From nek5000-users at lists.mcs.anl.gov Wed Apr 2 04:26:58 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 2 Apr 2014 09:26:58 +0000 Subject: [Nek5000-users] Unstructured Mesh Message-ID: Hi Paul, Yes the meshes now work and Nek clearly shows it is reversing element ordering. Thank you for your help! Best regards, JP -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Apr 2 12:33:16 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 2 Apr 2014 19:33:16 +0200 Subject: [Nek5000-users] Problem with passive scalar fields - subroutine outfld Message-ID: Dear Paul, Thanks for your answer. I already had flags as following: T T T T T T T T T T T T IFNAV & IFADVC (convection in P.S. fields) F F T T T T T T T T T T IFTMSH (IF mesh for this field is T mesh) because all passive scalar fields are temperature fields in my case. Is it correct? (By the way, why 2 flags for field 1, velocity, in the IFTMSH line? It seems to be that the first one doesn't matter, i.e. I don't see differences in results using "T F T T ..." instead of "F F T T ..."). Performing some tests (also setting p93=p94=p95=0. in .rea in some cases), I noted that if subroutine outfld is called during the simulation, then PS fields change as described in my previous mail. Indeed, if in .rea file is p15>p11 (i.e. outfld called at last step only) then PS fields are correct. And PS fields are correct also if vx,vy,vz,pr,t are dumped with outpost2 during the simulation while outfld is not called. This is the reason why I thought that the problem is subroutine outfld instead of outpost2. And I confirm that only some of the PS fields are changed: running two different simulations that differ only for the number of PS fields, a same field may be correct in one simulation and not in the other. My only solution, for now, is to run the simulation with p15>p11 in .rea, saving variables directly with outpost2. Is it a problem to restart a case with a field file obtained with outpost2(vx,vy,vz,pr,t,ldimt,'res') instead of outfld? Field files obtained seem to have different size, but results for restart seem to be the same. Best reagards, Donato -----Original Message----- Date: Mon, 31 Mar 2014 04:16:30 +0000 From: nek5000-users at lists.mcs.anl.gov To: "nek5000-users at lists.mcs.anl.gov" Dear Donato, I've not looked closely at this yet. However, I suspect it might be related to the projection. Can you run your example with param 94 = 0 in the .rea file ? This should turn off the velocity/passive scalar projection. Another question --- in your .rea file, where it says "IFADVC" there should be two lines like: T F F F F F F F F F F IFNAV & IFADVC (convection in P.S. fields) F F T T T T T T T T T T IFTMSH (IF mesh for this field is T mesh) For your cases, you probably want them: T T T T T T T T T T T T IFNAV & IFADVC (convection in P.S. fields) F F T F F F F F F F F F F IFTMSH (IF mesh for this field is T mesh) This would do the following: 1) It turns on advection for all fields (fluid, temperature, and passive scalars) 2) It sets the mesh field to be Fluid It sets the velocity field to be Fluid It sets the temperature to be Temperature (i.e., fluid + solid) It sets the remaining passive scalars to be Fluid For conjugate heat transfer, normally only the temperature acts over both the fluid and solid element set, which is why I set those flags as above. Let me know if this resolves the issue for you... Regards, Paul From nek5000-users at lists.mcs.anl.gov Wed Apr 2 12:28:34 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 2 Apr 2014 19:28:34 +0200 Subject: [Nek5000-users] to Michael--> Nek5000 & Gambit, blocked file Message-ID: does anyone found that the periodic boundary conditions can not be read by genmap? regards Wei From nek5000-users at lists.mcs.anl.gov Wed Apr 2 13:27:35 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 2 Apr 2014 18:27:35 +0000 Subject: [Nek5000-users] Problem with passive scalar fields - subroutine outfld In-Reply-To: References: Message-ID: Dear Donato, Thank you for bringing to my attention the issue with outpost/outpost2. It is almost certain that you want to use outpost2 - that was designed by one of our developers for exactly the scenario you describe where you have many passive scalars. (Though I don't think it was tested also with conjugate heat transfer.) Regarding the two flags in the IFTMSH line, the first one is actually for the "mesh" which is field 0, i.e., in moving boundary problems the moving part of the mesh could be either just fluid or fluid and solid. Thus, the flags are technically addressed to fields 1 2 3 4 ... for IFNAV/IFADVC and 0 1 2 3 ... for IFTMSH So, would things be functioning correctly for you if you use only outpost2() ? There should be no issue in restarting from fields generated by this process. 