governing non-linear eqns in the strong form. That?s why we have to project every term of the RHS onto H2 (dssum and collocate with bintm1). The sum is projected again onto H2 because it gets devided by vtrans. Hope this helps. Cheers, Stefan Von: Antworten an: Datum: Thursday, June 5, 2014 at 9:20 AM An: "nek5000-users at lists.mcs.anl.gov" Betreff: Re: [Nek5000-users] weak derivative, dssum and binvm1 in cvode_driver I?m adding another quick question: why in the routine makeq, under the cvode statement, there are these following 2 lines: call col2(bq,bintm1,ntot) call col2(bq,bm1,ntot) I?m not sure to understand why we are multiplying bq by the inverse of the mass matrix (bintm1) and just after multiplying it back by the mass matrix (bm1). Moreover, after leaving the makeq routine, fctfun will multiplying again ydot=bq/vtrans by the inverse of the mass matrix. Why all of these operations? Thank you for your help ! Best regards, Emmanuel On 5 Jun 2014, at 12:14, wrote: > Dear Nek team, > > I have a quick question: in cvode_driver.f, in the routine fcvfun, do all the > derivatives must be in weak formulation (using wgradm1) when constructing the > right hand side term ydot? > Because at the end of the routine fcvfun, dssum and multiplication by binvm1 > are applied to the right hand side term ydot. > > It?s also not clear to me if I need to apply dssum and binvm1 for each > derivative term appearing in my equation (in other terms, each time after > calling wgradm1), or if I need to apply dssum and binvm1 only to the whole RHS > term ydot ? > > I?m afraid of inconsistency if apply twice dssum and binvm1: one during the > construction of operators and one on the final ydot term. > > Thank you for you help ! > > Best regards, > Emmanuel > > > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Jun 5 04:10:12 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 5 Jun 2014 09:10:12 +0000 Subject: [Nek5000-users] How to run Nek5000 in cluster based on mpich? In-Reply-To: References: , Message-ID: Hi All, My apologies, I actually never use the "rm -f SESSION.NAME" in my scripts. I think it was put there just so you wouldn't have too many junk files. I suggest commenting it out or removing it. Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Thursday, June 05, 2014 12:41 AM To: Nek5000 Subject: Re: [Nek5000-users] How to run Nek5000 in cluster based on mpich? I see, maybe the problem is specific to my machine too, my god. Thank you for your help. Xianbei At 2014-06-05 01:35:31, nek5000-users at lists.mcs.anl.gov wrote: I?m just launching the code as explained in the ?quick start? chapter of the user manual. On my computer I had a problem with the sleeping time specified in the nek script. This problem is specific to my machine, but the description of your problem reminded me it. However I don?t know if it is really related ! Good luck ! Best regards, Emmanuel On 5 Jun 2014, at 14:58, > > wrote: Hi, Emmanuel: I try your method, while even if I change sleep to 10 sec, it still has the same error. Can you make it more clear about how you managed to run in different nodes? I mean how to setup and run, what's different with the common case? Best reguards Xianbei At 2014-06-05 12:57:27, nek5000-users at lists.mcs.anl.gov wrote: Hi all, I just would like to bring my experience because I had a similar problem. In my case it appears that the mpiexec command takes some times to be executed, and it is not fully completed after the end of instruction ?sleep 2? . So the command rm -f SESSION.NAME is executed before full execution of mpiexec. Consequently, nek can?t find the session file and it searches for nek.rea, which doesn?t exist. In my case the problem appears for a cpu number > to 4. I just added some more seconds to the sleeping time and everything works fine now. "Sleep 5" is reasonable in my case to be able to launch nek on 24 cpus. Hope that helps ! Best regards, Emmanuel On 5 Jun 2014, at 14:11, > > wrote: Hi,Paul: I change this line: mpiexec -np $2 ./nek5000 > $1.log.$2 & to mpiexec -n $2 ./nek5000 > $1.log.$2 & in nekbmpi and then changed the name to 'runnek' in each node Then type ./runnek xxx 48 While the error still exsits. Xianbei At 2014-06-04 11:20:52, nek5000-users at lists.mcs.anl.gov wrote: Hi Xianbei, Have a look at the nekbmpi script and modify to match the job submission procedure on your cluster. Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Wednesday, June 04, 2014 9:34 AM To: Nek5000 Subject: [Nek5000-users] How to run Nek5000 in cluster based on mpich? Hi,all: I have just built a small cluster of computers, based on mpich.I have tested the capability of this cluster, each node can be called freely. Now I want to do my simulation in it, however, I don't know how to run Nek. As known, on only 1 computer, one can do like this: nekmpi XXX X or nekbmpi XXX X while this is not the case in the cluster! I believe most of you have tried this, I'll appreciate if anyone can give me some advice. Best regards Xianbei ?????????????? ?????????????? _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users ?????????????? _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users ?????????????? -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Jun 5 04:55:22 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 5 Jun 2014 09:55:22 +0000 Subject: [Nek5000-users] weak derivative, dssum and binvm1 in cvode_driver In-Reply-To: References: , Message-ID: Hi Emmanuel, Note that bintm1 and bm1 are not precise inverses of one another. bm1 is the unassembled mass matrix - i.e., it is the collection of local (to each element) mass matrices, each of which is diagonal. Conceptually, we denote the local mass matrix as B_L, for local. Then, the assembled mass matrix is: B := Q^T B_L Q where Q is the Boolean matrix that copies global degrees of freedom to their shared counterparts (i.e., copies a values to shared faces, edges, vertices, etc.). For the SEM, B_L is diagonal, as is B, so Binv := B^-1 is easily computed. Once the entries of this diagonal matrix are known, we can copy them to their element-based locations, so that we can generate B^-1 * r very easily. Often, products with these matrices, in conjunction with dssum, are used to generate continuous fields and that appears to be what is happening in this case. An example would be if you want to find a the continuous counterpart to a discontinuous function g. The usual projection approach is: Find gc \in H1 such that \int v gc dV = \int v g dV for all v in H1, which ends up looking like: Find gc \in H1 such that: (v,gc) = (v,g) for all g \in H1 or v B gc = v Q^T B_L g_L gc = B^-1 Q^T B_L g_L gc_L = Q B^-1 Q^T B_L g_L In Nek, the last statement is expressed as: call col2(g,bm1,n) call dssum(g,nx1,ny1,nz1) call col2(g,bintm1,n) In your cvode case, these statements are permuted because of the initial state of the data and the desired output (which is to be B*q -- which is why the variable is labeled bq). Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Thursday, June 05, 2014 2:38 AM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] weak derivative, dssum and binvm1 in cvode_driver Hi Emmanuel >From what I recall: CVODE solves the governing non-linear eqns in the strong form. That?s why we have to project every term of the RHS onto H2 (dssum and collocate with bintm1). The sum is projected again onto H2 because it gets devided by vtrans. Hope this helps. Cheers, Stefan Von: > Antworten an: > Datum: Thursday, June 5, 2014 at 9:20 AM An: "nek5000-users at lists.mcs.anl.gov" > Betreff: Re: [Nek5000-users] weak derivative, dssum and binvm1 in cvode_driver I?m adding another quick question: why in the routine makeq, under the cvode statement, there are these following 2 lines: call col2(bq,bintm1,ntot) call col2(bq,bm1,ntot) I?m not sure to understand why we are multiplying bq by the inverse of the mass matrix (bintm1) and just after multiplying it back by the mass matrix (bm1). Moreover, after leaving the makeq routine, fctfun will multiplying again ydot=bq/vtrans by the inverse of the mass matrix. Why all of these operations? Thank you for your help ! Best regards, Emmanuel On 5 Jun 2014, at 12:14, > > wrote: Dear Nek team, I have a quick question: in cvode_driver.f, in the routine fcvfun, do all the derivatives must be in weak formulation (using wgradm1) when constructing the right hand side term ydot? Because at the end of the routine fcvfun, dssum and multiplication by binvm1 are applied to the right hand side term ydot. It?s also not clear to me if I need to apply dssum and binvm1 for each derivative term appearing in my equation (in other terms, each time after calling wgradm1), or if I need to apply dssum and binvm1 only to the whole RHS term ydot ? I?m afraid of inconsistency if apply twice dssum and binvm1: one during the construction of operators and one on the final ydot term. Thank you for you help ! Best regards, Emmanuel _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Jun 5 10:06:18 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 5 Jun 2014 15:06:18 +0000 Subject: [Nek5000-users] weak derivative, dssum and binvm1 in cvode_driver In-Reply-To: References: , Message-ID: Hi Paul and Stefan, Thank you for the explanations, things are going gradually more clear in my mind. So for a practical application, still in the context of cvode, I would like to add a new term to the RHS of the temperature equation. This new term is roughly (vdiff * grad (Y)) grad (T) where Y is a passive scalar, vdiff the diffusion coefficient of this passive scalar and T the temperature. Basically in the routine makeq.f the implementation should looks like to call wgradm1(Y_x, Y_y, Y_z, t(1,1,1,1,ifield+1), nelv) call dssum(grad_Y, Y_x, Y_y, Y_z) call col2(grad_Y,bintm1,ntot) call col2(grad_Y, vdiff(1,1,1,1,ifield+2) ,ntot ) call wgradm1(T_x, T_y, T_z, t(1,1,1,1,ifield), nelv) call dssum(grad_T, T_x, T_y, T_z) call col2(grad_T,grad_Y,ntot) call add2(bq(1,1,1,1,ifield), grad_T,ntot) and then convab and wlaplacian routines will add the other terms, and it will finish with call dssum(bq,nx1,ny1,nz1) call col2(bq,bintm1,ntot) call col2(bq,bm1,ntot) Am I right?? Thank you for your help ! Best regards, Emmanuel On 5 Jun 2014, at 19:25, > > wrote: Hi Emmanuel, Note that bintm1 and bm1 are not precise inverses of one another. bm1 is the unassembled mass matrix - i.e., it is the collection of local (to each element) mass matrices, each of which is diagonal. Conceptually, we denote the local mass matrix as B_L, for local. Then, the assembled mass matrix is: B := Q^T B_L Q where Q is the Boolean matrix that copies global degrees of freedom to their shared counterparts (i.e., copies a values to shared faces, edges, vertices, etc.). For the SEM, B_L is diagonal, as is B, so Binv := B^-1 is easily computed. Once the entries of this diagonal matrix are known, we can copy them to their element-based locations, so that we can generate B^-1 * r very easily. Often, products with these matrices, in conjunction with dssum, are used to generate continuous fields and that appears to be what is happening in this case. An example would be if you want to find a the continuous counterpart to a discontinuous function g. The usual projection approach is: Find gc \in H1 such that \int v gc dV = \int v g dV for all v in H1, which ends up looking like: Find gc \in H1 such that: (v,gc) = (v,g) for all g \in H1 or v B gc = v Q^T B_L g_L gc = B^-1 Q^T B_L g_L gc_L = Q B^-1 Q^T B_L g_L In Nek, the last statement is expressed as: call col2(g,bm1,n) call dssum(g,nx1,ny1,nz1) call col2(g,bintm1,n) In your cvode case, these statements are permuted because of the initial state of the data and the desired output (which is to be B*q -- which is why the variable is labeled bq). Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Thursday, June 05, 2014 2:38 AM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] weak derivative, dssum and binvm1 in cvode_driver Hi Emmanuel >From what I recall: CVODE solves the governing non-linear eqns in the strong form. That?s why we have to project every term of the RHS onto H2 (dssum and collocate with bintm1). The sum is projected again onto H2 because it gets devided by vtrans. Hope this helps. Cheers, Stefan Von: > Antworten an: > Datum: Thursday, June 5, 2014 at 9:20 AM An: "nek5000-users at lists.mcs.anl.gov" > Betreff: Re: [Nek5000-users] weak derivative, dssum and binvm1 in cvode_driver I?m adding another quick question: why in the routine makeq, under the cvode statement, there are these following 2 lines: call col2(bq,bintm1,ntot) call col2(bq,bm1,ntot) I?m not sure to understand why we are multiplying bq by the inverse of the mass matrix (bintm1) and just after multiplying it back by the mass matrix (bm1). Moreover, after leaving the makeq routine, fctfun will multiplying again ydot=bq/vtrans by the inverse of the mass matrix. Why all of these operations? Thank you for your help ! Best regards, Emmanuel On 5 Jun 2014, at 12:14, > > wrote: Dear Nek team, I have a quick question: in cvode_driver.f, in the routine fcvfun, do all the derivatives must be in weak formulation (using wgradm1) when constructing the right hand side term ydot? Because at the end of the routine fcvfun, dssum and multiplication by binvm1 are applied to the right hand side term ydot. It?s also not clear to me if I need to apply dssum and binvm1 for each derivative term appearing in my equation (in other terms, each time after calling wgradm1), or if I need to apply dssum and binvm1 only to the whole RHS term ydot ? I?m afraid of inconsistency if apply twice dssum and binvm1: one during the construction of operators and one on the final ydot term. Thank you for you help ! Best regards, Emmanuel _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing listNek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Jun 5 10:11:12 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 05 Jun 2014 17:11:12 +0200 Subject: [Nek5000-users] weak derivative, dssum and binvm1 in cvode_driver In-Reply-To: Message-ID: I guess you want to solve for species and temperature using detailed chemistry and transport. Right? Von: Antworten an: Datum: Thursday, June 5, 2014 at 5:06 PM An: "nek5000-users at lists.mcs.anl.gov" Betreff: Re: [Nek5000-users] weak derivative, dssum and binvm1 in cvode_driver Hi Paul and Stefan, Thank you for the explanations, things are going gradually more clear in my mind. So for a practical application, still in the context of cvode, I would like to add a new term to the RHS of the temperature equation. This new term is roughly (vdiff * grad (Y)) grad (T) where Y is a passive scalar, vdiff the diffusion coefficient of this passive scalar and T the temperature. Basically in the routine makeq.f the implementation should looks like to call wgradm1(Y_x, Y_y, Y_z, t(1,1,1,1,ifield+1), nelv) call dssum(grad_Y, Y_x, Y_y, Y_z) call col2(grad_Y,bintm1,ntot) call col2(grad_Y, vdiff(1,1,1,1,ifield+2) ,ntot ) call wgradm1(T_x, T_y, T_z, t(1,1,1,1,ifield), nelv) call dssum(grad_T, T_x, T_y, T_z) call col2(grad_T,grad_Y,ntot) call add2(bq(1,1,1,1,ifield), grad_T,ntot) and then convab and wlaplacian routines will add the other terms, and it will finish with call dssum(bq,nx1,ny1,nz1) call col2(bq,bintm1,ntot) call col2(bq,bm1,ntot) Am I right?? Thank you for your help ! Best regards, Emmanuel On 5 Jun 2014, at 19:25, wrote: > > Hi Emmanuel, > > Note that bintm1 and bm1 are not precise inverses of one another. > bm1 is the unassembled mass matrix - i.e., it is the collection of local > (to each element) mass matrices, each of which is diagonal. > > Conceptually, we denote the local mass matrix as B_L, for local. > Then, the assembled mass matrix is: > > B := Q^T B_L Q > > where Q is the Boolean matrix that copies global degrees of freedom > to their shared counterparts (i.e., copies a values to shared faces, > edges, vertices, etc.). For the SEM, B_L is diagonal, as is B, so > Binv := B^-1 is easily computed. Once the entries of this diagonal > matrix are known, we can copy them to their element-based locations, > so that we can generate B^-1 * r very easily. > > Often, products with these matrices, in conjunction with dssum, are used > to generate continuous fields and that appears to be what is happening in > this case. An example would be if you want to find a the continuous > counterpart to a discontinuous function g. The usual projection approach > is: Find gc \in H1 such that \int v gc dV = \int v g dV for all v in H1, > which > ends up looking like: > > Find gc \in H1 such that: > > > (v,gc) = (v,g) for all g \in H1 > > or > > v B gc = v Q^T B_L g_L > > gc = B^-1 Q^T B_L g_L > > gc_L = Q B^-1 Q^T B_L g_L > > In Nek, the last statement is expressed as: > > call col2(g,bm1,n) > call dssum(g,nx1,ny1,nz1) > call col2(g,bintm1,n) > > In your cvode case, these statements are permuted because of the > initial state of the data and the desired output (which is to be B*q -- > which is why the variable is labeled bq). > > Paul > > > > > > From: nek5000-users-bounces at lists.mcs.anl.gov > [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of > nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > Sent: Thursday, June 05, 2014 2:38 AM > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] weak derivative, dssum and binvm1 in cvode_driver > > Hi Emmanuel > > From what I recall: > CVODE solves the governing non-linear eqns in the strong form. That?s why we > have to project every term of the RHS onto H2 (dssum and collocate with > bintm1). The sum is projected again onto H2 because it gets devided by vtrans. > Hope this helps. > > Cheers, > Stefan > > Von: > Antworten an: > Datum: Thursday, June 5, 2014 at 9:20 AM > An: "nek5000-users at lists.mcs.anl.gov" > Betreff: Re: [Nek5000-users] weak derivative, dssum and binvm1 in cvode_driver > > I?m adding another quick question: > > why in the routine makeq, under the cvode statement, there are these following > 2 lines: > call col2(bq,bintm1,ntot) > call col2(bq,bm1,ntot) > > I?m not sure to understand why we are multiplying bq by the inverse of the > mass matrix (bintm1) and just after multiplying it back by the mass matrix > (bm1). Moreover, after leaving the makeq routine, fctfun will multiplying > again ydot=bq/vtrans by the inverse of the mass matrix. > > Why all of these operations? Thank you for your help ! > > > > Best regards, > Emmanuel > > > > On 5 Jun 2014, at 12:14, > wrote: > >> Dear Nek team, >> >> I have a quick question: in cvode_driver.f, in the routine fcvfun, do all the >> derivatives must be in weak formulation (using wgradm1) when constructing the >> right hand side term ydot? >> Because at the end of the routine fcvfun, dssum and multiplication by binvm1 >> are applied to the right hand side term ydot. >> >> It?s also not clear to me if I need to apply dssum and binvm1 for each >> derivative term appearing in my equation (in other terms, each time after >> calling wgradm1), or if I need to apply dssum and binvm1 only to the whole >> RHS term ydot ? >> >> I?m afraid of inconsistency if apply twice dssum and binvm1: one during the >> construction of operators and one on the final ydot term. >> >> Thank you for you help ! >> >> Best regards, >> Emmanuel >> >> >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > _______________________________________________ Nek5000-users mailing > listNek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Jun 5 10:14:47 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 5 Jun 2014 15:14:47 +0000 Subject: [Nek5000-users] weak derivative, dssum and binvm1 in cvode_driver In-Reply-To: References: Message-ID: Yes exactly ! Best regards, Emmanuel On 6 Jun 2014, at 0:41, > > wrote: I guess you want to solve for species and temperature using detailed chemistry and transport. Right? Von: > Antworten an: > Datum: Thursday, June 5, 2014 at 5:06 PM An: "nek5000-users at lists.mcs.anl.gov" > Betreff: Re: [Nek5000-users] weak derivative, dssum and binvm1 in cvode_driver Hi Paul and Stefan, Thank you for the explanations, things are going gradually more clear in my mind. So for a practical application, still in the context of cvode, I would like to add a new term to the RHS of the temperature equation. This new term is roughly (vdiff * grad (Y)) grad (T) where Y is a passive scalar, vdiff the diffusion coefficient of this passive scalar and T the temperature. Basically in the routine makeq.f the implementation should looks like to call wgradm1(Y_x, Y_y, Y_z, t(1,1,1,1,ifield+1), nelv) call dssum(grad_Y, Y_x, Y_y, Y_z) call col2(grad_Y,bintm1,ntot) call col2(grad_Y, vdiff(1,1,1,1,ifield+2) ,ntot ) call wgradm1(T_x, T_y, T_z, t(1,1,1,1,ifield), nelv) call dssum(grad_T, T_x, T_y, T_z) call col2(grad_T,grad_Y,ntot) call add2(bq(1,1,1,1,ifield), grad_T,ntot) and then convab and wlaplacian routines will add the other terms, and it will finish with call dssum(bq,nx1,ny1,nz1) call col2(bq,bintm1,ntot) call col2(bq,bm1,ntot) Am I right?? Thank you for your help ! Best regards, Emmanuel On 5 Jun 2014, at 19:25, > > wrote: Hi Emmanuel, Note that bintm1 and bm1 are not precise inverses of one another. bm1 is the unassembled mass matrix - i.e., it is the collection of local (to each element) mass matrices, each of which is diagonal. Conceptually, we denote the local mass matrix as B_L, for local. Then, the assembled mass matrix is: B := Q^T B_L Q where Q is the Boolean matrix that copies global degrees of freedom to their shared counterparts (i.e., copies a values to shared faces, edges, vertices, etc.). For the SEM, B_L is diagonal, as is B, so Binv := B^-1 is easily computed. Once the entries of this diagonal matrix are known, we can copy them to their element-based locations, so that we can generate B^-1 * r very easily. Often, products with these matrices, in conjunction with dssum, are used to generate continuous fields and that appears to be what is happening in this case. An example would be if you want to find a the continuous counterpart to a discontinuous function g. The usual projection approach is: Find gc \in H1 such that \int v gc dV = \int v g dV for all v in H1, which ends up looking like: Find gc \in H1 such that: (v,gc) = (v,g) for all g \in H1 or v B gc = v Q^T B_L g_L gc = B^-1 Q^T B_L g_L gc_L = Q B^-1 Q^T B_L g_L In Nek, the last statement is expressed as: call col2(g,bm1,n) call dssum(g,nx1,ny1,nz1) call col2(g,bintm1,n) In your cvode case, these statements are permuted because of the initial state of the data and the desired output (which is to be B*q -- which is why the variable is labeled bq). Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Thursday, June 05, 2014 2:38 AM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] weak derivative, dssum and binvm1 in cvode_driver Hi Emmanuel >From what I recall: CVODE solves the governing non-linear eqns in the strong form. That?s why we have to project every term of the RHS onto H2 (dssum and collocate with bintm1). The sum is projected again onto H2 because it gets devided by vtrans. Hope this helps. Cheers, Stefan Von: > Antworten an: > Datum: Thursday, June 5, 2014 at 9:20 AM An: "nek5000-users at lists.mcs.anl.gov" > Betreff: Re: [Nek5000-users] weak derivative, dssum and binvm1 in cvode_driver I?m adding another quick question: why in the routine makeq, under the cvode statement, there are these following 2 lines: call col2(bq,bintm1,ntot) call col2(bq,bm1,ntot) I?m not sure to understand why we are multiplying bq by the inverse of the mass matrix (bintm1) and just after multiplying it back by the mass matrix (bm1). Moreover, after leaving the makeq routine, fctfun will multiplying again ydot=bq/vtrans by the inverse of the mass matrix. Why all of these operations? Thank you for your help ! Best regards, Emmanuel On 5 Jun 2014, at 12:14, > > wrote: Dear Nek team, I have a quick question: in cvode_driver.f, in the routine fcvfun, do all the derivatives must be in weak formulation (using wgradm1) when constructing the right hand side term ydot? Because at the end of the routine fcvfun, dssum and multiplication by binvm1 are applied to the right hand side term ydot. It?s also not clear to me if I need to apply dssum and binvm1 for each derivative term appearing in my equation (in other terms, each time after calling wgradm1), or if I need to apply dssum and binvm1 only to the whole RHS term ydot ? I?m afraid of inconsistency if apply twice dssum and binvm1: one during the construction of operators and one on the final ydot term. Thank you for you help ! Best regards, Emmanuel _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing listNek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Jun 5 11:18:25 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 5 Jun 2014 16:18:25 +0000 Subject: [Nek5000-users] Create mesh for cylindrical domain Message-ID: Hello Neks, I'm simulating the 3D vortex breakdown problem in ~Nek/examples/vortex. However, I couldn't find the *.box file to create mesh for cylindrical domain. So I was wondering if anyone could provide me a *.box file for creating cylindrical domain. Thank you, Peng ************************* Peng Wang Ph.D. Candidate & Research Assistant Meteorology and Physical Oceanography Rosenstiel School of Marine and Atmospheric Science University of Miami 4600 Rickenbacker Causeway Miami, Florida 33149-1098, USA Web: http://www.rsmas.miami.edu/personal/pwang/ From nek5000-users at lists.mcs.anl.gov Thu Jun 5 12:22:44 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 5 Jun 2014 17:22:44 +0000 Subject: [Nek5000-users] Create mesh for cylindrical domain In-Reply-To: References: Message-ID: Hi Peng, You'll need to use prenek for this. I'll see if anyone has reasonable notes on how to go about it --- it's not very hard and just requires a bit of help to get started. Paul ________________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Thursday, June 05, 2014 11:18 AM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] Create mesh for cylindrical domain Hello Neks, I'm simulating the 3D vortex breakdown problem in ~Nek/examples/vortex. However, I couldn't find the *.box file to create mesh for cylindrical domain. So I was wondering if anyone could provide me a *.box file for creating cylindrical domain. Thank you, Peng ************************* Peng Wang Ph.D. Candidate & Research Assistant Meteorology and Physical Oceanography Rosenstiel School of Marine and Atmospheric Science University of Miami 4600 Rickenbacker Causeway Miami, Florida 33149-1098, USA Web: http://www.rsmas.miami.edu/personal/pwang/ _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Thu Jun 5 15:38:16 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 05 Jun 2014 23:38:16 +0300 Subject: [Nek5000-users] Create mesh for cylindrical domain In-Reply-To: References: Message-ID: Hi Peng, Paul, I am also interested in more general case, that is, a cone configuration in order to simulate a free jet flow. Thanks Barak On 06/05/2014 08:22 PM, nek5000-users at lists.mcs.anl.gov wrote: > > Hi Peng, > > You'll need to use prenek for this. I'll see if anyone has reasonable notes on > how to go about it --- it's not very hard and just requires a bit of help to get started. > > Paul > > ________________________________________ > From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > Sent: Thursday, June 05, 2014 11:18 AM > To: nek5000-users at lists.mcs.anl.gov > Subject: [Nek5000-users] Create mesh for cylindrical domain > > Hello Neks, > > I'm simulating the 3D vortex breakdown problem in ~Nek/examples/vortex. > However, I couldn't find the *.box file to create mesh for cylindrical domain. > So I was wondering if anyone could provide me a *.box file for creating cylindrical domain. > > Thank you, > Peng > > > > > ************************* > Peng Wang > > Ph.D. Candidate & Research Assistant > Meteorology and Physical Oceanography > Rosenstiel School of Marine and Atmospheric Science > University of Miami > 4600 Rickenbacker Causeway > Miami, Florida 33149-1098, USA > Web: http://www.rsmas.miami.edu/personal/pwang/ > > > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > From nek5000-users at lists.mcs.anl.gov Thu Jun 5 21:17:11 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 6 Jun 2014 10:17:11 +0800 Subject: [Nek5000-users] install NEK5000 on Mac Message-ID: Dear Sir I am new user of nek5000, and trying to install it on my macbook laptop. I am using OS X 10.9.3. I have installed Xcode from app store and also the gcc 4.8.1 with gfortran. but when I tried to build it with maketools all. I got error message as following. can anyone, tell me how to fix it? and actually I noticed some similar issue in the mail-list so I installed the home brewer. ./maketools all ---------------------- Make genmap... ---------------------- /usr/local/bin/gfortran -fdefault-real-8 -o /Users/zhang/bin/genmap genmap.o byte.o ld: in section __TEXT,__text reloc 62: length != 2 and X86_64_RELOC_GOT not supported file 'byte.o' for architecture x86_64 collect2: error: ld returned 1 exit status make[1]: *** [genmap] Error 1 make: *** [all] Error 1 /Wei -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Fri Jun 6 02:01:35 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 6 Jun 2014 07:01:35 +0000 Subject: [Nek5000-users] install NEK5000 on Mac In-Reply-To: References: Message-ID: Hello Wei, I encountered a similar issue on my mac once. Try setting the BIGMEM option to ?false? in the maketools script. Regards, Levi On 06 Jun 2014, at 04:17, > > wrote: Dear Sir I am new user of nek5000, and trying to install it on my macbook laptop. I am using OS X 10.9.3. I have installed Xcode from app store and also the gcc 4.8.1 with gfortran. but when I tried to build it with maketools all. I got error message as following. can anyone, tell me how to fix it? and actually I noticed some similar issue in the mail-list so I installed the home brewer. ./maketools all ---------------------- Make genmap... ---------------------- /usr/local/bin/gfortran -fdefault-real-8 -o /Users/zhang/bin/genmap genmap.o byte.o ld: in section __TEXT,__text reloc 62: length != 2 and X86_64_RELOC_GOT not supported file 'byte.o' for architecture x86_64 collect2: error: ld returned 1 exit status make[1]: *** [genmap] Error 1 make: *** [all] Error 1 /Wei _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Fri Jun 6 04:38:51 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 6 Jun 2014 17:38:51 +0800 Subject: [Nek5000-users] install NEK5000 on Mac In-Reply-To: References: Message-ID: Hi Levi. Thanks for replying and it works. cheers ---------------------------------------------- Zhang Wei waynezw0618 at gmail.com On 6 Jun, 2014, at 3:01 pm, nek5000-users at lists.mcs.anl.gov wrote: > Hello Wei, > > I encountered a similar issue on my mac once. Try setting the BIGMEM option to ?false? in the maketools script. > > Regards, > Levi > > On 06 Jun 2014, at 04:17, wrote: > >> Dear Sir >> I am new user of nek5000, and trying to install it on my macbook laptop. I am using OS X 10.9.3. I have installed Xcode from app store and also the gcc 4.8.1 with gfortran. but when I tried to build it with maketools all. I got error message as following. can anyone, tell me how to fix it? and actually I noticed some similar issue in the mail-list so I installed the home brewer. >> >> ./maketools all >> ---------------------- >> Make genmap... >> ---------------------- >> /usr/local/bin/gfortran -fdefault-real-8 -o /Users/zhang/bin/genmap genmap.o byte.o >> ld: in section __TEXT,__text reloc 62: length != 2 and X86_64_RELOC_GOT not supported file 'byte.o' for architecture x86_64 >> collect2: error: ld returned 1 exit status >> make[1]: *** [genmap] Error 1 >> make: *** [all] Error 1 >> >> >> /Wei >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Fri Jun 6 13:01:56 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 6 Jun 2014 18:01:56 +0000 Subject: [Nek5000-users] Create mesh for cylindrical domain In-Reply-To: References: Message-ID: Hi Paul and Barak, Thanks for the reply. Using ?genbox?, I have created a 2D annulus geometry with inner edges specified by ?o? (octagon). I guess the next step is to use Prenek to add elements into the central hollow of annulus and merge them. But I?m not sure how to finish this step? Best regards, Peng On Jun 6, 2014, at 1:00 PM, > > wrote: Hi Peng, Paul, I am also interested in more general case, that is, a cone configuration in order to simulate a free jet flow. Thanks Barak On 06/05/2014 08:22 PM, nek5000-users at lists.mcs.anl.gov wrote: Hi Peng, You'll need to use prenek for this. I'll see if anyone has reasonable notes on how to go about it --- it's not very hard and just requires a bit of help to get started. Paul ________________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf ofnek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Thursday, June 05, 2014 11:18 AM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] Create mesh for cylindrical domain Hello Neks, I'm simulating the 3D vortex breakdown problem in ~Nek/examples/vortex. However, I couldn't find the *.box file to create mesh for cylindrical domain. So I was wondering if anyone could provide me a *.box file for creating cylindrical domain. Thank you, Peng ************************* Peng Wang Ph.D. Candidate & Research Assistant Meteorology and Physical Oceanography Rosenstiel School of Marine and Atmospheric Science University of Miami 4600 Rickenbacker Causeway Miami, Florida 33149-1098, USA Web: http://www.rsmas.miami.edu/personal/pwang/ _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Fri Jun 6 15:21:55 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 6 Jun 2014 15:21:55 -0500 Subject: [Nek5000-users] Create mesh for cylindrical domain In-Reply-To: References: Message-ID: Hello all, I am new to nek. I have created a mesh using genbox. I want a run a simple case with 3d channel flow. I need information on giving the BC element wise for all the grid points. How to work on with .usr file. Thanks, Ravi Kiran Pendyala, On Fri, Jun 6, 2014 at 1:01 PM, wrote: > Hi Paul and Barak, > > Thanks for the reply. Using ?genbox?, I have created a 2D annulus > geometry with inner edges specified by > ?o? (octagon). I guess the next step is to use Prenek to add elements into > the central hollow of annulus and merge them. > But I?m not sure how to finish this step? > > Best regards, > Peng > > On Jun 6, 2014, at 1:00 PM, < > nek5000-users-request at lists.mcs.anl.gov> wrote: > > Hi Peng, Paul, > I am also interested in more general case, that is, a cone configuration > in order to simulate a free jet flow. > Thanks > Barak > > On 06/05/2014 08:22 PM, nek5000-users at lists.mcs.anl.gov wrote: > > > Hi Peng, > > You'll need to use prenek for this. I'll see if anyone has reasonable > notes on > how to go about it --- it's not very hard and just requires a bit of help > to get started. > > Paul > > ________________________________________ > From: nek5000-users-bounces at lists.mcs.anl.gov [ > nek5000-users-bounces at lists.mcs.anl.gov] on behalf of > nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > > Sent: Thursday, June 05, 2014 11:18 AM > To: nek5000-users at lists.mcs.anl.gov > Subject: [Nek5000-users] Create mesh for cylindrical domain > > Hello Neks, > > I'm simulating the 3D vortex breakdown problem in ~Nek/examples/vortex. > However, I couldn't find the *.box file to create mesh for cylindrical > domain. > So I was wondering if anyone could provide me a *.box file for creating > cylindrical domain. > > Thank you, > Peng > > > > > ************************* > Peng Wang > > Ph.D. Candidate & Research Assistant > Meteorology and Physical Oceanography > Rosenstiel School of Marine and Atmospheric Science > University of Miami > 4600 Rickenbacker Causeway > Miami, Florida 33149-1098, USA > Web: http://www.rsmas.miami.edu/personal/pwang/ > > > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Fri Jun 6 21:47:47 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sat, 7 Jun 2014 10:47:47 +0800 Subject: [Nek5000-users] how to get vorticity in the post processing Message-ID: Hi Neks Could any one tell me how to get vorticity in the NEK5000 for post processing? I also want to know if it is in the element level or global level. For my understanding, I suppose NEK5000 do things in C0 space, how could one enforce the continuity in first order derivative? Thanks Yours Sincerely ------------------------ Wei Zhang Ph.D From nek5000-users at lists.mcs.anl.gov Fri Jun 6 21:56:31 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 6 Jun 2014 21:56:31 -0500 (CDT) Subject: [Nek5000-users] how to get vorticity in the post processing In-Reply-To: References: Message-ID: On Fri, 6 Jun 2014, nek5000-users at lists.mcs.anl.gov wrote: > Hi Neks > Could any one tell me how to get vorticity in the NEK5000 for post > processing? I also want to know if it is in the element level or global > level. For my understanding, I suppose NEK5000 do things in C0 space, how > could one enforce the continuity in first order derivative? > > Thanks > > Yours Sincerely > ------------------------ > Wei Zhang > Ph.D Hi Wei, I would do the following from userchk: parameter (lt=lx1*ly1*lz1*lelt) common /myvort/ v1(lt),v2(lt),v3(lt) if (mod(istep,iostep).eq.0) then call comp_vort3(v1,v2,v3,vx,vy,vz) call outpost(v1,v2,v3,pr,t,'vrt') endif The result will be put into a file vrtsample0.f00001, etc., if your session name is "sample"... You can then visualize this field in VisIt. If you look at the source for comp_vort3 in navier5.f you will see that the returned field is averaged at the interfaces in order to make it continuous. Paul From nek5000-users at lists.mcs.anl.gov Fri Jun 6 22:14:52 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sat, 7 Jun 2014 11:14:52 +0800 Subject: [Nek5000-users] how to get vorticity in the post processing In-Reply-To: References: Message-ID: Hi Paul Thanks for replying so soon. I want to know how does comp_vort3 enforce that. If it just do average at element interface? Then it won't be so smooth, right? Yours Sincerely ------------------------ Wei Zhang Ph.D On 2014-6-7, at ??10:56, nek5000-users at lists.mcs.anl.gov wrote: > > > > On Fri, 6 Jun 2014, nek5000-users at lists.mcs.anl.gov wrote: > >> Hi Neks >> Could any one tell me how to get vorticity in the NEK5000 for post >> processing? I also want to know if it is in the element level or global >> level. For my understanding, I suppose NEK5000 do things in C0 space, how >> could one enforce the continuity in first order derivative? >> >> Thanks >> >> Yours Sincerely >> ------------------------ >> Wei Zhang >> Ph.D > > Hi Wei, > > I would do the following from userchk: > > parameter (lt=lx1*ly1*lz1*lelt) > common /myvort/ v1(lt),v2(lt),v3(lt) > > if (mod(istep,iostep).eq.0) then > call comp_vort3(v1,v2,v3,vx,vy,vz) > call outpost(v1,v2,v3,pr,t,'vrt') > endif > > The result will be put into a file vrtsample0.f00001, etc., > if your session name is "sample"... You can then > visualize this field in VisIt. > > If you look at the source for comp_vort3 in navier5.f you > will see that the returned field is averaged at the interfaces in order to make it continuous. > > Paul > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Fri Jun 6 22:18:11 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sat, 7 Jun 2014 03:18:11 +0000 Subject: [Nek5000-users] how to get vorticity in the post processing In-Reply-To: References: , Message-ID: Right -- not so smooth. Personally, I wouldn't enforce it... it somewhat depends on what you want to do with the vorticity. If it's nearly continuous, then the interface averaging will not be detrimental in any case. Paul ________________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Friday, June 06, 2014 10:14 PM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] how to get vorticity in the post processing Hi Paul Thanks for replying so soon. I want to know how does comp_vort3 enforce that. If it just do average at element interface? Then it won't be so smooth, right? Yours Sincerely ------------------------ Wei Zhang Ph.D On 2014-6-7, at ??10:56, nek5000-users at lists.mcs.anl.gov wrote: > > > > On Fri, 6 Jun 2014, nek5000-users at lists.mcs.anl.gov wrote: > >> Hi Neks >> Could any one tell me how to get vorticity in the NEK5000 for post >> processing? I also want to know if it is in the element level or global >> level. For my understanding, I suppose NEK5000 do things in C0 space, how >> could one enforce the continuity in first order derivative? >> >> Thanks >> >> Yours Sincerely >> ------------------------ >> Wei Zhang >> Ph.D > > Hi Wei, > > I would do the following from userchk: > > parameter (lt=lx1*ly1*lz1*lelt) > common /myvort/ v1(lt),v2(lt),v3(lt) > > if (mod(istep,iostep).eq.0) then > call comp_vort3(v1,v2,v3,vx,vy,vz) > call outpost(v1,v2,v3,pr,t,'vrt') > endif > > The result will be put into a file vrtsample0.f00001, etc., > if your session name is "sample"... You can then > visualize this field in VisIt. > > If you look at the source for comp_vort3 in navier5.f you > will see that the returned field is averaged at the interfaces in order to make it continuous. > > Paul > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Sat Jun 7 04:48:41 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sat, 7 Jun 2014 11:48:41 +0200 Subject: [Nek5000-users] gmsh to nek converter Message-ID: Dear neks Using a code from here https://bitbucket.org/mikael_mortensen/nek5000-tools we wrote a converter from gmsh to rea format. You can find it here https://bitbucket.org/cpraveen/nek5000 I would be very keen to have others try it out and tell us if there are any bugs. Currently it works only for 2d meshes. It can also create circular faces. See inside gmsh2nek directory. The karman.geo example can be tested together with the setup files from here https://code.google.com/p/cfdlab/source/browse/trunk/nek5000/cyl_turek/ Replace the mesh in cyl.rea with the mesh created in karman.rea To generate karman.rea do the following (use latest Gmsh software) gmsh -2 karman.geo python karman.py Best praveen -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Sun Jun 8 04:51:27 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 8 Jun 2014 11:51:27 +0200 Subject: [Nek5000-users] gmsh to nek converter In-Reply-To: References: Message-ID: Hi Praveen, Thanks for you supply this work for us, I met a error when I follow your introductions, like this python karman.py Traceback (most recent call last): File "karman.py", line 1, in from mshconvert import * File "/home/wei/Desktop/nek5000/ext_cyl_gmsh/mshconvert.py", line 6, in from numpy import zeros, array, sign, cross, dot, ones, arctan, sin, cos, pi, mod, sqrt ImportError: No module named numpy I don't know which part I missed. would you help me? Thanks Wei 2014-06-07 11:48 GMT+02:00 : > Dear neks > Using a code from here > https://bitbucket.org/mikael_mortensen/nek5000-tools we wrote a converter > from gmsh to rea format. You can find it here > > https://bitbucket.org/cpraveen/nek5000 > > I would be very keen to have others try it out and tell us if there are > any bugs. Currently it works only for 2d meshes. It can also create > circular faces. > > See inside gmsh2nek directory. The karman.geo example can be tested > together with the setup files from here > > https://code.google.com/p/cfdlab/source/browse/trunk/nek5000/cyl_turek/ > > Replace the mesh in cyl.rea with the mesh created in karman.rea > > To generate karman.rea do the following (use latest Gmsh software) > > gmsh -2 karman.geo > python karman.py > > Best > praveen > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > -- ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~ BEST REGARDS! *??