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, April 02, 2014 12:33 PM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] Problem with passive scalar fields - subroutine outfld Dear Paul, Thanks for your answer. I already had flags as following: T T T T T T T T T T T T IFNAV & IFADVC (convection in P.S. fields) F F T T T T T T T T T T IFTMSH (IF mesh for this field is T mesh) because all passive scalar fields are temperature fields in my case. Is it correct? (By the way, why 2 flags for field 1, velocity, in the IFTMSH line? It seems to be that the first one doesn't matter, i.e. I don't see differences in results using "T F T T ..." instead of "F F T T ..."). Performing some tests (also setting p93=p94=p95=0. in .rea in some cases), I noted that if subroutine outfld is called during the simulation, then PS fields change as described in my previous mail. Indeed, if in .rea file is p15>p11 (i.e. outfld called at last step only) then PS fields are correct. And PS fields are correct also if vx,vy,vz,pr,t are dumped with outpost2 during the simulation while outfld is not called. This is the reason why I thought that the problem is subroutine outfld instead of outpost2. And I confirm that only some of the PS fields are changed: running two different simulations that differ only for the number of PS fields, a same field may be correct in one simulation and not in the other. My only solution, for now, is to run the simulation with p15>p11 in .rea, saving variables directly with outpost2. Is it a problem to restart a case with a field file obtained with outpost2(vx,vy,vz,pr,t,ldimt,'res') instead of outfld? Field files obtained seem to have different size, but results for restart seem to be the same. Best reagards, Donato -----Original Message----- Date: Mon, 31 Mar 2014 04:16:30 +0000 From: nek5000-users at lists.mcs.anl.gov To: "nek5000-users at lists.mcs.anl.gov" Dear Donato, I've not looked closely at this yet. However, I suspect it might be related to the projection. Can you run your example with param 94 = 0 in the .rea file ? This should turn off the velocity/passive scalar projection. Another question --- in your .rea file, where it says "IFADVC" there should be two lines like: T F F F F F F F F F F IFNAV & IFADVC (convection in P.S. fields) F F T T T T T T T T T T IFTMSH (IF mesh for this field is T mesh) For your cases, you probably want them: T T T T T T T T T T T T IFNAV & IFADVC (convection in P.S. fields) F F T F F F F F F F F F F IFTMSH (IF mesh for this field is T mesh) This would do the following: 1) It turns on advection for all fields (fluid, temperature, and passive scalars) 2) It sets the mesh field to be Fluid It sets the velocity field to be Fluid It sets the temperature to be Temperature (i.e., fluid + solid) It sets the remaining passive scalars to be Fluid For conjugate heat transfer, normally only the temperature acts over both the fluid and solid element set, which is why I set those flags as above. Let me know if this resolves the issue for you... Regards, 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 Thu Apr 3 03:50:51 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 3 Apr 2014 10:50:51 +0200 Subject: [Nek5000-users] Problem with passive scalar fields - subroutine outfld Message-ID: Dear Paul, Yes, all ok saving fields with outpost2, i.e. setting p15>p11 in .rea file. Regarding restart, I obtained same results using both field file from outpost2 and (the only one) field file from outfld written on last step (step p11). So outfld seems to don't modify fields when it's called only on last step. Thanks. Regards, Donato From nek5000-users at lists.mcs.anl.gov Wed Apr 2 04:46:17 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 02 Apr 2014 11:46:17 +0200 Subject: [Nek5000-users] Velocity at the center line Message-ID: Hello Neks I would like to plot the value of axial-velocity at the center line of a pipe flow. At present am using Visit to do that, But I would like to know If it is possible to get it directly from Nek. I tried to loop on the elements to get the value ---------------------------------------------------------------------------------------------- n = lx1*ly1*lz1*lelt do i=1,n x = xm1(i,1,1,1) y = ym1(i,1,1,1) z = zm1(i,1,1,1) if (x.eq.0 .AND. y.eq.0 .AND. z.gt.0 .AND. z.lt.25) then l = z up = vz(i,1,1,1) write(13,*) z,up endif enddo ----------------------------------------------------------------------------------------------- but it doesn't seem to work. Could some tell me what is the correct variable to loop on to get the values. Thank you, Kamal. From nek5000-users at lists.mcs.anl.gov Thu Apr 3 07:01:10 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 3 Apr 2014 07:01:10 -0500 Subject: [Nek5000-users] Velocity at the center line In-Reply-To: References: Message-ID: Hi Kamal, This doesn't work as you expect because it is very unlikely that you have node points that fall exactly at x = 0 and y = 0. The best way to go about this is to use the hpts() routine. Instructions can be found at http://nek5000.mcs.anl.gov/index.php/Data_processing_example This will interpolate your solution to the points given in your "hpts.in" file. Hope this helps! Josh On Wed, Apr 2, 2014 at 4:46 AM, wrote: > Hello Neks > > I would like to plot the value of axial-velocity at the center line of a > pipe flow. At present am using Visit to do that, But I would like to know > If it is possible to get it directly from Nek. > > > I tried to loop on the elements to get the value > ------------------------------------------------------------ > ---------------------------------- > n = lx1*ly1*lz1*lelt > do i=1,n > > x = xm1(i,1,1,1) > y = ym1(i,1,1,1) > z = zm1(i,1,1,1) > > > > if (x.eq.0 .AND. y.eq.0 .AND. z.gt.0 .AND. z.lt.25) then > l = z > up = vz(i,1,1,1) > write(13,*) z,up > endif > > enddo > > ------------------------------------------------------------ > ----------------------------------- > > > but it doesn't seem to work. Could some tell me what is the correct > variable to loop on to get the values. > > Thank you, > > Kamal. > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > -- Josh Camp "All that is necessary for the triumph of evil is that good men do nothing" -- Edmund Burke -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Fri Apr 4 07:09:52 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 4 Apr 2014 12:09:52 +0000 Subject: [Nek5000-users] multiple runs and poisson for velocity Message-ID: Dear Neks, I have two issues that I would like to discuss with you. Firstly, I would like to perform many steady state simulations with different values of the viscosity, each time using the previous solution as starting condition. For this reason, I have built the following subroutine: c----------------------------------------------------------------------- subroutine userchk include 'SIZE' include 'TOTAL' do 120 ire=1,10 param(2) = -1*ire call setprop igeom=1 call fluid(igeom) 120 continue ifxyo = .true. call outpost(vx,vy,vz,pr,t,'ste') call exitt return end c----------------------------------------------------------------------- but this does not work as I expected, could somebody suggest me what I should do instead? Secondly, I would like to solve (in postprocessing mode) a Poisson problem for the velocity components, in the form -lapl(vx) = fx and -lapl(vy)=fy, with fx and fy known. Is it possible to do this within NEK? I think this could be done by adapting the Uzawa pressure solver in navier1.f, but I am not sure if this could work. Best regards, Giuseppe From nek5000-users at lists.mcs.anl.gov Fri Apr 4 12:40:07 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 4 Apr 2014 17:40:07 +0000 Subject: [Nek5000-users] multiple runs and poisson for velocity In-Reply-To: References: Message-ID: Hi Giuseppe, Regarding the first question, you need to change not the param(2) but copy the value of dynamic viscosity (which 1/Re for non-dimentional case with rho=1) into an array VDIFF (1,1,1,1,1) as in vprops() of subs1.f ... DO 1000 IEL=1,NEL ... ELSE IF(MATYPE(IGRP,IFIELD).EQ.0)THEN C C Default constant property C CDIFF = CPFLD(IFIELD,1) ... CALL CFILL(VDIFF (1,1,1,IEL,IFIELD),CDIFF,NXYZ1) where cpfld(1,1) array is filled in rdparam() of connect2.f during the ininitialization: CPFLD(1,1)=PARAM(2) 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: Friday, April 04, 2014 7:09 AM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] multiple runs and poisson for velocity Dear Neks, I have two issues that I would like to discuss with you. Firstly, I would like to perform many steady state simulations with different values of the viscosity, each time using the previous solution as starting condition. For this reason, I have built the following subroutine: c----------------------------------------------------------------------- subroutine userchk include 'SIZE' include 'TOTAL' do 120 ire=1,10 param(2) = -1*ire call setprop igeom=1 call fluid(igeom) 120 continue ifxyo = .true. call outpost(vx,vy,vz,pr,t,'ste') call exitt return end c----------------------------------------------------------------------- but this does not work as I expected, could somebody suggest me what I should do instead? Secondly, I would like to solve (in postprocessing mode) a Poisson problem for the velocity components, in the form -lapl(vx) = fx and -lapl(vy)=fy, with fx and fy known. Is it possible to do this within NEK? I think this could be done by adapting the Uzawa pressure solver in navier1.f, but I am not sure if this could work. Best regards, Giuseppe _______________________________________________ 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 Apr 4 13:01:37 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 4 Apr 2014 18:01:37 +0000 Subject: [Nek5000-users] multiple runs and poisson for velocity In-Reply-To: References: Message-ID: Hi Giuseppe, If you look at the .usr file in examples/eddy_psi_omega/ you'll see a call for a Poisson solve for a little psi-omega formulation of Navier-Stokes. Please let me know if this provides the insight you seek for setting up your Poisson solves. Best regards, 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, April 04, 2014 7:09 AM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] multiple runs and poisson for velocity Dear Neks, I have two issues that I would like to discuss with you. Firstly, I would like to perform many steady state simulations with different values of the viscosity, each time using the previous solution as starting condition. For this reason, I have built the following subroutine: c----------------------------------------------------------------------- subroutine userchk include 'SIZE' include 'TOTAL' do 120 ire=1,10 param(2) = -1*ire call setprop igeom=1 call fluid(igeom) 120 continue ifxyo = .true. call outpost(vx,vy,vz,pr,t,'ste') call exitt return end c----------------------------------------------------------------------- but this does not work as I expected, could somebody suggest me what I should do instead? Secondly, I would like to solve (in postprocessing mode) a Poisson problem for the velocity components, in the form -lapl(vx) = fx and -lapl(vy)=fy, with fx and fy known. Is it possible to do this within NEK? I think this could be done by adapting the Uzawa pressure solver in navier1.f, but I am not sure if this could work. Best regards, Giuseppe _______________________________________________ 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 Apr 5 08:36:04 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sat, 5 Apr 2014 13:36:04 +0000 Subject: [Nek5000-users] multiple runs and poisson for velocity In-Reply-To: References: Message-ID: Hi Paul, thank you for referring me to the psi-omega example. This was indeed useful, if I have understood correctly the way it works. If I am right, to solve a Poisson problem for a variable psi for instance, the steps are the following: 1) write the desired values to the rhs vector 2) call rone(h1,n) ! this sets to one the coefficient multiplying the stiffness matrix 3) call rzero(h2,n) ! this sets to zero the coefficient multiplying the mass matrix 4) call hmholtz('psi ',psi,rhs,h1,h2,tmask,tmult,imsh,tol,maxiter,isd) ! call the poisson solver for the psi vector, imsh specifies which mesh is used, tol is the tolerance for the CG, maxiter the maximum number of iterations, isd should be set to two for axisymmetric problems. If i am right tmult is the vector with the quadrature weights for the temperature mesh, should I replace tmult with vmult is psi is defined on the velocity mesh? tmask if I am right is related to the Dirichlet b.c. on the temperature mesh, should I replace this with v1mask if I work on velocity components? 