* *He Wei* -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Sun Jun 8 06:13:42 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 8 Jun 2014 13:13:42 +0200 Subject: [Nek5000-users] gmsh to nek converter In-Reply-To: References: Message-ID: On Sun, Jun 8, 2014 at 11:51 AM, wrote: > Hi Praveen, > > Thanks for you supply this work for us, I met a error when I follow your > introductions, like this > > python karman.py > Traceback (most recent call last): > File "karman.py", line 1, in > from mshconvert import * > File "/home/wei/Desktop/nek5000/ext_cyl_gmsh/mshconvert.py", line 6, in > > from numpy import zeros, array, sign, cross, dot, ones, arctan, sin, > cos, pi, mod, sqrt > ImportError: No module named numpy > > I don't know which part I missed. would you help me? > > Thanks > > Wei > Hi You have to install numpy. Since this is not completely nek related question, you can email me directly at cpraveen at gmail.com Best praveen -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Sun Jun 8 08:40:43 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 8 Jun 2014 21:40:43 +0800 Subject: [Nek5000-users] quasi 3D and boundary condition Message-ID: Hi Everyone. I am trying to run the flow past a cylinder case. I am going to move to the 3D simulation for my study. I have two questions: 1) how to run quasi 3D simulation in nek5000 ? if there is not existing code, andy suggestion to how to implement so? 2) how to specify the normal and tangential boundary condition for a curvature boundary? cheers ---------------------------------------------- Zhang Wei waynezw0618 at gmail.com From nek5000-users at lists.mcs.anl.gov Sun Jun 8 09:44:36 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 8 Jun 2014 14:44:36 +0000 Subject: [Nek5000-users] quasi 3D and boundary condition In-Reply-To: References: Message-ID: Hi Zhang, You can use periodic boundary conditions in the z direction, provided you have at least 3 elements in z. Prescribed boundary conditions are given in Cartesian coordinates. If you have the "mv " bc on your moving surface (i.e., the cylinder surface), along with the following things lx2=lx1-2 ly2=ly1-2 lz2=lz1-2 parameter (lx1m=lx1,ly1m=ly1,lz1m=lz1) in SIZE, and T ifstrs, T ifmvbd in the .rea file, then the mesh will move with the fluid velocity (which you prescribe as Cartesian velocity vectors, u,v,w). Note that nek uses an ALE formulation and the mesh motion must relatively limited or the mesh becomes too distorted. For an oscillating cylinder, this should be ok (see www.mcs.anl.gov/~fischer/ocyl.gif). I've just added a 2D oscillating cylinder case that illustrates the basic procedure to the examples suite. Paul ________________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Sunday, June 08, 2014 8:40 AM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] quasi 3D and boundary condition Hi Everyone. I am trying to run the flow past a cylinder case. I am going to move to the 3D simulation for my study. I have two questions: 1) how to run quasi 3D simulation in nek5000 ? if there is not existing code, andy suggestion to how to implement so? 2) how to specify the normal and tangential boundary condition for a curvature boundary? cheers ---------------------------------------------- Zhang Wei waynezw0618 at gmail.com _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Sun Jun 8 10:03:41 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 8 Jun 2014 23:03:41 +0800 Subject: [Nek5000-users] quasi 3D and boundary condition In-Reply-To: References: Message-ID: Hi Paul Thanks for replying. for quasi-2D, I mean I wish to define the velocity u(x,y,z) as sum(u(x,y,k)e^kz) to reduce the computational cost for really 3D case and also to avoid the long wave (which may longer then the geometry size in the z direction) in the axial direction.does nek currently support such feature? for prescribe the bc on curl surface, I mean something like non-immersed bc and and have velocity component in the tangential direction, like in the potential theory. cheers ---------------------------------------------- Zhang Wei waynezw0618 at gmail.com On 8 Jun, 2014, at 10:44 pm, nek5000-users at lists.mcs.anl.gov wrote: > > Hi Zhang, > > You can use periodic boundary conditions in the z direction, provided you have at least 3 > elements in z. > > Prescribed boundary conditions are given in Cartesian coordinates. If you have the "mv " > bc on your moving surface (i.e., the cylinder surface), along with the following things > > lx2=lx1-2 > ly2=ly1-2 > lz2=lz1-2 > > parameter (lx1m=lx1,ly1m=ly1,lz1m=lz1) > > in SIZE, and T ifstrs, T ifmvbd in the .rea file, then the mesh will move with the fluid > velocity (which you prescribe as Cartesian velocity vectors, u,v,w). Note that nek > uses an ALE formulation and the mesh motion must relatively limited or the mesh > becomes too distorted. For an oscillating cylinder, this should be ok (see > www.mcs.anl.gov/~fischer/ocyl.gif). I've just added a 2D oscillating cylinder case > that illustrates the basic procedure to the examples suite. > > Paul > > > > ________________________________________ > From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > Sent: Sunday, June 08, 2014 8:40 AM > To: nek5000-users at lists.mcs.anl.gov > Subject: [Nek5000-users] quasi 3D and boundary condition > > Hi Everyone. > I am trying to run the flow past a cylinder case. I am going to move to the 3D simulation for my study. I have two questions: > 1) how to run quasi 3D simulation in nek5000 ? if there is not existing code, andy suggestion to how to implement so? > 2) how to specify the normal and tangential boundary condition for a curvature boundary? > > > cheers > ---------------------------------------------- > Zhang Wei > waynezw0618 at gmail.com > > > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Sun Jun 8 15:15:59 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 8 Jun 2014 20:15:59 +0000 Subject: [Nek5000-users] quasi 3D and boundary condition In-Reply-To: References: , Message-ID: Hi Zhang, There is no support for 2.5D with Fourier in z and currently no plans to move in that direction. If you want a slip velocity on the curved surface you should use the stress formulation (lx2=lx1-2, etc., with ifstrs T. Then the "SYM" bc should give you the desired bc, i.e., U.nhat = 0, d/dn (U.t_hat) = 0. Paul _______________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Sunday, June 08, 2014 10:03 AM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] quasi 3D and boundary condition Hi Paul Thanks for replying. for quasi-2D, I mean I wish to define the velocity u(x,y,z) as sum(u(x,y,k)e^kz) to reduce the computational cost for really 3D case and also to avoid the long wave (which may longer then the geometry size in the z direction) in the axial direction.does nek currently support such feature? for prescribe the bc on curl surface, I mean something like non-immersed bc and and have velocity component in the tangential direction, like in the potential theory. cheers ---------------------------------------------- Zhang Wei waynezw0618 at gmail.com On 8 Jun, 2014, at 10:44 pm, nek5000-users at lists.mcs.anl.gov wrote: > > Hi Zhang, > > You can use periodic boundary conditions in the z direction, provided you have at least 3 > elements in z. > > Prescribed boundary conditions are given in Cartesian coordinates. If you have the "mv " > bc on your moving surface (i.e., the cylinder surface), along with the following things > > lx2=lx1-2 > ly2=ly1-2 > lz2=lz1-2 > > parameter (lx1m=lx1,ly1m=ly1,lz1m=lz1) > > in SIZE, and T ifstrs, T ifmvbd in the .rea file, then the mesh will move with the fluid > velocity (which you prescribe as Cartesian velocity vectors, u,v,w). Note that nek > uses an ALE formulation and the mesh motion must relatively limited or the mesh > becomes too distorted. For an oscillating cylinder, this should be ok (see > www.mcs.anl.gov/~fischer/ocyl.gif). I've just added a 2D oscillating cylinder case > that illustrates the basic procedure to the examples suite. > > Paul > > > > ________________________________________ > From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > Sent: Sunday, June 08, 2014 8:40 AM > To: nek5000-users at lists.mcs.anl.gov > Subject: [Nek5000-users] quasi 3D and boundary condition > > Hi Everyone. > I am trying to run the flow past a cylinder case. I am going to move to the 3D simulation for my study. I have two questions: > 1) how to run quasi 3D simulation in nek5000 ? if there is not existing code, andy suggestion to how to implement so? > 2) how to specify the normal and tangential boundary condition for a curvature boundary? > > > cheers > ---------------------------------------------- > Zhang Wei > waynezw0618 at gmail.com > > > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Mon Jun 9 02:30:07 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 9 Jun 2014 11:30:07 +0400 Subject: [Nek5000-users] Time-dependant boundary condition In-Reply-To: References: Message-ID: How should I impose time-dependant BC for velocity on the left vertical boundaty for a 2D box geometry. The velocity profile should be Vx=cos(pi*y)*cos(2*pi*t) Vy=0 To illustrate the idea here are the pictures. Instead of constant velocity Vx=c on the left (inflow) boundary of a channel V __________________ | | | |__________________ I would impose Vx=cos(pi*y)*cos(2*pi*t) so for t = 0 velocity profile is ____________________ \ \ \ \_________________ for t=1 velocity profile is _________________ / / / /____________________ and so on. I know it should be possible in nek5000, but still not very familiar with syntax and fortran. Thank you in advance. From nek5000-users at lists.mcs.anl.gov Mon Jun 9 07:05:57 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 9 Jun 2014 12:05:57 +0000 Subject: [Nek5000-users] Time-dependant boundary condition In-Reply-To: References: , Message-ID: In userbc: ux = cos(pi*y)*cos(2.*pi*time) uy = 0. Paul ________________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Monday, June 09, 2014 2:30 AM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] Time-dependant boundary condition How should I impose time-dependant BC for velocity on the left vertical boundaty for a 2D box geometry. The velocity profile should be Vx=cos(pi*y)*cos(2*pi*t) Vy=0 To illustrate the idea here are the pictures. Instead of constant velocity Vx=c on the left (inflow) boundary of a channel V __________________ | | | |__________________ I would impose Vx=cos(pi*y)*cos(2*pi*t) so for t = 0 velocity profile is ____________________ \ \ \ \_________________ for t=1 velocity profile is _________________ / / / /____________________ and so on. I know it should be possible in nek5000, but still not very familiar with syntax and fortran. Thank you in advance. _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Tue Jun 10 10:16:28 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 10 Jun 2014 11:16:28 -0400 Subject: [Nek5000-users] volumetric heat source w/ inflow Message-ID: Hello all, I am working on a problem consisting of an axially-horizontal cylindrical tank with an inlet (an opening) at its top and a connected pipe to its bottom as an outlet. The boundary conditions are set accordingly, i.e., inflow and outflow, respectively. There is no problem with isothermal simulation of such configuration. However, when volumetric heat source is added to the fluid domain (via userq2 subroutine), non-physical temperatures have been observed at the walls (w/ adiabatic BC) in the immediate vicinity of the inflow (w/ Dirichlet temperature BC). In fact, the element nodes close to the inlet have very high or very low temperatures, which are no expected. I am wondering if anyone has any experience/hint on this issue. Thanks, Mohsen From nek5000-users at lists.mcs.anl.gov Tue Jun 10 11:01:46 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 10 Jun 2014 16:01:46 +0000 Subject: [Nek5000-users] volumetric heat source w/ inflow In-Reply-To: References: Message-ID: Hi Mohsen, userq2 is used only with MOAB -- use qvol in userq instead -- see, e.g. examples/conj_ht/conj_ht.usr but without condition on nelgv Best. Aleks ________________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Tuesday, June 10, 2014 10:16 AM To: Nek 5000 Subject: [Nek5000-users] volumetric heat source w/ inflow Hello all, I am working on a problem consisting of an axially-horizontal cylindrical tank with an inlet (an opening) at its top and a connected pipe to its bottom as an outlet. The boundary conditions are set accordingly, i.e., inflow and outflow, respectively. There is no problem with isothermal simulation of such configuration. However, when volumetric heat source is added to the fluid domain (via userq2 subroutine), non-physical temperatures have been observed at the walls (w/ adiabatic BC) in the immediate vicinity of the inflow (w/ Dirichlet temperature BC). In fact, the element nodes close to the inlet have very high or very low temperatures, which are no expected. I am wondering if anyone has any experience/hint on this issue. Thanks, Mohsen _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Tue Jun 10 11:03:35 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 10 Jun 2014 12:03:35 -0400 Subject: [Nek5000-users] volumetric heat source w/ inflow In-Reply-To: References: Message-ID: Hi Aleks, I should have mentioned in my previous email that I am actually using MOAB. Thanks, Mohsen On 10-Jun-14, at 12:01 PM, wrote: > Hi Mohsen, > > userq2 is used only with MOAB -- use qvol in userq instead -- see, > e.g. examples/conj_ht/conj_ht.usr but without condition on nelgv > > Best. > Aleks > > > ________________________________________ > From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users- > bounces at lists.mcs.anl.gov] on behalf of nek5000- > users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > Sent: Tuesday, June 10, 2014 10:16 AM > To: Nek 5000 > Subject: [Nek5000-users] volumetric heat source w/ inflow > > Hello all, > I am working on a problem consisting of an axially-horizontal > cylindrical tank with an inlet (an opening) at its top and a > connected pipe to its bottom as an outlet. The boundary conditions > are set accordingly, i.e., inflow and outflow, respectively. There is > no problem with isothermal simulation of such configuration. However, > when volumetric heat source is added to the fluid domain (via userq2 > subroutine), non-physical temperatures have been observed at the > walls (w/ adiabatic BC) in the immediate vicinity of the inflow (w/ > Dirichlet temperature BC). In fact, the element nodes close to the > inlet have very high or very low temperatures, which are no expected. > > I am wondering if anyone has any experience/hint on this issue. > > Thanks, > Mohsen > > > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Tue Jun 10 11:27:29 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 10 Jun 2014 16:27:29 +0000 Subject: [Nek5000-users] volumetric heat source w/ inflow In-Reply-To: References: , Message-ID: Hi Mohsen, One way I usually check my MOAB setups is by running the Nek's version of it. For this one needs to get Mesh & BC by calling gen_rea(2) from say userchk, add the missing parameters to create .rea file, run genmap for .map file and fill q array in userq2() routine by calling the latter from userq() say once per timestep Aleks ________________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Tuesday, June 10, 2014 11:03 AM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] volumetric heat source w/ inflow Hi Aleks, I should have mentioned in my previous email that I am actually using MOAB. Thanks, Mohsen On 10-Jun-14, at 12:01 PM, wrote: > Hi Mohsen, > > userq2 is used only with MOAB -- use qvol in userq instead -- see, > e.g. examples/conj_ht/conj_ht.usr but without condition on nelgv > > Best. > Aleks > > > ________________________________________ > From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users- > bounces at lists.mcs.anl.gov] on behalf of nek5000- > users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > Sent: Tuesday, June 10, 2014 10:16 AM > To: Nek 5000 > Subject: [Nek5000-users] volumetric heat source w/ inflow > > Hello all, > I am working on a problem consisting of an axially-horizontal > cylindrical tank with an inlet (an opening) at its top and a > connected pipe to its bottom as an outlet. The boundary conditions > are set accordingly, i.e., inflow and outflow, respectively. There is > no problem with isothermal simulation of such configuration. However, > when volumetric heat source is added to the fluid domain (via userq2 > subroutine), non-physical temperatures have been observed at the > walls (w/ adiabatic BC) in the immediate vicinity of the inflow (w/ > Dirichlet temperature BC). In fact, the element nodes close to the > inlet have very high or very low temperatures, which are no expected. > > I am wondering if anyone has any experience/hint on this issue. > > Thanks, > Mohsen > > > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Tue Jun 10 12:23:18 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 10 Jun 2014 19:23:18 +0200 Subject: [Nek5000-users] problems running in parallel Message-ID: Dear users, I am trying to simulate the flow past a cylinder. If I run my simulation with lelt=2000, lelg=2000 in 1 processor, everything works fine. However, if I increase the resolution to lelt=4200 I get a compilation error. Following this post: http://lists.mcs.anl.gov/pipermail/nek5000-users/2013-April/002101.html I have seen that if I use more processors, the code compiles fine. However, now I am not able to run the code using 4 processors. I get the following error: Number of processors: 1 REAL wdsize : 8 INTEGER wdsize : 4 Beginning session: /SL/nek5_svn/test/cyl/cyl.rea timer accuracy: 1.1920929E-07 sec read .rea file Beginning session: /SL/nek5_svn/test/cyl/cyl.rea timer accuracy: 9.5367432E-08 sec read .rea file nelgt/nelgv/lelt: 4425 4425 2000 lx1 /lx2 /lx3 : 5 5 5 ABORT: Problem size too large! This solver has been compiled for: number of elements/proc (lelt): 2000 total number of elements (lelg): 5000 Recompile with the following SIZE parameters: lelt >= 4425 for np = 1 lelg >= 4425 I have a 3d mesh with 4425 elemnts. In the SIZE file I have set: parameter (ldim=3) parameter (lx1=5,ly1=lx1,lz1=lx1,lelt=2000,lelv=lelt) parameter (lxd=(3*lx1)/2,lyd=lxd,lzd=lxd) parameter (lelx=1,lely=lelx,lelz=lely) parameter (lx2=lx1-0) ! Pressure array dimensions parameter (ly2=ly1-0) parameter (lz2=lz1-0) parameter (lx3=lx2) parameter (ly3=ly2) parameter (lz3=lz2) parameter (lp = 4) ! Max # processors parameter (lelg = 5000) ! Max # elements, total parameter (lzl=3 + 2*(ldim-3)) I have tried to follow this post to solve the problem, but I couldn't: https://lists.mcs.anl.gov/mailman/htdig/nek5000-users/2013-December/002411.html Could you help me, please? Regards, SL From nek5000-users at lists.mcs.anl.gov Tue Jun 10 12:32:12 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 10 Jun 2014 19:32:12 +0200 Subject: [Nek5000-users] problems running in parallel In-Reply-To: References: Message-ID: You seem to be running on a single proc. You have to start the program using one one of the scripts nekmpi or nekbmpi E.g. nekmpi jobname 4 to run with 4 procs. praveen On Tue, Jun 10, 2014 at 7:23 PM, wrote: > Dear users, > > I am trying to simulate the flow past a cylinder. If I run my simulation > with lelt=2000, lelg=2000 in 1 processor, everything works fine. However, > if I increase the resolution to lelt=4200 I get a compilation error. > > Following this post: > > http://lists.mcs.anl.gov/pipermail/nek5000-users/2013-April/002101.html > > I have seen that if I use more processors, the code compiles fine. > > However, now I am not able to run the code using 4 processors. I get the > following error: > > Number of processors: 1 > REAL wdsize : 8 > INTEGER wdsize : 4 > > > Beginning session: > /SL/nek5_svn/test/cyl/cyl.rea > > > timer accuracy: 1.1920929E-07 sec > > read .rea file > > > Beginning session: > /SL/nek5_svn/test/cyl/cyl.rea > > > timer accuracy: 9.5367432E-08 sec > > read .rea file > nelgt/nelgv/lelt: 4425 4425 2000 > lx1 /lx2 /lx3 : 5 5 5 > > > ABORT: Problem size too large! > > This solver has been compiled for: > number of elements/proc (lelt): 2000 > total number of elements (lelg): 5000 > > Recompile with the following SIZE parameters: > lelt >= 4425 for np = 1 > lelg >= 4425 > > > > I have a 3d mesh with 4425 elemnts. In the SIZE file I have set: > > > parameter (ldim=3) > parameter (lx1=5,ly1=lx1,lz1=lx1,lelt=2000,lelv=lelt) > parameter (lxd=(3*lx1)/2,lyd=lxd,lzd=lxd) > parameter (lelx=1,lely=lelx,lelz=lely) > > parameter (lx2=lx1-0) ! Pressure array dimensions > parameter (ly2=ly1-0) > parameter (lz2=lz1-0) > > parameter (lx3=lx2) > parameter (ly3=ly2) > parameter (lz3=lz2) > > parameter (lp = 4) ! Max # processors > parameter (lelg = 5000) ! Max # elements, total > > parameter (lzl=3 + 2*(ldim-3)) > > I have tried to follow this post to solve the problem, but I couldn't: > > https://lists.mcs.anl.gov/mailman/htdig/nek5000-users/ > 2013-December/002411.html > > Could you help me, please? > > Regards, > > SL > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Jun 10 12:38:19 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 10 Jun 2014 19:38:19 +0200 Subject: [Nek5000-users] problems running in parallel In-Reply-To: References: Message-ID: Hi, Note also that sometime, for unknown reason, mpiexec does not work correctly on certain platforms and you should use instead mpiexec.mpich2 That has solved the problem for me few months ago. ++ JC 2014-06-10 19:32 GMT+02:00 : > You seem to be running on a single proc. You have to start the program > using one one of the scripts > > nekmpi > > or > > nekbmpi > > E.g. > > nekmpi jobname 4 > > to run with 4 procs. > > praveen > > > On Tue, Jun 10, 2014 at 7:23 PM, wrote: > >> Dear users, >> >> I am trying to simulate the flow past a cylinder. If I run my simulation >> with lelt=2000, lelg=2000 in 1 processor, everything works fine. However, >> if I increase the resolution to lelt=4200 I get a compilation error. >> >> Following this post: >> >> http://lists.mcs.anl.gov/pipermail/nek5000-users/2013-April/002101.html >> >> I have seen that if I use more processors, the code compiles fine. >> >> However, now I am not able to run the code using 4 processors. I get the >> following error: >> >> Number of processors: 1 >> REAL wdsize : 8 >> INTEGER wdsize : 4 >> >> >> Beginning session: >> /SL/nek5_svn/test/cyl/cyl.rea >> >> >> timer accuracy: 1.1920929E-07 sec >> >> read .rea file >> >> >> Beginning session: >> /SL/nek5_svn/test/cyl/cyl.rea >> >> >> timer accuracy: 9.5367432E-08 sec >> >> read .rea file >> nelgt/nelgv/lelt: 4425 4425 2000 >> lx1 /lx2 /lx3 : 5 5 5 >> >> >> ABORT: Problem size too large! >> >> This solver has been compiled for: >> number of elements/proc (lelt): 2000 >> total number of elements (lelg): 5000 >> >> Recompile with the following SIZE parameters: >> lelt >= 4425 for np = 1 >> lelg >= 4425 >> >> >> >> I have a 3d mesh with 4425 elemnts. In the SIZE file I have set: >> >> >> parameter (ldim=3) >> parameter (lx1=5,ly1=lx1,lz1=lx1,lelt=2000,lelv=lelt) >> parameter (lxd=(3*lx1)/2,lyd=lxd,lzd=lxd) >> parameter (lelx=1,lely=lelx,lelz=lely) >> >> parameter (lx2=lx1-0) ! Pressure array dimensions >> parameter (ly2=ly1-0) >> parameter (lz2=lz1-0) >> >> parameter (lx3=lx2) >> parameter (ly3=ly2) >> parameter (lz3=lz2) >> >> parameter (lp = 4) ! Max # processors >> parameter (lelg = 5000) ! Max # elements, total >> >> parameter (lzl=3 + 2*(ldim-3)) >> >> I have tried to follow this post to solve the problem, but I couldn't: >> >> https://lists.mcs.anl.gov/mailman/htdig/nek5000-users/ >> 2013-December/002411.html >> >> Could you help me, please? >> >> Regards, >> >> SL >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> > > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > -- Jean-Christophe Loiseau Homepage -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Jun 10 12:55:24 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 10 Jun 2014 13:55:24 -0400 Subject: [Nek5000-users] volumetric heat source w/ inflow In-Reply-To: References: , Message-ID: Thanks Aleks for your suggestion. So you think it might be because of some issue with MOAB. I'll check this out, though, apparently, I haven't had any problem reading the mesh and sidesets into Nek via MOAB. Mohsen On 10-Jun-14, at 12:27 PM, wrote: > Hi Mohsen, > > One way I usually check my MOAB setups is by running the Nek's > version of it. > > For this one needs to get Mesh & BC by calling gen_rea(2) from say > userchk, add the missing parameters to create .rea file, run genmap > for .map file and fill q array in userq2() routine by calling the > latter from userq() say once per timestep > > Aleks > > > > ________________________________________ > From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users- > bounces at lists.mcs.anl.gov] on behalf of nek5000- > users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > Sent: Tuesday, June 10, 2014 11:03 AM > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] volumetric heat source w/ inflow > > Hi Aleks, > I should have mentioned in my previous email that I am actually using > MOAB. > > Thanks, > Mohsen > > On 10-Jun-14, at 12:01 PM, wrote: > >> Hi Mohsen, >> >> userq2 is used only with MOAB -- use qvol in userq instead -- see, >> e.g. examples/conj_ht/conj_ht.usr but without condition on nelgv >> >> Best. >> Aleks >> >> >> ________________________________________ >> From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users- >> bounces at lists.mcs.anl.gov] on behalf of nek5000- >> users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] >> Sent: Tuesday, June 10, 2014 10:16 AM >> To: Nek 5000 >> Subject: [Nek5000-users] volumetric heat source w/ inflow >> >> Hello all, >> I am working on a problem consisting of an axially-horizontal >> cylindrical tank with an inlet (an opening) at its top and a >> connected pipe to its bottom as an outlet. The boundary conditions >> are set accordingly, i.e., inflow and outflow, respectively. There is >> no problem with isothermal simulation of such configuration. However, >> when volumetric heat source is added to the fluid domain (via userq2 >> subroutine), non-physical temperatures have been observed at the >> walls (w/ adiabatic BC) in the immediate vicinity of the inflow (w/ >> Dirichlet temperature BC). In fact, the element nodes close to the >> inlet have very high or very low temperatures, which are no expected. >> >> I am wondering if anyone has any experience/hint on this issue. >> >> Thanks, >> Mohsen >> >> >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Tue Jun 10 17:10:44 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 10 Jun 2014 18:10:44 -0400 Subject: [Nek5000-users] volumetric heat source w/ inflow In-Reply-To: References: , Message-ID: Hi Aleks, As a follow up on the following post, I just wanted to note that the results of Nek's version of my setup agreed exactly with the MOAB counterpart, and so the aforementioned issue has different origin. Thanks, Mohsen On 10-Jun-14, at 1:55 PM, Mohsen Behzad wrote: > Thanks Aleks for your suggestion. > So you think it might be because of some issue with MOAB. I'll > check this out, though, apparently, I haven't had any problem > reading the mesh and sidesets into Nek via MOAB. > > Mohsen > > > On 10-Jun-14, at 12:27 PM, wrote: > >> Hi Mohsen, >> >> One way I usually check my MOAB setups is by running the Nek's >> version of it. >> >> For this one needs to get Mesh & BC by calling gen_rea(2) from say >> userchk, add the missing parameters to create .rea file, run >> genmap for .map file and fill q array in userq2() routine by >> calling the latter from userq() say once per timestep >> >> Aleks >> >> >> >> ________________________________________ >> From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users- >> bounces at lists.mcs.anl.gov] on behalf of nek5000- >> users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] >> Sent: Tuesday, June 10, 2014 11:03 AM >> To: nek5000-users at lists.mcs.anl.gov >> Subject: Re: [Nek5000-users] volumetric heat source w/ inflow >> >> Hi Aleks, >> I should have mentioned in my previous email that I am actually using >> MOAB. >> >> Thanks, >> Mohsen >> >> On 10-Jun-14, at 12:01 PM, wrote: >> >>> Hi Mohsen, >>> >>> userq2 is used only with MOAB -- use qvol in userq instead -- see, >>> e.g. examples/conj_ht/conj_ht.usr but without condition on nelgv >>> >>> Best. >>> Aleks >>> >>> >>> ________________________________________ >>> From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users- >>> bounces at lists.mcs.anl.gov] on behalf of nek5000- >>> users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] >>> Sent: Tuesday, June 10, 2014 10:16 AM >>> To: Nek 5000 >>> Subject: [Nek5000-users] volumetric heat source w/ inflow >>> >>> Hello all, >>> I am working on a problem consisting of an axially-horizontal >>> cylindrical tank with an inlet (an opening) at its top and a >>> connected pipe to its bottom as an outlet. The boundary conditions >>> are set accordingly, i.e., inflow and outflow, respectively. >>> There is >>> no problem with isothermal simulation of such configuration. >>> However, >>> when volumetric heat source is added to the fluid domain (via userq2 >>> subroutine), non-physical temperatures have been observed at the >>> walls (w/ adiabatic BC) in the immediate vicinity of the inflow (w/ >>> Dirichlet temperature BC). In fact, the element nodes close to the >>> inlet have very high or very low temperatures, which are no >>> expected. >>> >>> I am wondering if anyone has any experience/hint on this issue. >>> >>> Thanks, >>> Mohsen >>> >>> >>> >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > From nek5000-users at lists.mcs.anl.gov Wed Jun 11 02:50:52 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 11 Jun 2014 11:50:52 +0400 Subject: [Nek5000-users] Time-dependant boundary condition In-Reply-To: References: Message-ID: Thanks, I will try Van > 09.06.2014, 16:06:05 ???????????? (nek5000-users at lists.mcs.anl.gov) ???????: > > In userbc: > > ??????ux = cos(pi*y)*cos(2.*pi*time) > ??????uy = 0. > > Paul > > ________________________________________ > From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > Sent: Monday, June 09, 2014 2:30 AM > To: nek5000-users at lists.mcs.anl.gov > Subject: [Nek5000-users] Time-dependant boundary condition > > How should I impose time-dependant BC for velocity on the left vertical boundaty for a 2D box geometry. > The velocity profile should be > Vx=cos(pi*y)*cos(2*pi*t) > Vy=0 > > To illustrate the idea here are the pictures. > Instead of constant velocity Vx=c on the left (inflow) boundary of a channel > V __________________ > ??| > ??| > ??| > ??|__________________ > > I would impose Vx=cos(pi*y)*cos(2*pi*t) > so for t = 0 velocity profile is > ____________________ > \ > \ > ??\ > ???\_________________ > for t=1 velocity profile is > ????_________________ > ???/ > ??/ > / > /____________________ > > and so on. > > I know it should be possible in nek5000, but still not very familiar with syntax and fortran. > > Thank you in advance. > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > From nek5000-users at lists.mcs.anl.gov Wed Jun 11 02:52:42 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 11 Jun 2014 11:52:42 +0400 Subject: [Nek5000-users] PRENEK, how to set o change parameters ("input vales" like thermal conductivity)? Is there a manual with pictures? Message-ID: According to manual http://www.mcs.anl.gov/~fischer/nek_manual_v0.pdf (which lacks for pictures) after you have set the [EQUATION TYPE] and switch [CONVECTION] you are prompted to enter [INPUT VALUES] where you can set parameter CONDUCT (the thermal conductivity), NORDER and so on but really in prex after you "Assemble form of equation to be solved" and "ACCEPT CURRENT SWITCHES", choose the switches "WITH CONVECTION" and "CHARACTERISTICS" you are to "BUILD FROM FILE" or "BUILD INTERACTIVELY" so there is no option to set material properties Then, after you have created the geometry you can set [SET MATL PROPS,Q] But when you try to assign a constant value you got a message "If properties in group zero are constants, they can be set in the SET PARAMETER menu. You cannot override those values here except with a FORTRAN FUNCTION. Please change them in the SET PARAMETER menu in a new session." I have looked for "SET PARAMETER" everywhere in the menu, but have not found. So how do I set and change thermal expansion, thermal conductivity, rho, cp, viscosity and so on? Thanks in advance Van From nek5000-users at lists.mcs.anl.gov Wed Jun 11 05:30:19 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 11 Jun 2014 12:30:19 +0200 Subject: [Nek5000-users] problems running in parallel In-Reply-To: References: Message-ID: Thanks. Now it works! El 10-06-2014 19:38, nek5000-users at lists.mcs.anl.gov escribi?: > Hi, > > Note also that sometime, for unknown reason, mpiexec does not work > correctly on certain platforms and you should use instead > mpiexec.mpich2 > That has solved the problem for me few months ago. > > ++ > JC > > 2014-06-10 19:32 GMT+02:00 : > >> You seem to be running on a single proc. You have to start the >> program using one one of the scripts >> >> nekmpi >> >> or >> >> nekbmpi >> >> E.g. >> >> nekmpi jobname 4 >> >> to run with 4 procs. >> >> praveen >> >> On Tue, Jun 10, 2014 at 7:23 PM, >> wrote: >> >>> Dear users, >>> >>> I am trying to simulate the flow past a cylinder. If I run my >>> simulation with lelt=2000, lelg=2000 in 1 processor, everything >>> works fine. However, if I increase the resolution to lelt=4200 I >>> get a compilation error. >>> >>> Following this post: >>> >>> >> > http://lists.mcs.anl.gov/pipermail/nek5000-users/2013-April/002101.html >>> [1] >>> >>> I have seen that if I use more processors, the code compiles >>> fine. >>> >>> However, now I am not able to run the code using 4 processors. I >>> get the following error: >>> >>> ?Number of processors: ? ? ? ? ? 1 >>> ?REAL ? ?wdsize ? ? ?: ? ? ? ? ? 8 >>> ?INTEGER wdsize ? ? ?: ? ? ? ? ? 4 >>> >>> ? Beginning session: >>> ? /SL/nek5_svn/test/cyl/cyl.rea >>> >>> ?timer accuracy: ? 1.1920929E-07 sec >>> >>> ?read .rea file >>> >>> ? Beginning session: >>> ? /SL/nek5_svn/test/cyl/cyl.rea >>> >>> ?timer accuracy: ? 9.5367432E-08 sec >>> >>> ?read .rea file >>> ?nelgt/nelgv/lelt: ? ? ? ?4425 ? ? ? ?4425 ? ? ? >>> ?2000 >>> ?lx1 ?/lx2 ?/lx3 : ? ? ? ? ? 5 ? ? ? ? ? 5 ? ? ? >>> ? ? 5 >>> >>> ? ABORT: Problem size too large! >>> >>> ? This solver has been compiled for: >>> ? ? ?number of elements/proc ?(lelt): ? ? ? ?2000 >>> ? ? ?total number of elements (lelg): ? ? ? ?5000 >>> >>> ? Recompile with the following SIZE ?parameters: >>> ? ? ?lelt >= ? ? ? ? 4425 ?for np = ? ? ? ? ? ?1 >>> ? ? ?lelg >= ? ? ? ? 4425 >>> >>> I have a 3d mesh with 4425 elemnts. In the SIZE file I have set: >>> >>> ? ? ? parameter (ldim=3) >>> ? ? ? parameter (lx1=5,ly1=lx1,lz1=lx1,lelt=2000,lelv=lelt) >>> ? ? ? parameter (lxd=(3*lx1)/2,lyd=lxd,lzd=lxd) >>> ? ? ? parameter (lelx=1,lely=lelx,lelz=lely) >>> >>> ? ? ? parameter (lx2=lx1-0) ? ! Pressure array dimensions >>> ? ? ? parameter (ly2=ly1-0) >>> ? ? ? parameter (lz2=lz1-0) >>> >>> ? ? ? parameter (lx3=lx2) >>> ? ? ? parameter (ly3=ly2) >>> ? ? ? parameter (lz3=lz2) >>> >>> ? ? ? parameter (lp = 4) ?! Max # processors >>> ? ? ? parameter (lelg = 5000) ! Max # elements, total >>> >>> ? ? ? parameter (lzl=3 + 2*(ldim-3)) >>> >>> I have tried to follow this post to solve the problem, but I >>> couldn't: >>> >>> >> > https://lists.mcs.anl.gov/mailman/htdig/nek5000-users/2013-December/002411.html >>> [2] >>> >>> Could you help me, please? >>> >>> Regards, >>> >>> SL >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users [3] >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users [3] > > -- > > Jean-Christophe Loiseau > Homepage [4] > > > Links: > ------ > [1] > http://lists.mcs.anl.gov/pipermail/nek5000-users/2013-April/002101.html > [2] > https://lists.mcs.anl.gov/mailman/htdig/nek5000-users/2013-December/002411.html > [3] https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > [4] https://sites.google.com/site/loiseaujc/ > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Wed Jun 11 06:40:11 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 11 Jun 2014 11:40:11 +0000 Subject: [Nek5000-users] PRENEK, how to set o change parameters ("input vales" like thermal conductivity)? Is there a manual with pictures? In-Reply-To: References: Message-ID: The best way to change these parameters is to edit the .rea file and change them; or to reset them in the .usr file in subroutine usrdat, e.g. subroutine usrdat include 'SIZE' include 'TOTAL' param(1) = 1.0 ! density param(2) = .0001 ! viscosity return end Paul ________________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Wednesday, June 11, 2014 2:52 AM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] PRENEK, how to set o change parameters ("input vales" like thermal conductivity)? Is there a manual with pictures? According to manual http://www.mcs.anl.gov/~fischer/nek_manual_v0.pdf (which lacks for pictures) after you have set the [EQUATION TYPE] and switch [CONVECTION] you are prompted to enter [INPUT VALUES] where you can set parameter CONDUCT (the thermal conductivity), NORDER and so on but really in prex after you "Assemble form of equation to be solved" and "ACCEPT CURRENT SWITCHES", choose the switches "WITH CONVECTION" and "CHARACTERISTICS" you are to "BUILD FROM FILE" or "BUILD INTERACTIVELY" so there is no option to set material properties Then, after you have created the geometry you can set [SET MATL PROPS,Q] But when you try to assign a constant value you got a message "If properties in group zero are constants, they can be set in the SET PARAMETER menu. You cannot override those values here except with a FORTRAN FUNCTION. Please change them in the SET PARAMETER menu in a new session." I have looked for "SET PARAMETER" everywhere in the menu, but have not found. So how do I set and change thermal expansion, thermal conductivity, rho, cp, viscosity and so on? Thanks in advance Van _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Sat Jun 14 15:36:24 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 15 Jun 2014 00:36:24 +0400 Subject: [Nek5000-users] how to turn off conductivity/diffusion Message-ID: I would like to model scalar transport without diffusion. Now I model scalar transport with the help of temperature variable (as in examples.pdf). If I just set parameter p0008 to zero or less than e-7 I got exception (background scalar gradient is about 100), which is quite comprehensible because of the insulated boundary condition. Even e-7 is quite a lot for my problem. So is there a way to model scalar transport without diffusion, i.e. without RHS at all? Or may be some trick with boundary conditions, which allows to set diffusion coefficient to zero? From nek5000-users at lists.mcs.anl.gov Sun Jun 15 02:07:36 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 15 Jun 2014 11:07:36 +0400 Subject: [Nek5000-users] Monitor points, location probe Message-ID: I need to monitor scalar gradient (scalar is modelled with temperature as in examples.pdf). So I have inserted in USERCHK parameter (lt=lx1*ly1*lz1*lelt) common /ilgrad/ dtdx(lt),dtdy(lt),dtdz(lt) if ((mod(istep,iostep).eq.0).and.(istep.ge.iostep)) then call gradm1(dtdx,dtdy,dtdz,t) endif call hpts() Next there are two options to monitor a quantity 1. in .rea file like ***** HISTORY AND INTEGRAL DATA ***** 001 POINTS. Hcode, I,J,H,IEL UV PT H 3 3 1 1 But I dont know how to tell it that I want instead of UV, and also I don't know how to calculate number of element IEL from physical location. 2. hpts.in file you can input physical coordinates of a location, but in hpts.out only the following variables # time vx vy [vz] pr T PS1 PS2 ... are being stored. So I tried to modify nek5000/branches/mvmesh/postpro.f in the following way: first I put parameter (lt=lx1*ly1*lz1*lelt) common /ilgrad/ dtdx(lt),dtdy(lt),dtdz(lt) in the beginning of subroutine hpts and later in this routine changed the code: ! pack working array nflds = 0 if(ifvo) then call copy(wrk(1,1),vx,ntot) call copy(wrk(1,2),vy,ntot) if(if3d) call copy(wrk(1,3),vz,ntot) nflds = ndim endif if(ifpo) then nflds = nflds + 1 call copy(wrk(1,nflds),pm1,ntot) endif if(ifto) then nflds = nflds + 1 call copy(wrk(1,nflds),t,ntot) endif nflds = nflds + 1 !!!!!!!!!inserted call copy(wrk(1,nflds),dtdx,ntot) !!!!!!!!!inserted nflds = nflds + 1 !!!!!!!!!inserted call copy(wrk(1,nflds),dtdy,ntot) !!!!!!!!!inserted do i = 1,ldimt if(ifpsco(i)) then nflds = nflds + 1 call copy(wrk(1,nflds),T(1,1,1,1,i+1),ntot) endif enddo It was compiled without problem, but running the program yielded no change in hpts.out, as before there are only 5 columns # time vx vy [vz] pr T Please help From nek5000-users at lists.mcs.anl.gov Sun Jun 15 07:12:33 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 15 Jun 2014 14:12:33 +0200 Subject: [Nek5000-users] Monitor points, location probe In-Reply-To: References: Message-ID: Hi, You can make it much simpler! Simply do for instance: real work1(lx1,ly1,lz1,lelt), work2(lx1,ly1,lz1,lelt), work3(lx1,ly1,lz1,lelt) ... compute your dtdx dtdy dtdz call opcopy(work1,work2,work3,vx,vy,vz) ! Save vx vy vz for later call opcopy(vx,vy,vz,dtdx,dtdy,dtdz) ! Save dtdx into vx for the hpts output call hpts call opcopy(vx,vy,vz,work1,work2,work3) ! Restore vx vy vz That should do the trick I guess. Cheers, JC 2014-06-15 9:07 GMT+02:00 : > > I need to monitor scalar gradient (scalar is modelled with temperature as > in examples.pdf). > So I have inserted in USERCHK > parameter (lt=lx1*ly1*lz1*lelt) > common /ilgrad/ dtdx(lt),dtdy(lt),dtdz(lt) > if ((mod(istep,iostep).eq.0).and.(istep.ge.iostep)) then > call gradm1(dtdx,dtdy,dtdz,t) > endif > call hpts() > > Next there are two options to monitor a quantity > 1. in .rea file like > ***** HISTORY AND INTEGRAL DATA ***** > 001 POINTS. Hcode, I,J,H,IEL > UV PT H 3 3 1 1 > > But I dont know how to tell it that I want instead of UV, and also I don't > know how to calculate number of element IEL from physical location. > > 2. hpts.in file > you can input physical coordinates of a location, but in hpts.out only the > following variables # time vx vy [vz] pr T PS1 PS2 ... > are being stored. > > So I tried to modify nek5000/branches/mvmesh/postpro.f in the following > way: > first I put parameter (lt=lx1*ly1*lz1*lelt) > common /ilgrad/ dtdx(lt),dtdy(lt),dtdz(lt) > in the beginning of subroutine hpts > > and later in this routine changed the code: > > > ! pack working array > nflds = 0 > if(ifvo) then > call copy(wrk(1,1),vx,ntot) > call copy(wrk(1,2),vy,ntot) > if(if3d) call copy(wrk(1,3),vz,ntot) > nflds = ndim > endif > if(ifpo) then > nflds = nflds + 1 > call copy(wrk(1,nflds),pm1,ntot) > endif > if(ifto) then > nflds = nflds + 1 > call copy(wrk(1,nflds),t,ntot) > endif > nflds = nflds + 1 !!!!!!!!!inserted > call copy(wrk(1,nflds),dtdx,ntot) !!!!!!!!!inserted > nflds = nflds + 1 !!!!!!!!!inserted > call copy(wrk(1,nflds),dtdy,ntot) !!!!!!!!!inserted > do i = 1,ldimt > if(ifpsco(i)) then > nflds = nflds + 1 > call copy(wrk(1,nflds),T(1,1,1,1,i+1),ntot) > endif > enddo > It was compiled without problem, but running the program yielded no > change in hpts.out, > as before there are only 5 columns > # time vx vy [vz] pr T > Please help > > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > -- Jean-Christophe Loiseau Homepage -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Sun Jun 15 15:05:16 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 15 Jun 2014 15:05:16 -0500 Subject: [Nek5000-users] Reg: error in Genmap Message-ID: Hello all, I get the following error, Input mesh tolerance (default 0.2): NOTE: smaller is better, but generous is more forgiving for bad meshes. .005 reading .rea file data ... start locglob_lexico: 8 8 64 5.000000000000000E-003 locglob: 1 1 64 locglob: 2 3 64 locglob: 3 9 64 locglob: 1 18 64 locglob: 2 18 64 locglob: 3 18 64 locglob: 1 18 64 locglob: 2 18 64 locglob: 3 18 64 1 2 4 Matrix: SELF!! 1 SELF!! 1 3 1 3 2 SELF!! 7 9 7 9 cont: SELF!! 1 ?? ABORT: SELF-CHK 1 5 1 0 Try to tighten the mesh tolerance! 0 quit How to address this problem. I manually modified the mesh coniditons in the .rea file. I tried to look out for this in the previous posts. Nothing worked for my case from the suggestions. Thanks, Ravi Kiran Pendyala, -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Sun Jun 15 18:11:39 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 15 Jun 2014 23:11:39 +0000 Subject: [Nek5000-users] Reg: error in Genmap In-Reply-To: References: Message-ID: Dear Ravi, My guess is that your mesh is somehow invalid. A quick look at the genmap.f source indicates that the first number in front of the SELF error indicator is the element number, which would imply something wrong with element number 1. Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Sunday, June 15, 2014 3:05 PM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] Reg: error in Genmap Hello all, I get the following error, Input mesh tolerance (default 0.2): NOTE: smaller is better, but generous is more forgiving for bad meshes. .005 reading .rea file data ... start locglob_lexico: 8 8 64 5.000000000000000E-003 locglob: 1 1 64 locglob: 2 3 64 locglob: 3 9 64 locglob: 1 18 64 locglob: 2 18 64 locglob: 3 18 64 locglob: 1 18 64 locglob: 2 18 64 locglob: 3 18 64 1 2 4 Matrix: SELF!! 1 SELF!! 1 3 1 3 2 SELF!! 7 9 7 9 cont: SELF!! 1 ?? ABORT: SELF-CHK 1 5 1 0 Try to tighten the mesh tolerance! 