5) then I should be done, the example continues computing the gradient of psi to get the velocity components from the velocity potential, but I don't need this. Thanks also to Aleks for his help with the first part of my question, I will write again if I have other questions. Best regards, Giuseppe Il giorno 04/apr/2014, alle ore 20:01, ha scritto: > > Hi Giuseppe, > > If you look at the .usr file in examples/eddy_psi_omega/ > you'll see a call for a Poisson solve for a little psi-omega formulation > of Navier-Stokes. > > Please let me know if this provides the insight you seek for setting > up your Poisson solves. > > Best regards, > > 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, April 04, 2014 7:09 AM > To: nek5000-users at lists.mcs.anl.gov > Subject: [Nek5000-users] multiple runs and poisson for velocity > > Dear Neks, > I have two issues that I would like to discuss with you. > Firstly, I would like to perform many steady state simulations with different values of the viscosity, each time using the previous solution as starting condition. > For this reason, I have built the following subroutine: > > c----------------------------------------------------------------------- > subroutine userchk > include 'SIZE' > include 'TOTAL' > > > do 120 ire=1,10 > param(2) = -1*ire > call setprop > igeom=1 > call fluid(igeom) > 120 continue > > ifxyo = .true. > call outpost(vx,vy,vz,pr,t,'ste') > call exitt > > return > end > c----------------------------------------------------------------------- > > but this does not work as I expected, could somebody suggest me what I should do instead? > > Secondly, I would like to solve (in postprocessing mode) a Poisson problem for the velocity components, in the form -lapl(vx) = fx and -lapl(vy)=fy, with fx and fy known. > Is it possible to do this within NEK? I think this could be done by adapting the Uzawa pressure solver in navier1.f, but I am not sure if this could work. > Best regards, > Giuseppe > _______________________________________________ > 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 Apr 5 13:34:50 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sat, 5 Apr 2014 18:34:50 +0000 Subject: [Nek5000-users] multiple runs and poisson for velocity In-Reply-To: References: , Message-ID: Hi Giuseppe, Your understanding is essentially correct. One minor point is that the rhs should be rhs = B*f i.e., as given by: call col3(rhs,bm1,f,n) or (more typically) call col2(rhs,bm1,n) where rhs() would be filled with the desired rhs. The idea here is that the rhs should be multiplied by the mass matrix --- that is, when nek solves the Poisson equation it is expressed as: A u = B f for -del^2 u = f(x,y), say. I hope this helps. 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, April 05, 2014 8:36 AM To: Subject: Re: [Nek5000-users] multiple runs and poisson for velocity Hi Paul, thank you for referring me to the psi-omega example. This was indeed useful, if I have understood correctly the way it works. If I am right, to solve a Poisson problem for a variable psi for instance, the steps are the following: 1) write the desired values to the rhs vector 2) call rone(h1,n) ! this sets to one the coefficient multiplying the stiffness matrix 3) call rzero(h2,n) ! this sets to zero the coefficient multiplying the mass matrix 4) call hmholtz('psi ',psi,rhs,h1,h2,tmask,tmult,imsh,tol,maxiter,isd) ! call the poisson solver for the psi vector, imsh specifies which mesh is used, tol is the tolerance for the CG, maxiter the maximum number of iterations, isd should be set to two for axisymmetric problems. If i am right tmult is the vector with the quadrature weights for the temperature mesh, should I replace tmult with vmult is psi is defined on the velocity mesh? tmask if I am right is related to the Dirichlet b.c. on the temperature mesh, should I replace this with v1mask if I work on velocity components? 5) then I should be done, the example continues computing the gradient of psi to get the velocity components from the velocity potential, but I don't need this. Thanks also to Aleks for his help with the first part of my question, I will write again if I have other questions. Best regards, Giuseppe Il giorno 04/apr/2014, alle ore 20:01, ha scritto: > > Hi Giuseppe, > > If you look at the .usr file in examples/eddy_psi_omega/ > you'll see a call for a Poisson solve for a little psi-omega formulation > of Navier-Stokes. > > Please let me know if this provides the insight you seek for setting > up your Poisson solves. > > Best regards, > > 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, April 04, 2014 7:09 AM > To: nek5000-users at lists.mcs.anl.gov > Subject: [Nek5000-users] multiple runs and poisson for velocity > > Dear Neks, > I have two issues that I would like to discuss with you. > Firstly, I would like to perform many steady state simulations with different values of the viscosity, each time using the previous solution