0 quit How to address this problem. I manually modified the mesh coniditons in the .rea file. I tried to look out for this in the previous posts. Nothing worked for my case from the suggestions. Thanks, Ravi Kiran Pendyala, -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Sun Jun 15 21:15:27 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 16 Jun 2014 10:15:27 +0800 Subject: [Nek5000-users] quasi 3D and boundary condition In-Reply-To: References: , Message-ID: Hi Paul what is implementation of SYM BC in NEK5000? I mean the variation formula. cheers ---------------------------------------------- Zhang Wei waynezw0618 at gmail.com On 9 Jun, 2014, at 4:15 am, nek5000-users at lists.mcs.anl.gov wrote: > > Hi Zhang, > > There is no support for 2.5D with Fourier in z and currently no plans to move in that direction. > > If you want a slip velocity on the curved surface you should use the stress formulation (lx2=lx1-2, etc., > with ifstrs T. Then the "SYM" bc should give you the desired bc, i.e., U.nhat = 0, d/dn (U.t_hat) = 0. > > Paul > > _______________________________________ > From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > Sent: Sunday, June 08, 2014 10:03 AM > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] quasi 3D and boundary condition > > Hi Paul > Thanks for replying. > for quasi-2D, I mean I wish to define the velocity u(x,y,z) as sum(u(x,y,k)e^kz) to reduce the computational cost for really 3D case and also to avoid the long wave (which may longer then the geometry size in the z direction) in the axial direction.does nek currently support such feature? > > for prescribe the bc on curl surface, I mean something like non-immersed bc and and have velocity component in the tangential direction, like in the potential theory. > > > > > cheers > ---------------------------------------------- > Zhang Wei > waynezw0618 at gmail.com > > > > On 8 Jun, 2014, at 10:44 pm, nek5000-users at lists.mcs.anl.gov wrote: > >> >> Hi Zhang, >> >> You can use periodic boundary conditions in the z direction, provided you have at least 3 >> elements in z. >> >> Prescribed boundary conditions are given in Cartesian coordinates. If you have the "mv " >> bc on your moving surface (i.e., the cylinder surface), along with the following things >> >> lx2=lx1-2 >> ly2=ly1-2 >> lz2=lz1-2 >> >> parameter (lx1m=lx1,ly1m=ly1,lz1m=lz1) >> >> in SIZE, and T ifstrs, T ifmvbd in the .rea file, then the mesh will move with the fluid >> velocity (which you prescribe as Cartesian velocity vectors, u,v,w). Note that nek >> uses an ALE formulation and the mesh motion must relatively limited or the mesh >> becomes too distorted. For an oscillating cylinder, this should be ok (see >> www.mcs.anl.gov/~fischer/ocyl.gif). I've just added a 2D oscillating cylinder case >> that illustrates the basic procedure to the examples suite. >> >> Paul >> >> >> >> ________________________________________ >> From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] >> Sent: Sunday, June 08, 2014 8:40 AM >> To: nek5000-users at lists.mcs.anl.gov >> Subject: [Nek5000-users] quasi 3D and boundary condition >> >> Hi Everyone. >> I am trying to run the flow past a cylinder case. I am going to move to the 3D simulation for my study. I have two questions: >> 1) how to run quasi 3D simulation in nek5000 ? if there is not existing code, andy suggestion to how to implement so? >> 2) how to specify the normal and tangential boundary condition for a curvature boundary? >> >> >> cheers >> ---------------------------------------------- >> Zhang Wei >> waynezw0618 at gmail.com >> >> >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Sun Jun 15 22:09:10 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 16 Jun 2014 03:09:10 +0000 Subject: [Nek5000-users] quasi 3D and boundary condition In-Reply-To: References: , , Message-ID: Assuming that the surface normal is x, y, or z, then it is simply U.nhat = 0 and Neumann on the other two boundaries. Paul ________________________ ________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Sunday, June 15, 2014 9:15 PM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] quasi 3D and boundary condition Hi Paul what is implementation of SYM BC in NEK5000? I mean the variation formula. cheers ---------------------------------------------- Zhang Wei waynezw0618 at gmail.com On 9 Jun, 2014, at 4:15 am, nek5000-users at lists.mcs.anl.gov wrote: > > Hi Zhang, > > There is no support for 2.5D with Fourier in z and currently no plans to move in that direction. > > If you want a slip velocity on the curved surface you should use the stress formulation (lx2=lx1-2, etc., > with ifstrs T. Then the "SYM" bc should give you the desired bc, i.e., U.nhat = 0, d/dn (U.t_hat) = 0. > > Paul > > _______________________________________ > From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > Sent: Sunday, June 08, 2014 10:03 AM > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] quasi 3D and boundary condition > > Hi Paul > Thanks for replying. > for quasi-2D, I mean I wish to define the velocity u(x,y,z) as sum(u(x,y,k)e^kz) to reduce the computational cost for really 3D case and also to avoid the long wave (which may longer then the geometry size in the z direction) in the axial direction.does nek currently support such feature? > > for prescribe the bc on curl surface, I mean something like non-immersed bc and and have velocity component in the tangential direction, like in the potential theory. > > > > > cheers > ---------------------------------------------- > Zhang Wei > waynezw0618 at gmail.com > > > > On 8 Jun, 2014, at 10:44 pm, nek5000-users at lists.mcs.anl.gov wrote: > >> >> Hi Zhang, >> >> You can use periodic boundary conditions in the z direction, provided you have at least 3 >> elements in z. >> >> Prescribed boundary conditions are given in Cartesian coordinates. If you have the "mv " >> bc on your moving surface (i.e., the cylinder surface), along with the following things >> >> lx2=lx1-2 >> ly2=ly1-2 >> lz2=lz1-2 >> >> parameter (lx1m=lx1,ly1m=ly1,lz1m=lz1) >> >> in SIZE, and T ifstrs, T ifmvbd in the .rea file, then the mesh will move with the fluid >> velocity (which you prescribe as Cartesian velocity vectors, u,v,w). Note that nek >> uses an ALE formulation and the mesh motion must relatively limited or the mesh >> becomes too distorted. For an oscillating cylinder, this should be ok (see >> www.mcs.anl.gov/~fischer/ocyl.gif). I've just added a 2D oscillating cylinder case >> that illustrates the basic procedure to the examples suite. >> >> Paul >> >> >> >> ________________________________________ >> From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] >> Sent: Sunday, June 08, 2014 8:40 AM >> To: nek5000-users at lists.mcs.anl.gov >> Subject: [Nek5000-users] quasi 3D and boundary condition >> >> Hi Everyone. >> I am trying to run the flow past a cylinder case. I am going to move to the 3D simulation for my study. I have two questions: >> 1) how to run quasi 3D simulation in nek5000 ? if there is not existing code, andy suggestion to how to implement so? >> 2) how to specify the normal and tangential boundary condition for a curvature boundary? >> >> >> cheers >> ---------------------------------------------- >> Zhang Wei >> waynezw0618 at gmail.com >> >> >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Sun Jun 15 22:13:11 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 16 Jun 2014 11:13:11 +0800 Subject: [Nek5000-users] quasi 3D and boundary condition In-Reply-To: References: , , Message-ID: Hi Paul but for curved boundary, how you do so? I want to know the formula for what you mentioned as stress formula. cheers ---------------------------------------------- Zhang Wei waynezw0618 at gmail.com On 16 Jun, 2014, at 11:09 am, nek5000-users at lists.mcs.anl.gov wrote: > > Assuming that the surface normal is x, y, or z, then it is simply > > U.nhat = 0 > > and Neumann on the other two boundaries. > > Paul > > ________________________ > ________________ > From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > Sent: Sunday, June 15, 2014 9:15 PM > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] quasi 3D and boundary condition > > Hi Paul > what is implementation of SYM BC in NEK5000? I mean the variation formula. > > > cheers > ---------------------------------------------- > Zhang Wei > waynezw0618 at gmail.com > > > > On 9 Jun, 2014, at 4:15 am, nek5000-users at lists.mcs.anl.gov wrote: > >> >> Hi Zhang, >> >> There is no support for 2.5D with Fourier in z and currently no plans to move in that direction. >> >> If you want a slip velocity on the curved surface you should use the stress formulation (lx2=lx1-2, etc., >> with ifstrs T. Then the "SYM" bc should give you the desired bc, i.e., U.nhat = 0, d/dn (U.t_hat) = 0. >> >> Paul >> >> _______________________________________ >> From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] >> Sent: Sunday, June 08, 2014 10:03 AM >> To: nek5000-users at lists.mcs.anl.gov >> Subject: Re: [Nek5000-users] quasi 3D and boundary condition >> >> Hi Paul >> Thanks for replying. >> for quasi-2D, I mean I wish to define the velocity u(x,y,z) as sum(u(x,y,k)e^kz) to reduce the computational cost for really 3D case and also to avoid the long wave (which may longer then the geometry size in the z direction) in the axial direction.does nek currently support such feature? >> >> for prescribe the bc on curl surface, I mean something like non-immersed bc and and have velocity component in the tangential direction, like in the potential theory. >> >> >> >> >> cheers >> ---------------------------------------------- >> Zhang Wei >> waynezw0618 at gmail.com >> >> >> >> On 8 Jun, 2014, at 10:44 pm, nek5000-users at lists.mcs.anl.gov wrote: >> >>> >>> Hi Zhang, >>> >>> You can use periodic boundary conditions in the z direction, provided you have at least 3 >>> elements in z. >>> >>> Prescribed boundary conditions are given in Cartesian coordinates. If you have the "mv " >>> bc on your moving surface (i.e., the cylinder surface), along with the following things >>> >>> lx2=lx1-2 >>> ly2=ly1-2 >>> lz2=lz1-2 >>> >>> parameter (lx1m=lx1,ly1m=ly1,lz1m=lz1) >>> >>> in SIZE, and T ifstrs, T ifmvbd in the .rea file, then the mesh will move with the fluid >>> velocity (which you prescribe as Cartesian velocity vectors, u,v,w). Note that nek >>> uses an ALE formulation and the mesh motion must relatively limited or the mesh >>> becomes too distorted. For an oscillating cylinder, this should be ok (see >>> www.mcs.anl.gov/~fischer/ocyl.gif). I've just added a 2D oscillating cylinder case >>> that illustrates the basic procedure to the examples suite. >>> >>> Paul >>> >>> >>> >>> ________________________________________ >>> From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] >>> Sent: Sunday, June 08, 2014 8:40 AM >>> To: nek5000-users at lists.mcs.anl.gov >>> Subject: [Nek5000-users] quasi 3D and boundary condition >>> >>> Hi Everyone. >>> I am trying to run the flow past a cylinder case. I am going to move to the 3D simulation for my study. I have two questions: >>> 1) how to run quasi 3D simulation in nek5000 ? if there is not existing code, andy suggestion to how to implement so? >>> 2) how to specify the normal and tangential boundary condition for a curvature boundary? >>> >>> >>> cheers >>> ---------------------------------------------- >>> Zhang Wei >>> waynezw0618 at gmail.com >>> >>> >>> >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Sun Jun 15 22:34:07 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 16 Jun 2014 03:34:07 +0000 Subject: [Nek5000-users] quasi 3D and boundary condition In-Reply-To: References: , , , Message-ID: Hi, In that case, you need to use the stress formulation and the net result is U.n_hat = 0 and d/dn (U.t_hat) = 0, where t_hat constitutes the two tangent vectors. I've not tried this myself but I assume it works - it was written by Lee W. Ho when we were graduate students and I believe that others have used it. If I were you I would do a small test case in 2D first. -- I just tried it and it worked ok... you need to set ifstrs T in the .rea file and lx1m=lx1, etc. in the SIZE file. Paul ________________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Sunday, June 15, 2014 10:13 PM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] quasi 3D and boundary condition Hi Paul but for curved boundary, how you do so? I want to know the formula for what you mentioned as stress formula. cheers ---------------------------------------------- Zhang Wei waynezw0618 at gmail.com On 16 Jun, 2014, at 11:09 am, nek5000-users at lists.mcs.anl.gov wrote: > > Assuming that the surface normal is x, y, or z, then it is simply > > U.nhat = 0 > > and Neumann on the other two boundaries. > > Paul > > ________________________ > ________________ > From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > Sent: Sunday, June 15, 2014 9:15 PM > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] quasi 3D and boundary condition > > Hi Paul > what is implementation of SYM BC in NEK5000? I mean the variation formula. > > > cheers > ---------------------------------------------- > Zhang Wei > waynezw0618 at gmail.com > > > > On 9 Jun, 2014, at 4:15 am, nek5000-users at lists.mcs.anl.gov wrote: > >> >> Hi Zhang, >> >> There is no support for 2.5D with Fourier in z and currently no plans to move in that direction. >> >> If you want a slip velocity on the curved surface you should use the stress formulation (lx2=lx1-2, etc., >> with ifstrs T. Then the "SYM" bc should give you the desired bc, i.e., U.nhat = 0, d/dn (U.t_hat) = 0. >> >> Paul >> >> _______________________________________ >> From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] >> Sent: Sunday, June 08, 2014 10:03 AM >> To: nek5000-users at lists.mcs.anl.gov >> Subject: Re: [Nek5000-users] quasi 3D and boundary condition >> >> Hi Paul >> Thanks for replying. >> for quasi-2D, I mean I wish to define the velocity u(x,y,z) as sum(u(x,y,k)e^kz) to reduce the computational cost for really 3D case and also to avoid the long wave (which may longer then the geometry size in the z direction) in the axial direction.does nek currently support such feature? >> >> for prescribe the bc on curl surface, I mean something like non-immersed bc and and have velocity component in the tangential direction, like in the potential theory. >> >> >> >> >> cheers >> ---------------------------------------------- >> Zhang Wei >> waynezw0618 at gmail.com >> >> >> >> On 8 Jun, 2014, at 10:44 pm, nek5000-users at lists.mcs.anl.gov wrote: >> >>> >>> Hi Zhang, >>> >>> You can use periodic boundary conditions in the z direction, provided you have at least 3 >>> elements in z. >>> >>> Prescribed boundary conditions are given in Cartesian coordinates. If you have the "mv " >>> bc on your moving surface (i.e., the cylinder surface), along with the following things >>> >>> lx2=lx1-2 >>> ly2=ly1-2 >>> lz2=lz1-2 >>> >>> parameter (lx1m=lx1,ly1m=ly1,lz1m=lz1) >>> >>> in SIZE, and T ifstrs, T ifmvbd in the .rea file, then the mesh will move with the fluid >>> velocity (which you prescribe as Cartesian velocity vectors, u,v,w). Note that nek >>> uses an ALE formulation and the mesh motion must relatively limited or the mesh >>> becomes too distorted. For an oscillating cylinder, this should be ok (see >>> www.mcs.anl.gov/~fischer/ocyl.gif). I've just added a 2D oscillating cylinder case >>> that illustrates the basic procedure to the examples suite. >>> >>> Paul >>> >>> >>> >>> ________________________________________ >>> From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] >>> Sent: Sunday, June 08, 2014 8:40 AM >>> To: nek5000-users at lists.mcs.anl.gov >>> Subject: [Nek5000-users] quasi 3D and boundary condition >>> >>> Hi Everyone. >>> I am trying to run the flow past a cylinder case. I am going to move to the 3D simulation for my study. I have two questions: >>> 1) how to run quasi 3D simulation in nek5000 ? if there is not existing code, andy suggestion to how to implement so? >>> 2) how to specify the normal and tangential boundary condition for a curvature boundary? >>> >>> >>> cheers >>> ---------------------------------------------- >>> Zhang Wei >>> waynezw0618 at gmail.com >>> >>> >>> >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Sun Jun 15 22:36:00 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 16 Jun 2014 11:36:00 +0800 Subject: [Nek5000-users] quasi 3D and boundary condition In-Reply-To: References: , , , Message-ID: Hi Paul. is there any paper of about that? I would know more math work of this implementation. cheers ---------------------------------------------- Zhang Wei waynezw0618 at gmail.com On 16 Jun, 2014, at 11:34 am, nek5000-users at lists.mcs.anl.gov wrote: > > Hi, > > In that case, you need to use the stress formulation and the net result > is U.n_hat = 0 and d/dn (U.t_hat) = 0, where t_hat constitutes the two tangent > vectors. > > I've not tried this myself but I assume it works - it was written by Lee W. Ho > when we were graduate students and I believe that others have used it. > > If I were you I would do a small test case in 2D first. -- I just tried it and it > worked ok... you need to set ifstrs T in the .rea file and lx1m=lx1, etc. in > the SIZE file. > > > > Paul > ________________________________________ > From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > Sent: Sunday, June 15, 2014 10:13 PM > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] quasi 3D and boundary condition > > Hi Paul > > but for curved boundary, how you do so? I want to know the formula for what you mentioned as stress formula. > > cheers > ---------------------------------------------- > Zhang Wei > waynezw0618 at gmail.com > > > > On 16 Jun, 2014, at 11:09 am, nek5000-users at lists.mcs.anl.gov wrote: > >> >> Assuming that the surface normal is x, y, or z, then it is simply >> >> U.nhat = 0 >> >> and Neumann on the other two boundaries. >> >> Paul >> >> ________________________ >> ________________ >> From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] >> Sent: Sunday, June 15, 2014 9:15 PM >> To: nek5000-users at lists.mcs.anl.gov >> Subject: Re: [Nek5000-users] quasi 3D and boundary condition >> >> Hi Paul >> what is implementation of SYM BC in NEK5000? I mean the variation formula. >> >> >> cheers >> ---------------------------------------------- >> Zhang Wei >> waynezw0618 at gmail.com >> >> >> >> On 9 Jun, 2014, at 4:15 am, nek5000-users at lists.mcs.anl.gov wrote: >> >>> >>> Hi Zhang, >>> >>> There is no support for 2.5D with Fourier in z and currently no plans to move in that direction. >>> >>> If you want a slip velocity on the curved surface you should use the stress formulation (lx2=lx1-2, etc., >>> with ifstrs T. Then the "SYM" bc should give you the desired bc, i.e., U.nhat = 0, d/dn (U.t_hat) = 0. >>> >>> Paul >>> >>> _______________________________________ >>> From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] >>> Sent: Sunday, June 08, 2014 10:03 AM >>> To: nek5000-users at lists.mcs.anl.gov >>> Subject: Re: [Nek5000-users] quasi 3D and boundary condition >>> >>> Hi Paul >>> Thanks for replying. >>> for quasi-2D, I mean I wish to define the velocity u(x,y,z) as sum(u(x,y,k)e^kz) to reduce the computational cost for really 3D case and also to avoid the long wave (which may longer then the geometry size in the z direction) in the axial direction.does nek currently support such feature? >>> >>> for prescribe the bc on curl surface, I mean something like non-immersed bc and and have velocity component in the tangential direction, like in the potential theory. >>> >>> >>> >>> >>> cheers >>> ---------------------------------------------- >>> Zhang Wei >>> waynezw0618 at gmail.com >>> >>> >>> >>> On 8 Jun, 2014, at 10:44 pm, nek5000-users at lists.mcs.anl.gov wrote: >>> >>>> >>>> Hi Zhang, >>>> >>>> You can use periodic boundary conditions in the z direction, provided you have at least 3 >>>> elements in z. >>>> >>>> Prescribed boundary conditions are given in Cartesian coordinates. If you have the "mv " >>>> bc on your moving surface (i.e., the cylinder surface), along with the following things >>>> >>>> lx2=lx1-2 >>>> ly2=ly1-2 >>>> lz2=lz1-2 >>>> >>>> parameter (lx1m=lx1,ly1m=ly1,lz1m=lz1) >>>> >>>> in SIZE, and T ifstrs, T ifmvbd in the .rea file, then the mesh will move with the fluid >>>> velocity (which you prescribe as Cartesian velocity vectors, u,v,w). Note that nek >>>> uses an ALE formulation and the mesh motion must relatively limited or the mesh >>>> becomes too distorted. For an oscillating cylinder, this should be ok (see >>>> www.mcs.anl.gov/~fischer/ocyl.gif). I've just added a 2D oscillating cylinder case >>>> that illustrates the basic procedure to the examples suite. >>>> >>>> Paul >>>> >>>> >>>> >>>> ________________________________________ >>>> From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] >>>> Sent: Sunday, June 08, 2014 8:40 AM >>>> To: nek5000-users at lists.mcs.anl.gov >>>> Subject: [Nek5000-users] quasi 3D and boundary condition >>>> >>>> Hi Everyone. >>>> I am trying to run the flow past a cylinder case. I am going to move to the 3D simulation for my study. I have two questions: >>>> 1) how to run quasi 3D simulation in nek5000 ? if there is not existing code, andy suggestion to how to implement so? >>>> 2) how to specify the normal and tangential boundary condition for a curvature boundary? >>>> >>>> >>>> cheers >>>> ---------------------------------------------- >>>> Zhang Wei >>>> waynezw0618 at gmail.com >>>> >>>> >>>> >>>> _______________________________________________ >>>> Nek5000-users mailing list >>>> Nek5000-users at lists.mcs.anl.gov >>>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>>> _______________________________________________ >>>> Nek5000-users mailing list >>>> Nek5000-users at lists.mcs.anl.gov >>>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>> >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Sun Jun 15 22:39:35 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 16 Jun 2014 03:39:35 +0000 Subject: [Nek5000-users] quasi 3D and boundary condition In-Reply-To: References: , , , , Message-ID: You can find Lee Ho's MIT Ph.D. thesis online - 1989. It's really just the variational formulation for the Stokes operator. Paul ________________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Sunday, June 15, 2014 10:36 PM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] quasi 3D and boundary condition Hi Paul. is there any paper of about that? I would know more math work of this implementation. cheers ---------------------------------------------- Zhang Wei waynezw0618 at gmail.com On 16 Jun, 2014, at 11:34 am, nek5000-users at lists.mcs.anl.gov wrote: > > Hi, > > In that case, you need to use the stress formulation and the net result > is U.n_hat = 0 and d/dn (U.t_hat) = 0, where t_hat constitutes the two tangent > vectors. > > I've not tried this myself but I assume it works - it was written by Lee W. Ho > when we were graduate students and I believe that others have used it. > > If I were you I would do a small test case in 2D first. -- I just tried it and it > worked ok... you need to set ifstrs T in the .rea file and lx1m=lx1, etc. in > the SIZE file. > > > > Paul > ________________________________________ > From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > Sent: Sunday, June 15, 2014 10:13 PM > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] quasi 3D and boundary condition > > Hi Paul > > but for curved boundary, how you do so? I want to know the formula for what you mentioned as stress formula. > > cheers > ---------------------------------------------- > Zhang Wei > waynezw0618 at gmail.com > > > > On 16 Jun, 2014, at 11:09 am, nek5000-users at lists.mcs.anl.gov wrote: > >> >> Assuming that the surface normal is x, y, or z, then it is simply >> >> U.nhat = 0 >> >> and Neumann on the other two boundaries. >> >> Paul >> >> ________________________ >> ________________ >> From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] >> Sent: Sunday, June 15, 2014 9:15 PM >> To: nek5000-users at lists.mcs.anl.gov >> Subject: Re: [Nek5000-users] quasi 3D and boundary condition >> >> Hi Paul >> what is implementation of SYM BC in NEK5000? I mean the variation formula. >> >> >> cheers >> ---------------------------------------------- >> Zhang Wei >> waynezw0618 at gmail.com >> >> >> >> On 9 Jun, 2014, at 4:15 am, nek5000-users at lists.mcs.anl.gov wrote: >> >>> >>> Hi Zhang, >>> >>> There is no support for 2.5D with Fourier in z and currently no plans to move in that direction. >>> >>> If you want a slip velocity on the curved surface you should use the stress formulation (lx2=lx1-2, etc., >>> with ifstrs T. Then the "SYM" bc should give you the desired bc, i.e., U.nhat = 0, d/dn (U.t_hat) = 0. >>> >>> Paul >>> >>> _______________________________________ >>> From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] >>> Sent: Sunday, June 08, 2014 10:03 AM >>> To: nek5000-users at lists.mcs.anl.gov >>> Subject: Re: [Nek5000-users] quasi 3D and boundary condition >>> >>> Hi Paul >>> Thanks for replying. >>> for quasi-2D, I mean I wish to define the velocity u(x,y,z) as sum(u(x,y,k)e^kz) to reduce the computational cost for really 3D case and also to avoid the long wave (which may longer then the geometry size in the z direction) in the axial direction.does nek currently support such feature? >>> >>> for prescribe the bc on curl surface, I mean something like non-immersed bc and and have velocity component in the tangential direction, like in the potential theory. >>> >>> >>> >>> >>> cheers >>> ---------------------------------------------- >>> Zhang Wei >>> waynezw0618 at gmail.com >>> >>> >>> >>> On 8 Jun, 2014, at 10:44 pm, nek5000-users at lists.mcs.anl.gov wrote: >>> >>>> >>>> Hi Zhang, >>>> >>>> You can use periodic boundary conditions in the z direction, provided you have at least 3 >>>> elements in z. >>>> >>>> Prescribed boundary conditions are given in Cartesian coordinates. If you have the "mv " >>>> bc on your moving surface (i.e., the cylinder surface), along with the following things >>>> >>>> lx2=lx1-2 >>>> ly2=ly1-2 >>>> lz2=lz1-2 >>>> >>>> parameter (lx1m=lx1,ly1m=ly1,lz1m=lz1) >>>> >>>> in SIZE, and T ifstrs, T ifmvbd in the .rea file, then the mesh will move with the fluid >>>> velocity (which you prescribe as Cartesian velocity vectors, u,v,w). Note that nek >>>> uses an ALE formulation and the mesh motion must relatively limited or the mesh >>>> becomes too distorted. For an oscillating cylinder, this should be ok (see >>>> www.mcs.anl.gov/~fischer/ocyl.gif). I've just added a 2D oscillating cylinder case >>>> that illustrates the basic procedure to the examples suite. >>>> >>>> Paul >>>> >>>> >>>> >>>> ________________________________________ >>>> From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] >>>> Sent: Sunday, June 08, 2014 8:40 AM >>>> To: nek5000-users at lists.mcs.anl.gov >>>> Subject: [Nek5000-users] quasi 3D and boundary condition >>>> >>>> Hi Everyone. >>>> I am trying to run the flow past a cylinder case. I am going to move to the 3D simulation for my study. I have two questions: >>>> 1) how to run quasi 3D simulation in nek5000 ? if there is not existing code, andy suggestion to how to implement so? >>>> 2) how to specify the normal and tangential boundary condition for a curvature boundary? >>>> >>>> >>>> cheers >>>> ---------------------------------------------- >>>> Zhang Wei >>>> waynezw0618 at gmail.com >>>> >>>> >>>> >>>> _______________________________________________ >>>> Nek5000-users mailing list >>>> Nek5000-users at lists.mcs.anl.gov >>>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>>> _______________________________________________ >>>> Nek5000-users mailing list >>>> Nek5000-users at lists.mcs.anl.gov >>>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>> >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Sun Jun 15 23:50:52 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 15 Jun 2014 23:50:52 -0500 Subject: [Nek5000-users] Reg: error in Genmap In-Reply-To: References: Message-ID: Hi Ravi, How did you modify the .rea file? Katherine On Sun, Jun 15, 2014 at 6:11 PM, wrote: > > Dear Ravi, > > My guess is that your mesh is somehow invalid. > > A quick look at the genmap.f source indicates that the first number > in front of the SELF error indicator is the element number, which would > imply something wrong with element number 1. > > Paul > > ------------------------------ > *From:* nek5000-users-bounces at lists.mcs.anl.gov [ > nek5000-users-bounces at lists.mcs.anl.gov] on behalf of > nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > *Sent:* Sunday, June 15, 2014 3:05 PM > *To:* nek5000-users at lists.mcs.anl.gov > *Subject:* [Nek5000-users] Reg: error in Genmap > > Hello all, > > I get the following error, > > Input mesh tolerance (default 0.2): > NOTE: smaller is better, but generous is more forgiving for bad meshes. > .005 > reading .rea file data ... > start locglob_lexico: 8 8 64 5.000000000000000E-003 > locglob: 1 1 64 > locglob: 2 3 64 > locglob: 3 9 64 > locglob: 1 18 64 > locglob: 2 18 64 > locglob: 3 18 64 > locglob: 1 18 64 > locglob: 2 18 64 > locglob: 3 18 64 > > 1 2 4 Matrix: SELF!! > 1 SELF!! 1 3 1 3 > 2 SELF!! 7 9 7 9 > cont: SELF!! 1 ?? > > ABORT: SELF-CHK 1 5 1 0 > Try to tighten the mesh tolerance! > > 0 quit > > > How to address this problem. I manually modified the mesh coniditons in > the .rea file. > I tried to look out for this in the previous posts. Nothing worked for my > case from the suggestions. > > Thanks, > > > Ravi Kiran Pendyala, > > > > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jun 16 10:28:23 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 16 Jun 2014 19:28:23 +0400 Subject: [Nek5000-users] Monitor points, location probe In-Reply-To: References: Message-ID: ?Thank you! ? ? ? ? ? ? ? ? ? ? ? Works great after a little change real work1(lt), work2(lt), work3(lt) ? Van 6/15/2014 4:13:03 PM ???????????? (nek5000-users at lists.mcs.anl.gov) ???????: Hi,You can make it much simpler! Simply do for instance: real work1(lx1,ly1,lz1,lelt), work2(lx1,ly1,lz1,lelt), work3(lx1,ly1,lz1,lelt) ... compute your dtdx dtdy dtdz call opcopy(work1,work2,work3,vx,vy,vz) ? ?! Save vx vy vz for later call opcopy(vx,vy,vz,dtdx,dtdy,dtdz) ? ? ? ? ? ! Save dtdx into vx for the hpts output call hpts call opcopy(vx,vy,vz,work1,work2,work3) ? ?! Restore vx vy vz That should do the trick I guess. Cheers, JC 2014-06-15 9:07 GMT+02:00 : I need to monitor scalar gradient (scalar is modelled with temperature as in examples.pdf). So I have inserted in USERCHK ? ? ?parameter (lt=lx1*ly1*lz1*lelt) ? ? ?common /ilgrad/ dtdx(lt),dtdy(lt),dtdz(lt) ? ? ?if ((mod(istep,iostep).eq.0).and.(istep.ge.iostep)) then ? ? ?call gradm1(dtdx,dtdy,dtdz,t) ? ? ?endif ? ? ?call hpts() Next there are two options to monitor a quantity 1. in .rea file like ?***** HISTORY AND INTEGRAL DATA ***** 001 ? POINTS. ?Hcode, I,J,H,IEL UV PT ? ?H ? ? ?3 ? ?3 ? ?1 ? ?1 But I dont know how to tell it that I want instead of UV, and also I don't know how to calculate number of element IEL from physical location. 2. hpts.in file you can input physical coordinates of a location, but in hpts.out only the following variables # time ?vx ?vy ?[vz] ?pr ?T ?PS1 ?PS2 ?... are being stored. So I tried to modify nek5000/branches/mvmesh/postpro.f in the following way: first I put ? ? ?parameter (lt=lx1*ly1*lz1*lelt) ? ? ?common /ilgrad/ dtdx(lt),dtdy(lt),dtdz(lt) in the beginning of subroutine hpts and later in this routine changed the code: ? ? ?! pack working array ? ? ?nflds = 0 ? ? ?if(ifvo) then ? ? ? ?call copy(wrk(1,1),vx,ntot) ? ? ? ?call copy(wrk(1,2),vy,ntot) ? ? ? ?if(if3d) call copy(wrk(1,3),vz,ntot) ? ? ? ?nflds = ndim ? ? ?endif ? ? ?if(ifpo) then ? ? ? ?nflds = nflds + 1 ? ? ? ?call copy(wrk(1,nflds),pm1,ntot) ? ? ?endif ? ? ?if(ifto) then ? ? ? ?nflds = nflds + 1 ? ? ? ?call copy(wrk(1,nflds),t,ntot) ? ? ?endif ? ? ? ?nflds = nflds + 1 ? ? ? ? ? ? ? ? ? ? ? ?!!!!!!!!!inserted ? ? ? ?call copy(wrk(1,nflds),dtdx,ntot) ? ? ? ?!!!!!!!!!inserted ? ? ? ?nflds = nflds + 1 ? ? ? ? ? ? ? ? ? ? ? ?!!!!!!!!!inserted ? ? ? ?call copy(wrk(1,nflds),dtdy,ntot) ? ? ? ?!!!!!!!!!inserted ? ? ?do i = 1,ldimt ? ? ? ? if(ifpsco(i)) then ? ? ? ? ? nflds = nflds + 1 ? ? ? ? ? call copy(wrk(1,nflds),T(1,1,1,1,i+1),ntot) ? ? ? ? endif ? ? ?enddo ? ? ?It was compiled without problem, but running the program yielded no change in hpts.out, as before there are only 5 columns # time ?vx ?vy ?[vz] ?pr ?T ? Please help _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -- Jean-Christophe Loiseau Homepage From nek5000-users at lists.mcs.anl.gov Mon Jun 16 10:29:49 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 16 Jun 2014 19:29:49 +0400 Subject: [Nek5000-users] Time-dependant boundary condition In-Reply-To: References: Message-ID: Works greate! Van > 6/9/2014 4:06:05 PM ???????????? (nek5000-users at lists.mcs.anl.gov) ???????: > > In userbc: > > ??????ux = cos(pi*y)*cos(2.*pi*time) > ??????uy = 0. > > Paul > > ________________________________________ > From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > Sent: Monday, June 09, 2014 2:30 AM > To: nek5000-users at lists.mcs.anl.gov > Subject: [Nek5000-users] Time-dependant boundary condition > > How should I impose time-dependant BC for velocity on the left vertical boundaty for a 2D box geometry. > The velocity profile should be > Vx=cos(pi*y)*cos(2*pi*t) > Vy=0 > > To illustrate the idea here are the pictures. > Instead of constant velocity Vx=c on the left (inflow) boundary of a channel > V __________________ > ??| > ??| > ??| > ??|__________________ > > I would impose Vx=cos(pi*y)*cos(2*pi*t) > so for t = 0 velocity profile is > ____________________ > \ > \ > ??\ > ???\_________________ > for t=1 velocity profile is > ????_________________ > ???/ > ??/ > / > /____________________ > > and so on. > > I know it should be possible in nek5000, but still not very familiar with syntax and fortran. > > Thank you in advance. > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > From nek5000-users at lists.mcs.anl.gov Mon Jun 16 14:23:52 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 16 Jun 2014 14:23:52 -0500 Subject: [Nek5000-users] Reg: error in Genmap In-Reply-To: References: Message-ID: I consider your suggestions Paul. I modified manually. I assume from what paul suggestion, there is error in the way the mesh points are given. I'm trying to recheck how the .rea file can be modified using prenek. I already posted on modifying mesh & BC in .rea using prenek, but it didn't work. Ravi On Sun, Jun 15, 2014 at 11:50 PM, wrote: > Hi Ravi, > > How did you modify the .rea file? > Katherine > > > On Sun, Jun 15, 2014 at 6:11 PM, wrote: > >> >> Dear Ravi, >> >> My guess is that your mesh is somehow invalid. >> >> A quick look at the genmap.f source indicates that the first number >> in front of the SELF error indicator is the element number, which would >> imply something wrong with element number 1. >> >> Paul >> >> ------------------------------ >> *From:* nek5000-users-bounces at lists.mcs.anl.gov [ >> nek5000-users-bounces at lists.mcs.anl.gov] on behalf of >> nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] >> *Sent:* Sunday, June 15, 2014 3:05 PM >> *To:* nek5000-users at lists.mcs.anl.gov >> *Subject:* [Nek5000-users] Reg: error in Genmap >> >> Hello all, >> >> I get the following error, >> >> Input mesh tolerance (default 0.2): >> NOTE: smaller is better, but generous is more forgiving for bad meshes. >> .005 >> reading .rea file data ... >> start locglob_lexico: 8 8 64 5.000000000000000E-003 >> locglob: 1 1 64 >> locglob: 2 3 64 >> locglob: 3 9 64 >> locglob: 1 18 64 >> locglob: 2 18 64 >> locglob: 3 18 64 >> locglob: 1 18 64 >> locglob: 2 18 64 >> locglob: 3 18 64 >> >> 1 2 4 Matrix: SELF!! >> 1 SELF!! 1 3 1 3 >> 2 SELF!! 7 9 7 9 >> cont: SELF!! 1 ?? >> >> ABORT: SELF-CHK 1 5 1 0 >> Try to tighten the mesh tolerance! >> >> 0 quit >> >> >> How to address this problem. I manually modified the mesh coniditons in >> the .rea file. >> I tried to look out for this in the previous posts. Nothing worked for my >> case from the suggestions. >> >> Thanks, >> >> >> Ravi Kiran Pendyala, >> >> >> >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> >> > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jun 16 16:55:06 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 17 Jun 2014 01:55:06 +0400 Subject: [Nek5000-users] what exactly is thermal flux and how to set it on different sides? Message-ID: 1. if n is a normal direction, is it that flux = dTEMP/dn (what I supposed) or is it a real thermal flux flux = k dTEMP/dn with k as conductivity? A am asking because I dont understand the source of instability in solution when I simulate a stratified flow between two boundaries with TEMP=1-z as initial condition When I set flux on upper and lower boundaries to 0 the program works, but when I set it to -1 the program blows up in few steps. 2. The next question is how to set differen user defined BC on different boundaries if you set in .rea files lowcase "f" for two boundaries it means that the BC is determined by "flux" in userbc subroutine, but I have different expressions for fluxes for different sides. I have not found this question described in docs. 3. And sorry for another qiestion: In benard example there are files like ray_nn.rea ray_dn.rea ray_dd.rea for different combinations of BCs. But only one .usr file - ray_cr.usr. I suppose that these BCs must be defined in userbc subroutine of .usr file. So how does it work? Van From nek5000-users at lists.mcs.anl.gov Mon Jun 16 17:04:27 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 16 Jun 2014 22:04:27 +0000 Subject: [Nek5000-users] what exactly is thermal flux and how to set it on different sides? In-Reply-To: References: Message-ID: Van, It is a real flux: q" = k dT/dn If it is blowing up it's probably because of the nonlinear response of the Boussinesq equations to the I.C./B.C. combination that you are using --- you might be able to cure this with sufficiently small timestep. For inhomogeneous Neumann conditions there is no stability issue of the type that's encountered with Robin (i.e., Newton law of cooling) BC's, where a sign change can indeed lead to an instability. 2. I like things like: if (y.lt.0.5) flux = 1 if (y.gt.0.5) flux=2 as discriminators for different surfaces. 3. The BC types are assigned in the .rea file. The functionality for each type is prescribed in the .usr file. Having extra definitions in the .usr file doesn't matter if there is no reference to them. Paul ________________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Monday, June 16, 2014 4:55 PM To: Nek5000 Users Subject: [Nek5000-users] what exactly is thermal flux and how to set it on different sides? 1. if n is a normal direction, is it that flux = dTEMP/dn (what I supposed) or is it a real thermal flux flux = k dTEMP/dn with k as conductivity? A am asking because I dont understand the source of instability in solution when I simulate a stratified flow between two boundaries with TEMP=1-z as initial condition When I set flux on upper and lower boundaries to 0 the program works, but when I set it to -1 the program blows up in few steps. 2. The next question is how to set differen user defined BC on different boundaries if you set in .rea files lowcase "f" for two boundaries it means that the BC is determined by "flux" in userbc subroutine, but I have different expressions for fluxes for different sides. I have not found this question described in docs. 3. And sorry for another qiestion: In benard example there are files like ray_nn.rea ray_dn.rea ray_dd.rea for different combinations of BCs. But only one .usr file - ray_cr.usr. I suppose that these BCs must be defined in userbc subroutine of .usr file. So how does it work? Van _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Mon Jun 16 19:49:54 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 16 Jun 2014 20:49:54 -0400 Subject: [Nek5000-users] XL compiler w/ moab Message-ID: Hello all, I just wondered if anyone has experience in linking moab to nek on BGQ platforms. I am looking for appropriate libraries for USR_LFLAGS in makenek for IBM XL compilers, using to link moab to nek. Thanks, Mohsen From nek5000-users at lists.mcs.anl.gov Tue Jun 17 10:33:39 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 17 Jun 2014 17:33:39 +0200 Subject: [Nek5000-users] how to define boundary conditions with a specified function. Message-ID: Hello everyone, Now I have a problem. that how to define boundary conditions in the .usr file. I know that I can write some code in the usrbc() what I want do is like this if (y .eq. 1) then u=2*x endif where y is the value of boundary coodinates . what I wrote is like if (ym1(1,1,11) .eq. 1) then ux=2*x uy=0 uz=0 endif it can be compiled, but not imposed. so what should I do? How can I know the relation between ux(i,j,k,e) and index informations? thanks. Wei From nek5000-users at lists.mcs.anl.gov Tue Jun 17 10:36:44 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 17 Jun 2014 15:36:44 +0000 Subject: [Nek5000-users] how to define boundary conditions with a specified function. In-Reply-To: References: Message-ID: Wei, I would just do ux=0 uy=0 uz=0 eps = 1.e-4 if (abs(y-1.).le.eps) ux=2*x That will work. Paul ________________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Tuesday, June 17, 2014 10:33 AM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] how to define boundary conditions with a specified function. Hello everyone, Now I have a problem. that how to define boundary conditions in the .usr file. I know that I can write some code in the usrbc() what I want do is like this if (y .eq. 1) then u=2*x endif where y is the value of boundary coodinates . what I wrote is like if (ym1(1,1,11) .eq. 1) then ux=2*x uy=0 uz=0 endif it can be compiled, but not imposed. so what should I do? How can I know the relation between ux(i,j,k,e) and index informations? thanks. Wei _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Tue Jun 17 11:42:42 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 17 Jun 2014 18:42:42 +0200 Subject: [Nek5000-users] how to define boundary conditions with a specified function. In-Reply-To: References: Message-ID: Thanks you Paul, for your so quickly response and help!!. It works. Wei On Jun 17, 2014, at 5:36 PM, nek5000-users at lists.mcs.anl.gov wrote: > ux=0 > uy=0 > uz=0 > eps = 1.e-4 > if (abs(y-1.).le.eps) ux=2*x -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Jun 17 13:56:10 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 17 Jun 2014 14:56:10 -0400 Subject: [Nek5000-users] XL compiler w/ moab In-Reply-To: <81761CAE-7503-4A99-BB32-BEE1B4EF331E@mail.utoronto.ca> References: <81761CAE-7503-4A99-BB32-BEE1B4EF331E@mail.utoronto.ca> Message-ID: Hello again, Following my previous post, I tried the following libraries (as recommended by our cluster admin): libibmc++.a libibmc++.so libxl.a libxlopt.a libmc++ But apparently the link is not yet provided by these libraries as the following error message appears: "make: [obj/moab.o] Error 40" "make: waiting for unfinished jobs..." Note that I have no problem compiling Nek w/o Moab on BGQ. So I wondered if anyone has similar issue in compiling, probably related to linking. I attached the compiler output and makenek file. Thanks, Mohsen ?? On 16-Jun-14, at 8:49 PM, Mohsen Behzad wrote: > Hello all, > I just wondered if anyone has experience in linking moab to nek on > BGQ platforms. I am looking for appropriate libraries for > USR_LFLAGS in makenek for IBM XL compilers, using to link moab to nek. > > Thanks, > Mohsen > -------------- next part -------------- An HTML attachment was scrubbed... URL: -------------- next part -------------- A non-text attachment was scrubbed... Name: compiler.out Type: application/octet-stream Size: 27091 bytes Desc: not available URL: -------------- next part -------------- An HTML attachment was scrubbed... URL: -------------- next part -------------- A non-text attachment was scrubbed... Name: makenek Type: application/octet-stream Size: 1846 bytes Desc: not available URL: -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Jun 18 03:46:24 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 18 Jun 2014 10:46:24 +0200 Subject: [Nek5000-users] how to define boundary conditions with a specified function. In-Reply-To: References: Message-ID: Hello Neks, Again, since u=2*x, then u_x=2, the boundary conditions for uy should be v_y = -u_x = -2. when I set the boundary type as "v" and it is aligned/parallel with X-axis. the value of uy will be equal to zero by default. So in this case is it feasible to set "v" as boundary type? I find here http://lists.mcs.anl.gov/pipermail/nek5000-users/2011-April/001312.html and http://lists.mcs.anl.gov/pipermail/nek5000-users/2010-December/001184.html have a similar question with mine. Is there someone can give me some advices? thank you!! Wei On Jun 17, 2014, at 6:42 PM, nek5000-users at lists.mcs.anl.gov wrote: > Thanks you Paul, for your so quickly response and help!!. It works. > > Wei > On Jun 17, 2014, at 5:36 PM, nek5000-users at lists.mcs.anl.gov wrote: > >> ux=0 >> uy=0 >> uz=0 >> eps = 1.e-4 >> if (abs(y-1.).le.eps) ux=2*x > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Jun 18 03:55:11 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 18 Jun 2014 03:55:11 -0500 Subject: [Nek5000-users] Reg: error in Genmap In-Reply-To: References: Message-ID: I am trying to create a cube from scratch. I get errors during meshing and giving boundary conditions. Could I get a possible help to start this up. Thanks, Ravi, On Mon, Jun 16, 2014 at 2:23 PM, wrote: > I consider your suggestions Paul. I modified manually. I assume from what > paul suggestion, there is error in the way the mesh points are given. I'm > trying to recheck how the .rea file can be modified using prenek. I already > posted on modifying mesh & BC in .rea using prenek, but it didn't work. > > > > Ravi > > > > On Sun, Jun 15, 2014 at 11:50 PM, wrote: > >> Hi Ravi, >> >> How did you modify the .rea file? >> Katherine >> >> >> On Sun, Jun 15, 2014 at 6:11 PM, wrote: >> >>> >>> Dear Ravi, >>> >>> My guess is that your mesh is somehow invalid. >>> >>> A quick look at the genmap.f source indicates that the first number >>> in front of the SELF error indicator is the element number, which would >>> imply something wrong with element number 1. >>> >>> Paul >>> >>> ------------------------------ >>> *From:* nek5000-users-bounces at lists.mcs.anl.gov [ >>> nek5000-users-bounces at lists.mcs.anl.gov] on behalf of >>> nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] >>> *Sent:* Sunday, June 15, 2014 3:05 PM >>> *To:* nek5000-users at lists.mcs.anl.gov >>> *Subject:* [Nek5000-users] Reg: error in Genmap >>> >>> Hello all, >>> >>> I get the following error, >>> >>> Input mesh tolerance (default 0.2): >>> NOTE: smaller is better, but generous is more forgiving for bad meshes. >>> .005 >>> reading .rea file data ... >>> start locglob_lexico: 8 8 64 5.000000000000000E-003 >>> locglob: 1 1 64 >>> locglob: 2 3 64 >>> locglob: 3 9 64 >>> locglob: 1 18 64 >>> locglob: 2 18 64 >>> locglob: 3 18 64 >>> locglob: 1 18 64 >>> locglob: 2 18 64 >>> locglob: 3 18 64 >>> >>> 1 2 4 Matrix: SELF!! >>> 1 SELF!! 1 3 1 3 >>> 2 SELF!! 7 9 7 9 >>> cont: SELF!! 1 ?? >>> >>> ABORT: SELF-CHK 1 5 1 0 >>> Try to tighten the mesh tolerance! >>> >>> 0 quit >>> >>> >>> How to address this problem. I manually modified the mesh coniditons >>> in the .rea file. >>> I tried to look out for this in the previous posts. Nothing worked for >>> my case from the suggestions. >>> >>> Thanks, >>> >>> >>> Ravi Kiran Pendyala, >>> >>> >>> >>> >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>> >>> >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> >> > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Jun 18 04:14:16 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 18 Jun 2014 11:14:16 +0200 Subject: [Nek5000-users] snapshots in ascii file Message-ID: Hi Neks, I would like to save a data set of snapshots in ascii, containing position and velocity. I've tried to modify the userchk subroutine in the following way: real us(lx1,ly1,lz1,lelt), vs(lx1,ly1,lz1,lelt) integer i, j, k, l call opcopy(us,vs,ws,vx,vy,vz) ... open(223,file='example.dat') do i=1,lx do j=1,ly do k=1,lz do l=1,lelt write(223,*) xm(i,j,k,l),ym(i,j,k,l),us(i,j,k,l),vs(i,j,k,l) end do end do end do end do close(223) but the example.dat file is empty. Could you help me? SL From nek5000-users at lists.mcs.anl.gov Wed Jun 18 04:16:57 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 18 Jun 2014 11:16:57 +0200 Subject: [Nek5000-users] snapshots in ascii file In-Reply-To: References: Message-ID: Hi, > do i=1,lx > do j=1,ly > do k=1,lz Maybe you meant lx1, ly1, lz1 here. Most probably (unless you defined them somewhere else), lx, ly, lz are 0, which would explain this: > but the example.dat file is empty. -- Ismael From nek5000-users at lists.mcs.anl.gov Wed Jun 18 07:28:40 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 18 Jun 2014 12:28:40 +0000 Subject: [Nek5000-users] snapshots in ascii file In-Reply-To: References: , Message-ID: Also, it would be far better to do do l=1,nelv do k=1,nz1 do j=1,ny1 do i=1,nx1 write(223,*) xm1(i,j,k,l),ym1(i,k,j,l),vx(i,j,k,l),vy(i,j,k,l) enddo enddo enddo enddo or better still: n=nx1*ny1*nz1*nelt do i=1,n write(223,*) xm1(i,1,1,1),ym1(i,1,1,1),vx(i,1,1,1),vy(i,1,1,1) enddo Why? With your original scheme you are not accessing the data with unit stride, which means you're generating a lot of unnecessary cache misses and unwanted data traffic. Also, your original scheme writes out all the declared elements (lelt) rather than just the active ones (nelt). Both the approaches above yield the same result with the second one preferred because it's much easier for the compiler to generate vector code (in general, but in this case i/o actually inhibits vectorization). Also, the second case takes up far less precious screen space, which makes the overall code easier to debug. Paul ________________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Wednesday, June 18, 2014 4:16 AM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] snapshots in ascii file Hi, > do i=1,lx > do j=1,ly > do k=1,lz Maybe you meant lx1, ly1, lz1 here. Most probably (unless you defined them somewhere else), lx, ly, lz are 0, which would explain this: > but the example.dat file is empty. -- Ismael _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Thu Jun 19 03:46:04 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 19 Jun 2014 12:46:04 +0400 Subject: [Nek5000-users] what exactly is thermal flux and how to set it ondifferent sides? In-Reply-To: References: Message-ID: Paul, Thank you very much for the quick answer, now it works fine Van > 6/17/2014 2:04:30 AM ???????????? (nek5000-users at lists.mcs.anl.gov) ???????: > > > Van, > > It is a real flux: ????q" = k dT/dn > > If it is blowing up it's probably because of the nonlinear response of the Boussinesq > equations to the I.C./B.C. combination that you are using --- you might be able to > cure this with sufficiently small timestep. ???For inhomogeneous Neumann conditions > there is no stability issue of the type that's encountered with Robin (i.e., Newton > law of cooling) BC's, where a sign change can indeed lead to an instability. > > 2. ??I like things like: > > if (y.lt.0.5) flux = 1 > if (y.gt.0.5) flux=2 > > as discriminators for different surfaces. > > 3. The BC types are assigned in the .rea file. ???The functionality for each type > is prescribed in the .usr file. ???Having extra definitions in the .usr file doesn't matter > if there is no reference to them. > > Paul > > ________________________________________ > From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > Sent: Monday, June 16, 2014 4:55 PM > To: Nek5000 Users > Subject: [Nek5000-users] what exactly is thermal flux and how to set it on ??????different sides? > > 1. > if n is a normal direction, > is it that > flux = dTEMP/dn (what I supposed) > or is it a ??real thermal flux > flux = k dTEMP/dn with k as conductivity? > > A am asking because I dont understand the source of instability in solution when I simulate a stratified flow > between two boundaries with > TEMP=1-z as initial condition > When I set flux on upper and lower boundaries to 0 ??the program works, > but when I set it to -1 the program blows up in few steps. > > 2. The next question is how to set differen user defined BC on different boundaries > > if you set in .rea files lowcase "f" > for two boundaries it means that the BC is determined by "flux" in userbc subroutine, > but I have different expressions for fluxes for different sides. > I have not found this question described in docs. > > 3. And sorry for another qiestion: > In benard example there are files like ray_nn.rea ray_dn.rea ray_dd.rea for different combinations of BCs. > But only one .usr file - ray_cr.usr. > I suppose that these BCs must be defined in userbc subroutine of .usr file. > So how does it work? > > Van > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > From nek5000-users at lists.mcs.anl.gov Thu Jun 19 13:10:33 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 19 Jun 2014 14:10:33 -0400 Subject: [Nek5000-users] Beginner to NEK5000-Need help Message-ID: Hi, My name is Arash and I have started to work on NEK5000 code recently. I have some questions and need help! Are there any PDF or documents about the way in which Nek discritizes the equations? I dont know in where should I start to know the code. Thanks Arash From nek5000-users at lists.mcs.anl.gov Thu Jun 19 15:20:56 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 19 Jun 2014 13:20:56 -0700 Subject: [Nek5000-users] Beginner to NEK5000-Need help In-Reply-To: References: Message-ID: Hi, You can look at Nek5000 Primer for an introduction. You can google it easily. Also some other good references are: http://www.mcs.anl.gov/~fischer/nek5000/fischer_nek5000_dec2010.pdf http://www.mcs.anl.gov/~fischer/new.pdf Thanks, Tanmoy On Thu, Jun 19, 2014 at 11:10 AM, wrote: > Hi, > > My name is Arash and I have started to work on NEK5000 code recently. > I have some questions and need help! > Are there any PDF or documents about the way in which Nek discritizes the > equations? > I dont know in where should I start to know the code. > > Thanks > > Arash > > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Jun 19 15:25:02 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 19 Jun 2014 22:25:02 +0200 Subject: [Nek5000-users] Beginner to NEK5000-Need help In-Reply-To: References: Message-ID: Also, I find the following useful Thesis of Couzy SPECTRAL ?L?MENT DISCRETIZATION OF THE ... The book High-Order Methods for Incompressible Fluid FlowM. O. Deville, P. F. Fischer, E. H. Mund praveen On Thu, Jun 19, 2014 at 10:20 PM, wrote: > Hi, > > You can look at Nek5000 Primer for an introduction. You can google it > easily. > > Also some other good references are: > http://www.mcs.anl.gov/~fischer/nek5000/fischer_nek5000_dec2010.pdf > > http://www.mcs.anl.gov/~fischer/new.pdf > > Thanks, > Tanmoy > > > > On Thu, Jun 19, 2014 at 11:10 AM, wrote: > >> Hi, >> >> My name is Arash and I have started to work on NEK5000 code recently. >> I have some questions and need help! >> Are there any PDF or documents about the way in which Nek discritizes the >> equations? >> I dont know in where should I start to know the code. >> >> Thanks >> >> Arash >> >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> > > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Jun 19 21:26:15 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 20 Jun 2014 02:26:15 +0000 Subject: [Nek5000-users] XL compiler errors Message-ID: Hello all, I just tried to compile Nek with XL compiler, which seems to be pickier than others, and got a few errors (not severe though). I wondered if anyone can confirm whether the corrections, which are made by compiler, are in the right way. Here are the errors: "$HOME/nek5_svn/trunk/nek/jl/lob_bnd.c", line 153.29: 1506-1418 (E) Assignment between restrict pointers "br" and "br_" is not allowed. Only outer-to-inner scope assignments between restrict pointers are allowed. "$HOME/nek5_svn/trunk/nek/jl/lob_bnd.c", line 154.22: 1506-1418 (E) Assignment between restrict pointers "b" and "b_" is not allowed. Only outer-to-inner scope assignments between restrict pointers are allowed. "$HOME/nek5_svn/trunk/nek/jl/lob_bnd.c", line 165.5: 1506-1418 (E) Assignment between restrict pointers "br" and "br_" is not allowed. Only outer-to-inner scope assignments between restrict pointers are allowed. "$HOME/nek5_svn/trunk/nek/jl/lob_bnd.c", line 168.7: 1506-1418 (E) Assignment between restrict pointers "b" and "b_" is not allowed. Only outer-to-inner scope assignments between restrict pointers are allowed. ... ..... "$HOME/nek5_svn/trunk/nek/3rd_party/moab.f", line 564.15: 1514-133 (E) Variable declared as an integer pointer was previously specified in a type declaration statement. The type specification is ignored. "$HOME/nek5_svn/trunk/nek/3rd_party/moab.f", line 875.16: 1514-133 (E) Variable declared as an integer pointer was previously specified in a type declaration statement. The type specification is ignored. "$HOME/nek5_svn/trunk/nek/3rd_party/moab.f", line 928.15: 1514-133 (E) Variable declared as an integer pointer was previously specified in a type declaration statement. The type specification is ignored. "$HOME/nek5_svn/trunk/nek/3rd_party/moab.f", line 1846.16: 1514-133 (E) Variable declared as an integer pointer was previously specified in a type declaration statement. The type specification is ignored. Thanks, Mohsen From nek5000-users at lists.mcs.anl.gov Fri Jun 20 14:14:38 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 20 Jun 2014 14:14:38 -0500 Subject: [Nek5000-users] Element mesh mismatch Message-ID: Hello all, I got the following error which had a very similar post in the archives *My error: * regenerate geometry data 1 vol_t,vol_v: 435.175813056833 435.175813056833 done :: regenerate geometry data 1 verify mesh topology 0.00000000000000 6.28318530717959 Xrange 0.00000000000000 6.28318530717959 Yrange 0.00000000000000 11.0231321178589 Zrange WARNING1 Element mesh mismatch at: i,j,k,ie: 2 1 1 1 Near X = 0.62933884E-01 0.0000000 0.0000000 , d: 6.1573175 0.0000000 0.31830989 call exitt: dying ... *Link to the post : * http://lists.mcs.anl.gov/pipermail/nek5000-users/2009-September/000039.html *I** did not understand the suggestion given for this. * Thanks, Ravi -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Sun Jun 22 16:54:24 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 22 Jun 2014 17:54:24 -0400 Subject: [Nek5000-users] (no subject) Message-ID: Dear NEK Users, I need some help in modelling fluid-structure using NEK5000. Based on the inputs from mailing list, I am able to extract the forces on a cylinder in laminar flow. The physical problem I am trying to model is vortex-induced vibration (VIV) of a circular cylinder. I will be restricting the motion of cylinder to be only along cross flow direction, driven by the lift, F_L = dragy(1) --------------------------------(1) My next step is to use the lift force to solve dynamics of the cylinder using: M ddy + C dy + K y = F_L --------------------(2) I am asking my questions first; please find additional details below the questions. 1. Q1. How can I assign the mesh velocity only to the portion of boundary with identifier ?mv? in *.rea file? In my pseudo code and program structure of *.usr file below, I tried to assign mesh velocity by calling a subroutine in ?u_meshv? within the subroutine ?userbc? by following the ocyl.usr example. If I do so, my cylinder dynamics is being called for each node, since ?usrbc? is called for each node. I would like to avoid this, since I would like to compute cylinder dynamics only once per time step and assign the resulting velocity to moving boundary. Q2. How can I get the lift force for each time-step? Currently, I am calling the ?torque_calc? in ?userchk? and using the common block ?common /ctorq/? in all the subroutine that I need the lift force for further computation. My program setup: I am using the moving cylinder examples from the NEK5000 examples ?ocyl? and adding/modifying subroutines to accomplish solution of the cylinder coupled with fluid & mesh motion solution in a staggered fashion. I am providing my pseudo-code/code snippet to illustrate my approach. 1. I will call the u_meshv from the userbc subroutine to set the mesh velocity on the moving boundary. ***************************** usrbc******************************* subroutine usrbc ? ? if (x .lt. -1.1) then ux=1 uy=0. uz=0. else call u_meshv(ux,uy,uz,x,y,z) endif ***************************** ********************************** 2. In u_meshv, I will call a subroutine to ?cyl_dynamics? which will solve the second-order differential equation (2) above for acceleration, velocity, and displacement (an, vn, dn at nth time step and an1, vn1, dn1 at (n+1)th time step). *************************u_meshv******************************* subroutine u_meshv(ux,uy,uz,x,y,z) ? common /cyldyn/ dn,vn,an,dn1,vn1,an1 ? do FSI_ITR call cyl_dynamics if (cyl. Dynamics is in equilibrium with fluid dynamics) then goto XXXX ! exit the loop else call cyl_dynamics endif ********************************************************** ************************* cyl_dynamics ******************************* subroutine cyl_dynamics ? common /cyldyn/ dn,vn,an,dn1,vn1,an1 ? c Code for calculation cylinder dynamics for a given F_L ********************************************************** Any help in implementing this fluid-structure interaction problem is much appreciated. If there is an example which performs such fluid-structure couple solution please let me know. Please let me know if I need to provide any additional details to explain my problem. -- Ravi Kumar T R University of Illinois at Urbana-Champaign ph : +1 217 778 7538 http://lndvl.mechse.illinois.edu/ -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Sun Jun 22 16:55:40 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 22 Jun 2014 17:55:40 -0400 Subject: [Nek5000-users] Fluid-structure interaction setup Message-ID: Dear NEK Users, I need some help in modelling fluid-structure using NEK5000. Based on the inputs from mailing list, I am able to extract the forces on a cylinder in laminar flow. The physical problem I am trying to model is vortex-induced vibration (VIV) of a circular cylinder. I will be restricting the motion of cylinder to be only along cross flow direction, driven by the lift, F_L = dragy(1) --------------------------------(1) My next step is to use the lift force to solve dynamics of the cylinder using: M ddy + C dy + K y = F_L --------------------(2) I am asking my questions first; please find additional details below the questions. 1. Q1. How can I assign the mesh velocity only to the portion of boundary with identifier ?mv? in *.rea file? In my pseudo code and program structure of *.usr file below, I tried to assign mesh velocity by calling a subroutine in ?u_meshv? within the subroutine ?userbc? by following the ocyl.usr example. If I do so, my cylinder dynamics is being called for each node, since ?usrbc? is called for each node. I would like to avoid this, since I would like to compute cylinder dynamics only once per time step and assign the resulting velocity to moving boundary. Q2. How can I get the lift force for each time-step? Currently, I am calling the ?torque_calc? in ?userchk? and using the common block ?common /ctorq/? in all the subroutine that I need the lift force for further computation. My program setup: I am using the moving cylinder examples from the NEK5000 examples ?ocyl? and adding/modifying subroutines to accomplish solution of the cylinder coupled with fluid & mesh motion solution in a staggered fashion. I am providing my pseudo-code/code snippet to illustrate my approach. 1. I will call the u_meshv from the userbc subroutine to set the mesh velocity on the moving boundary. ***************************** usrbc******************************* subroutine usrbc ? ? if (x .lt. -1.1) then ux=1 uy=0. uz=0. else call u_meshv(ux,uy,uz,x,y,z) endif ***************************** ********************************** 2. In u_meshv, I will call a subroutine to ?cyl_dynamics? which will solve the second-order differential equation (2) above for acceleration, velocity, and displacement (an, vn, dn at nth time step and an1, vn1, dn1 at (n+1)th time step). *************************u_meshv******************************* subroutine u_meshv(ux,uy,uz,x,y,z) ? common /cyldyn/ dn,vn,an,dn1,vn1,an1 ? do FSI_ITR call cyl_dynamics if (cyl. Dynamics is in equilibrium with fluid dynamics) then goto XXXX ! exit the loop else call cyl_dynamics endif ********************************************************** ************************* cyl_dynamics ******************************* subroutine cyl_dynamics ? common /cyldyn/ dn,vn,an,dn1,vn1,an1 ? c Code for calculation cylinder dynamics for a given F_L ********************************************************** Any help in implementing this fluid-structure interaction problem is much appreciated. If there is an example which performs such fluid-structure couple solution please let me know. Please let me know if I need to provide any additional details to explain my problem. -- Ravi Kumar T R University of Illinois at Urbana-Champaign ph : +1 217 778 7538 http://lndvl.mechse.illinois.edu/ -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Sun Jun 22 17:22:25 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 22 Jun 2014 22:22:25 +0000 Subject: [Nek5000-users] Fluid-structure interaction setup In-Reply-To: References: Message-ID: Hi Ravi, I have a couple of ideas about this - but they likely need some development. Can you contact me off-list? Paul Fischer ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Sunday, June 22, 2014 4:55 PM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] Fluid-structure interaction setup Dear NEK Users, I need some help in modelling fluid-structure using NEK5000. Based on the inputs from mailing list, I am able to extract the forces on a cylinder in laminar flow. The physical problem I am trying to model is vortex-induced vibration (VIV) of a circular cylinder. I will be restricting the motion of cylinder to be only along cross flow direction, driven by the lift, F_L = dragy(1) --------------------------------(1) My next step is to use the lift force to solve dynamics of the cylinder using: M ddy + C dy + K y = F_L --------------------(2) I am asking my questions first; please find additional details below the questions. 1. Q1. How can I assign the mesh velocity only to the portion of boundary with identifier ?mv? in *.rea file? In my pseudo code and program structure of *.usr file below, I tried to assign mesh velocity by calling a subroutine in ?u_meshv? within the subroutine ?userbc? by following the ocyl.usr example. If I do so, my cylinder dynamics is being called for each node, since ?usrbc? is called for each node. I would like to avoid this, since I would like to compute cylinder dynamics only once per time step and assign the resulting velocity to moving boundary. Q2. How can I get the lift force for each time-step? Currently, I am calling the ?torque_calc? in ?userchk? and using the common block ?common /ctorq/? in all the subroutine that I need the lift force for further computation. My program setup: I am using the moving cylinder examples from the NEK5000 examples ?ocyl? and adding/modifying subroutines to accomplish solution of the cylinder coupled with fluid & mesh motion solution in a staggered fashion. I am providing my pseudo-code/code snippet to illustrate my approach. 1. I will call the u_meshv from the userbc subroutine to set the mesh velocity on the moving boundary. ***************************** usrbc******************************* subroutine usrbc ? ? if (x .lt. -1.1) then ux=1 uy=0. uz=0. else call u_meshv(ux,uy,uz,x,y,z) endif ***************************** ********************************** 2. In u_meshv, I will call a subroutine to ?cyl_dynamics? which will solve the second-order differential equation (2) above for acceleration, velocity, and displacement (an, vn, dn at nth time step and an1, vn1, dn1 at (n+1)th time step). *************************u_meshv******************************* subroutine u_meshv(ux,uy,uz,x,y,z) ? common /cyldyn/ dn,vn,an,dn1,vn1,an1 ? do FSI_ITR call cyl_dynamics if (cyl. Dynamics is in equilibrium with fluid dynamics) then goto XXXX ! exit the loop else call cyl_dynamics endif ********************************************************** ************************* cyl_dynamics ******************************* subroutine cyl_dynamics ? common /cyldyn/ dn,vn,an,dn1,vn1,an1 ? c Code for calculation cylinder dynamics for a given F_L ********************************************************** Any help in implementing this fluid-structure interaction problem is much appreciated. If there is an example which performs such fluid-structure couple solution please let me know. Please let me know if I need to provide any additional details to explain my problem. -- Ravi Kumar T R University of Illinois at Urbana-Champaign ph : +1 217 778 7538 http://lndvl.mechse.illinois.edu/ -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jun 23 08:20:47 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 23 Jun 2014 15:20:47 +0200 Subject: [Nek5000-users] test of the time average of turbChannel--what's wrong? Message-ID: Hi Paul, I just wanted to come back to this point as it seems the correction regarding the turbchannel case in the new version of nek is quite sound; though, the command "timel = time" seems to sit in a wrong position. To what I understand it must appear after the 'if' statement with regards the 'write' block to make sure the timel is saved correctly per timestep. Cheers Azad ________________________________ Hi Xianbei, You are correct that dtime should be equal to DT. If you look at avg_all() in navier5.f in the main nek source directory, this is what happens because timel is updated after the averaging. In the turbchannel case, this was not done - so I've now modified the .usr file to reflect this. I would suggest to simply use the avg_all code to do the time averaging and then to use those average fields to generate profiles. Thanks for pointing out the problem with the turbChannel example. Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Saturday, May 31, 2014 10:38 PM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] test of the time average of turbChannel--what's wrong? Hi Xianbei, The usr files are meant to be modified by the users, so you can adjust it to suit your needs. Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Saturday, May 31, 2014 9:58 PM To: Nek5000 Subject: [Nek5000-users] test of the time average of turbChannel--what's wrong? Hi, all: I read about the time average method in the turbChannel.usr/userchk,here is the origin codes: if(icalld.eq.0) then call rzero(uavg,n) call rzero(urms,n) call rzero(vrms,n) call rzero(wrms,n) call rzero(uvms,n) atime = 0. timel = time call planar_average_s(yy ,ym1 ,w1,w2) icalld = 1 endif dtime = time - timel atime = atime + dtime if (atime.ne.0. .and. dtime.ne.0.) then beta = dtime/atime alpha = 1.-beta ifverbose = .false. call avg1(uavg,vx ,alpha,beta,n,'uavg',ifverbose) As seen , atime and timel is initialized by 0 and time, so when time=time+DT, dtime=DT, atime=DT, so the first average value is vx(t=DT), when time=time+2*DT, dtime=2*DT(timel is not changed, just equal to the initial value ),atime=3*DT, here question comes: this will lead to vxmean(t=2*DT)=2/3*vx(t=DT)+1/3*vx(t=2*DT), this is not what we respect. The right one is make sure that dtime=DT all the time. Also, I do a test to verify this.In order to be more reliable, the velocity isn't nomorlized by u_tau. First, calculate by 1 step and output the means.dat, so the value equal to the time=DT's #time = 2.0000000E-02 # y uup_tau Umean 0.000000000E+00 2.031155153E-02 0.000000000E+00 2.565198406E-03 2.031155153E-02 1.285886819E-02 then restart with the field from previous calculation and output the means.dat, this will output the value of time=2*DT's, #time = 4.0000000E-02 # y uup_tau Umean 0.000000000E+00 2.072569248E-02 0.000000000E+00 2.565205097E-03 2.072569248E-02 1.288671376E-02 At last, restart the calculation and run 2 steps to calculate the average of vx(time=DT) and vx(time=2*DT) #time = 4.0000000E-02 # y uup_tau Umean 0.000000000E+00 2.061649552E-02 0.000000000E+00 2.565198406E-03 2.061649552E-02 1.287524390E-02 As can be seen, the 2 step average is almost equal to the average of step 1 and step 2. So what's wrong with my understanding? Is timel alway updated to the previous time and make sure that dtime=constant? How? Can anyone help? Xianbei From nek5000-users at lists.mcs.anl.gov Mon Jun 23 08:50:53 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 23 Jun 2014 15:50:53 +0200 Subject: [Nek5000-users] Fully resolved fluid-structure interaction by NEK5000: a broadcast Message-ID: Hello, dear Nekers, Here I would like to draw your attention to our recently published paper 'http://pubs.rsc.org/en/content/articlelanding/2014/sm/c4sm01097c#!divAbstract '. We perform 3D direct numerical simulations by NEK5000 to help the design of a micro-fluidic device capable of differentiating and sorting biological cells based on their deformability. As far as we know, this is the first attempt of using NEK as a platform to fully resolve the fluid-structure interaction at low Reynolds number. Indeed, we use an accelerated boundary integral method (BIM) to solve the Stokes flow, one part of the solution is from the Stokes solver of NEK5000, and another from traditional boundary integral computations. As we employ a spherical-harmonics-based spectral method to interpretate the surface of the cell, the whole numerical framework is of almost spectral accuracy (not exactly due to BIM); as well as near the immersed interface. For traditional immersed boundary method or lattice Boltzmann method, the accuracy near the interface is normally around first to second order. Of course, we then restrict our simulations in the Stokes regime. Our manuscript regarding the whole implementation is not published yet, but is accessible as included in my Phd thesis, page 163 (http://kth.diva-portal.org/smash/record.jsf;jsessionid=c60f995693b968342b9e9c03c839?pid=diva2:703338). I recently obtained my Phd degree with Prof. Luca Brandt at KTH Mechanics. kind regards, Lailai -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jun 23 09:18:46 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 23 Jun 2014 14:18:46 +0000 Subject: [Nek5000-users] test of the time average of turbChannel--what's wrong? In-Reply-To: References: Message-ID: Thanks Azad -- so is it currently messed up? Or was it messed up before? (i.e., do I need to undo my recent change?) Thanks! Paul ________________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Monday, June 23, 2014 8:20 AM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] test of the time average of turbChannel--what's wrong? Hi Paul, I just wanted to come back to this point as it seems the correction regarding the turbchannel case in the new version of nek is quite sound; though, the command "timel = time" seems to sit in a wrong position. To what I understand it must appear after the 'if' statement with regards the 'write' block to make sure the timel is saved correctly per timestep. Cheers Azad ________________________________ Hi Xianbei, You are correct that dtime should be equal to DT. If you look at avg_all() in navier5.f in the main nek source directory, this is what happens because timel is updated after the averaging. In the turbchannel case, this was not done - so I've now modified the .usr file to reflect this. I would suggest to simply use the avg_all code to do the time averaging and then to use those average fields to generate profiles. Thanks for pointing out the problem with the turbChannel example. Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Saturday, May 31, 2014 10:38 PM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] test of the time average of turbChannel--what's wrong? Hi Xianbei, The usr files are meant to be modified by the users, so you can adjust it to suit your needs. Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Saturday, May 31, 2014 9:58 PM To: Nek5000 Subject: [Nek5000-users] test of the time average of turbChannel--what's wrong? Hi, all: I read about the time average method in the turbChannel.usr/userchk,here is the origin codes: if(icalld.eq.0) then call rzero(uavg,n) call rzero(urms,n) call rzero(vrms,n) call rzero(wrms,n) call rzero(uvms,n) atime = 0. timel = time call planar_average_s(yy ,ym1 ,w1,w2) icalld = 1 endif dtime = time - timel atime = atime + dtime if (atime.ne.0. .and. dtime.ne.0.) then beta = dtime/atime alpha = 1.-beta ifverbose = .false. call avg1(uavg,vx ,alpha,beta,n,'uavg',ifverbose) As seen , atime and timel is initialized by 0 and time, so when time=time+DT, dtime=DT, atime=DT, so the first average value is vx(t=DT), when time=time+2*DT, dtime=2*DT(timel is not changed, just equal to the initial value ),atime=3*DT, here question comes: this will lead to vxmean(t=2*DT)=2/3*vx(t=DT)+1/3*vx(t=2*DT), this is not what we respect. The right one is make sure that dtime=DT all the time. Also, I do a test to verify this.In order to be more reliable, the velocity isn't nomorlized by u_tau. First, calculate by 1 step and output the means.dat, so the value equal to the time=DT's #time = 2.0000000E-02 # y uup_tau Umean 0.000000000E+00 2.031155153E-02 0.000000000E+00 2.565198406E-03 2.031155153E-02 1.285886819E-02 then restart with the field from previous calculation and output the means.dat, this will output the value of time=2*DT's, #time = 4.0000000E-02 # y uup_tau Umean 0.000000000E+00 2.072569248E-02 0.000000000E+00 2.565205097E-03 2.072569248E-02 1.288671376E-02 At last, restart the calculation and run 2 steps to calculate the average of vx(time=DT) and vx(time=2*DT) #time = 4.0000000E-02 # y uup_tau Umean 0.000000000E+00 2.061649552E-02 0.000000000E+00 2.565198406E-03 2.061649552E-02 1.287524390E-02 As can be seen, the 2 step average is almost equal to the average of step 1 and step 2. So what's wrong with my understanding? Is timel alway updated to the previous time and make sure that dtime=constant? How? Can anyone help? Xianbei _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Mon Jun 23 09:35:22 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 23 Jun 2014 16:35:22 +0200 Subject: [Nek5000-users] test of the time average of turbChannel--what's wrong? Message-ID: I think at the end of 'userchk' the 'timel = time' just needed to come after the 'endif' rather than before. Otherwise things seems to be fine, I guess. Thanks Azad ________________________________________ Thanks Azad -- so is it currently messed up? Or was it messed up before? (i.e., do I need to undo my recent change?) Thanks! Paul ________________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Monday, June 23, 2014 8:20 AM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] test of the time average of turbChannel--what's wrong? Hi Paul, I just wanted to come back to this point as it seems the correction regarding the turbchannel case in the new version of nek is quite sound; though, the command "timel = time" seems to sit in a wrong position. To what I understand it must appear after the 'if' statement with regards the 'write' block to make sure the timel is saved correctly per timestep. Cheers Azad ________________________________ Hi Xianbei, You are correct that dtime should be equal to DT. If you look at avg_all() in navier5.f in the main nek source directory, this is what happens because timel is updated after the averaging. In the turbchannel case, this was not done - so I've now modified the .usr file to reflect this. I would suggest to simply use the avg_all code to do the time averaging and then to use those average fields to generate profiles. Thanks for pointing out the problem with the turbChannel example. Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Saturday, May 31, 2014 10:38 PM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] test of the time average of turbChannel--what's wrong? Hi Xianbei, The usr files are meant to be modified by the users, so you can adjust it to suit your needs. Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Saturday, May 31, 2014 9:58 PM To: Nek5000 Subject: [Nek5000-users] test of the time average of turbChannel--what's wrong? Hi, all: I read about the time average method in the turbChannel.usr/userchk,here is the origin codes: if(icalld.eq.0) then call rzero(uavg,n) call rzero(urms,n) call rzero(vrms,n) call rzero(wrms,n) call rzero(uvms,n) atime = 0. timel = time call planar_average_s(yy ,ym1 ,w1,w2) icalld = 1 endif dtime = time - timel atime = atime + dtime if (atime.ne.0. .and. dtime.ne.0.) then beta = dtime/atime alpha = 1.-beta ifverbose = .false. call avg1(uavg,vx ,alpha,beta,n,'uavg',ifverbose) As seen , atime and timel is initialized by 0 and time, so when time=time+DT, dtime=DT, atime=DT, so the first average value is vx(t=DT), when time=time+2*DT, dtime=2*DT(timel is not changed, just equal to the initial value ),atime=3*DT, here question comes: this will lead to vxmean(t=2*DT)=2/3*vx(t=DT)+1/3*vx(t=2*DT), this is not what we respect. The right one is make sure that dtime=DT all the time. Also, I do a test to verify this.In order to be more reliable, the velocity isn't nomorlized by u_tau. First, calculate by 1 step and output the means.dat, so the value equal to the time=DT's #time = 2.0000000E-02 # y uup_tau Umean 0.000000000E+00 2.031155153E-02 0.000000000E+00 2.565198406E-03 2.031155153E-02 1.285886819E-02 then restart with the field from previous calculation and output the means.dat, this will output the value of time=2*DT's, #time = 4.0000000E-02 # y uup_tau Umean 0.000000000E+00 2.072569248E-02 0.000000000E+00 2.565205097E-03 2.072569248E-02 1.288671376E-02 At last, restart the calculation and run 2 steps to calculate the average of vx(time=DT) and vx(time=2*DT) #time = 4.0000000E-02 # y uup_tau Umean 0.000000000E+00 2.061649552E-02 0.000000000E+00 2.565198406E-03 2.061649552E-02 1.287524390E-02 As can be seen, the 2 step average is almost equal to the average of step 1 and step 2. So what's wrong with my understanding? Is timel alway updated to the previous time and make sure that dtime=constant? How? Can anyone help? Xianbei From nek5000-users at lists.mcs.anl.gov Tue Jun 24 07:21:59 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 24 Jun 2014 14:21:59 +0200 Subject: [Nek5000-users] perturbation mode question Message-ID: Hi Neks, I'm trying to solve the linearized Navier Stokes equations. Following different posts, I've seen that it maight be possible if I activate the perturbation mode. What I'm doing is the following: 1) I set param 31 to -1.00000 p031 NPERT: #perturbation modes 2) I have introduced the base flow in the presolve/restart options in the following way: 1 PRESOLVE/RESTART OPTIONS ***** BASE0.f00011 Should it be enough to solve this problem? I don't know how to introduce the perturbation in the equations and how to set in Nek5000 the file BASE0.f00011 as base flow. Thanks SL From nek5000-users at lists.mcs.anl.gov Wed Jun 25 07:57:48 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 25 Jun 2014 14:57:48 +0200 Subject: [Nek5000-users] why history file has weird output? In-Reply-To: References: Message-ID: Hi Neks, I want to out the U V and P values from one elemet, but it out put same time step line repeatly with all values are zero. like this 91 1.03171068E-02 1.67794142E+00 1.18830199E-01 -7.60391611E-01 92 1.03171068E-02 0.00000000E+00 0.00000000E+00 0.00000000E+00 93 1.05331012E-02 1.67757255E+00 1.18681458E-01 -7.62501274E-01 94 1.05331012E-02 0.00000000E+00 0.00000000E+00 0.00000000E+00 95 1.07490956E-02 1.67714286E+00 1.18533770E-01 -7.64569516E-01 96 1.07490956E-02 0.00000000E+00 0.00000000E+00 0.00000000E+00 so what is the problem? Anyone has met this before_? thanks Wei From nek5000-users at lists.mcs.anl.gov Wed Jun 25 14:30:44 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 25 Jun 2014 15:30:44 -0400 Subject: [Nek5000-users] Output problem Message-ID: Hi, Neks I want to frequently output my data. Every run will generate over 10000 files. However the maximum value for fld file is fld9999. Is there any way to solve this problem? Thank you. Mu Xu -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Jun 25 15:33:16 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 25 Jun 2014 20:33:16 +0000 Subject: [Nek5000-users] Output problem In-Reply-To: References: Message-ID: Hi Mu, Switch to the f00000 file format. You can do this by changing param(66) and (67) to be 6 in the .usr file. Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Wednesday, June 25, 2014 2:30 PM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] Output problem Hi, Neks I want to frequently output my data. Every run will generate over 10000 files. However the maximum value for fld file is fld9999. Is there any way to solve this problem? Thank you. Mu Xu -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Jun 26 09:05:22 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 26 Jun 2014 10:05:22 -0400 Subject: [Nek5000-users] Separation Problem -2D In-Reply-To: References: Message-ID: Hi, I want to solve the Navier-Stokes problem in 2D with Nek5000. Which is the best way to prepare the mesh? Do you suggest a software or code? Moreover, how should I solve it with Nek5000? Is there any open source code for that? Thank, Arash From nek5000-users at lists.mcs.anl.gov Thu Jun 26 10:10:06 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 26 Jun 2014 19:10:06 +0400 Subject: [Nek5000-users] Small diffusivity. How heat/diffusion equations are solved? Message-ID: I am trying to model inner waves in a salinity-stratified solution, for which kinematic viscosity is 10^-6, diffusivity is 10^-9, so Schmidt number is about 10^-3. If I set viscosity=diffusivity=10^-6, the program works fine, but I get too great effect of diffusion. If I set diffusivity to be less than 10^-6, solution blows up. In this connection I have two questions: Is there a description how heat/diffusion equations are solved in nek5000? Is it possible to change transport/diffusion equation just to transport equation, i.e. without diffusion at all? Thanks. From nek5000-users at lists.mcs.anl.gov Fri Jun 27 03:45:44 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 27 Jun 2014 12:45:44 +0400 Subject: [Nek5000-users] Small diffusivity. How heat/diffusion equations aresolved? In-Reply-To: References: Message-ID: I have fixed the parameters and now it works fine for Sm=1000. Still it is interesting where it is better to read about nek solution of diffusion equations. Thanks > 6/26/2014 7:10:13 PM ???????????? (nek5000-users at lists.mcs.anl.gov) ???????: > > > I am trying to model inner waves in a salinity-stratified solution, > for which kinematic viscosity is 10^-6, diffusivity is 10^-9, so Schmidt number is about 10^-3. > If I set viscosity=diffusivity=10^-6, the program works fine, but I get too great effect of diffusion. > If I set diffusivity to be less than 10^-6, solution blows up. > > In this connection I have two questions: > > Is there a description how heat/diffusion equations are solved in nek5000? > > Is it possible to change transport/diffusion equation just to transport equation, i.e. without diffusion at all? > > Thanks. > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > From nek5000-users at lists.mcs.anl.gov Fri Jun 27 10:28:19 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 27 Jun 2014 17:28:19 +0200 Subject: [Nek5000-users] SFD error message from p66 Message-ID: Dear Nek's, I'm trying to program a Selective Frequency Damping following the article of Akervik et. al (Physics of Fluids, 2006) and some Nek5000 posts. I'm able to compile the code, however, when I try to run my simulation, I find the following error message: 0 0.0000E+00 Write checkpoint: 0 0.0000E+00 OPEN: At line 335 of file User/nek5_svn/trunk/nek/prepost.f (unit = 24, file = '') Fortran runtime error: File '' does not exist It seems to be something related to param 66. I've tried with p66=6, 0, 1, -1, but I always get the same error. Do you know what happens? Thanks SL From nek5000-users at lists.mcs.anl.gov Sun Jun 29 04:16:02 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 29 Jun 2014 13:16:02 +0400 Subject: [Nek5000-users] running NEK5000 on a cluster with fast/slow storage subsystems. Relative paths instead of absolute Message-ID: I am trying to use nek5000 on the cluster Lomonosov. What is special in the configuration is that it has two levels of storage. The basic storage of a user (i.e. his home directory) is not seen by computational nodes. Computational nodes have their own file system which can be accessed by user through "~/_scratch" subdirectory of the user's home directory. So "~/_scratch" is the home directory for programs running on computational nodes. This is why I can't run nek5000 on this very cluster. I have the following message in the log file: ... read .rea file forrtl: No such file or directory forrtl: severe (29): file not found, unit 9, file /mnt/data/users/dm4/vol12/vanvan/_scratch/stw/stw32x32.rea ... You can see that the program tries to look for an absolute path of the file: it expanded home directory to "/mnt/data/users/dm4/vol12/vanvan" and tries to find the file in the "_scratch" subdirectory which does not exist on computational nodes. For the program on computational nodes the path is simply "~/stw/stw32x32.rea" or "/home/users/vanvan/stw/stw32x32.rea" Can you tell me what I have to change for a relative path instead of absolute or give the absolute path manually. Suppose this situation can happen on other clusters. Thank you, Van From nek5000-users at lists.mcs.anl.gov Sun Jun 29 09:02:10 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 29 Jun 2014 14:02:10 +0000 Subject: [Nek5000-users] running NEK5000 on a cluster with fast/slow storage subsystems. Relative paths instead of absolute In-Reply-To: References: Message-ID: Van, It looks to me like you should move your files to ...vanvan/_scratch/stw and launch your job from there. I'm assuming you're using some type of script to launch the job, like one of those provided in trunk/tools/scripts. If you need, you can have the script copy SESSION.NAME to your top directory, if that's where the compute node is looking for it. In any case, a slight modification to the launch script is exactly what is needed. SESSION.NAME, which is created by the launch script (e.g., nekbmpi blah 4, would create a SESSION.NAME file), has the session name on the first line and the path where files are to be found on the second. Just modify your own nekbmpi script to have it reflect where the compute node is to find the files. Note that you'll all have to ensure that SESSION.NAME is in a directory where the compute node can read it. Paul ________________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Sunday, June 29, 2014 4:16 AM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] running NEK5000 on a cluster with fast/slow storage subsystems. Relative paths instead of absolute I am trying to use nek5000 on the cluster Lomonosov. What is special in the configuration is that it has two levels of storage. The basic storage of a user (i.e. his home directory) is not seen by computational nodes. Computational nodes have their own file system which can be accessed by user through "~/_scratch" subdirectory of the user's home directory. So "~/_scratch" is the home directory for programs running on computational nodes. This is why I can't run nek5000 on this very cluster. I have the following message in the log file: ... read .rea file forrtl: No such file or directory forrtl: severe (29): file not found, unit 9, file /mnt/data/users/dm4/vol12/vanvan/_scratch/stw/stw32x32.rea ... You can see that the program tries to look for an absolute path of the file: it expanded home directory to "/mnt/data/users/dm4/vol12/vanvan" and tries to find the file in the "_scratch" subdirectory which does not exist on computational nodes. For the program on computational nodes the path is simply "~/stw/stw32x32.rea" or "/home/users/vanvan/stw/stw32x32.rea" Can you tell me what I have to change for a relative path instead of absolute or give the absolute path manually. Suppose this situation can happen on other clusters. Thank you, Van _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Mon Jun 30 02:51:20 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 30 Jun 2014 09:51:20 +0200 Subject: [Nek5000-users] SFD error message from p66 In-Reply-To: References: Message-ID: Hi SL We have implemented SFD some time ago and we can share the code if you wish. It is probably good to have single tested version of the code than develop number of variations. We've already shared the code with Elia. Regards Adam On 27/06/14 17:28, nek5000-users at lists.mcs.anl.gov wrote: > Dear Nek's, > > I'm trying to program a Selective Frequency Damping following the > article of Akervik et. al (Physics of Fluids, 2006) and some Nek5000 > posts. > > I'm able to compile the code, however, when I try to run my > simulation, I find the following error message: > > 0 0.0000E+00 Write checkpoint: > > 0 0.0000E+00 OPEN: > At line 335 of file User/nek5_svn/trunk/nek/prepost.f (unit = 24, file > = '') > Fortran runtime error: File '' does not exist > > It seems to be something related to param 66. I've tried with p66=6, > 0, 1, -1, but I always get the same error. > > Do you know what happens? > > Thanks > SL > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Mon Jun 30 11:29:03 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 30 Jun 2014 12:29:03 -0400 Subject: [Nek5000-users] non-physical temp. at walls Message-ID: Hello all, I wondered if anyone have ever experienced high/low nonphysical temperature field for a configuration in which there is a volumetric heat source. I have such hot/cold spots very close to a few insulated walls as boundary conditions in my configuration. In fact, such temperatures have been observed in the elements adjacent to the wall. The heat source is uniform for part of the domain and zero for the rest of it. It might be due to non-monotonicity of advection scheme and insufficient resolution. The minimum temperature can be clipped, but there is no way to limit the maximum temperature. Any help would be appreciated. Thanks, Mohsen