as starting condition. > For this reason, I have built the following subroutine: > > c----------------------------------------------------------------------- > subroutine userchk > include 'SIZE' > include 'TOTAL' > > > do 120 ire=1,10 > param(2) = -1*ire > call setprop > igeom=1 > call fluid(igeom) > 120 continue > > ifxyo = .true. > call outpost(vx,vy,vz,pr,t,'ste') > call exitt > > return > end > c----------------------------------------------------------------------- > > but this does not work as I expected, could somebody suggest me what I should do instead? > > Secondly, I would like to solve (in postprocessing mode) a Poisson problem for the velocity components, in the form -lapl(vx) = fx and -lapl(vy)=fy, with fx and fy known. > Is it possible to do this within NEK? I think this could be done by adapting the Uzawa pressure solver in navier1.f, but I am not sure if this could work. > Best regards, > Giuseppe > _______________________________________________ > 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 Apr 7 01:54:28 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 7 Apr 2014 06:54:28 +0000 Subject: [Nek5000-users] multiple runs and poisson for velocity In-Reply-To: References: , Message-ID: Thank you Paul, I managed to obtain the Poisson solver I needed. Best, Giuseppe Il giorno 05/apr/2014, alle ore 20:34, ha scritto: > > Hi Giuseppe, > > Your understanding is essentially correct. One minor point is that the rhs should be > > > rhs = B*f > > i.e., as given by: > > call col3(rhs,bm1,f,n) > > or (more typically) > > call col2(rhs,bm1,n) > > where rhs() would be filled with the desired rhs. The idea here is that the rhs should > be multiplied by the mass matrix --- that is, when nek solves the Poisson equation it > is expressed as: > > > A u = B f > > for -del^2 u = f(x,y), say. > > I hope this helps. > > 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, April 05, 2014 8:36 AM > To: > Subject: Re: [Nek5000-users] multiple runs and poisson for velocity > > Hi Paul, > thank you for referring me to the psi-omega example. This was indeed useful, if I have understood correctly the way it works. > If I am right, to solve a Poisson problem for a variable psi for instance, the steps are the following: > > 1) write the desired values to the rhs vector > 2) call rone(h1,n) ! this sets to one the coefficient multiplying the stiffness matrix > 3) call rzero(h2,n) ! this sets to zero the coefficient multiplying the mass matrix > 4) call hmholtz('psi ',psi,rhs,h1,h2,tmask,tmult,imsh,tol,maxiter,isd) ! call the poisson solver for the psi vector, imsh specifies which mesh is used, tol is the tolerance for the CG, maxiter the maximum number of iterations, isd should be set to two for axisymmetric problems. If i am right tmult is the vector with the quadrature weights for the temperature mesh, should I replace tmult with vmult is psi is defined on the velocity mesh? tmask if I am right is related to the Dirichlet b.c. on the temperature mesh, should I replace this with v1mask if I work on velocity components? > 5) then I should be done, the example continues computing the gradient of psi to get the velocity components from the velocity potential, but I don't need this. > > Thanks also to Aleks for his help with the first part of my question, I will write again if I have other questions. > Best regards, > Giuseppe > > > > Il giorno 04/apr/2014, alle ore 20:01, > ha scritto: > >> >> Hi Giuseppe, >> >> If you look at the .usr file in examples/eddy_psi_omega/ >> you'll see a call for a Poisson solve for a little psi-omega formulation >> of Navier-Stokes. >> >> Please let me know if this provides the insight you seek for setting >> up your Poisson solves. >> >> Best regards, >> >> 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, April 04, 2014 7:09 AM >> To: nek5000-users at lists.mcs.anl.gov >> Subject: [Nek5000-users] multiple runs and poisson for velocity >> >> Dear Neks, >> I have two issues that I would like to discuss with you. >> Firstly, I would like to perform many steady state simulations with different values of the viscosity, each time using the previous solution as starting condition. >> For this reason, I have built the following subroutine: >> >> c----------------------------------------------------------------------- >> subroutine userchk >> include 'SIZE' >> include 'TOTAL' >> >> >> do 120 ire=1,10 >> param(2) = -1*ire >> call setprop >> igeom=1 >> call fluid(igeom) >> 120 continue >> >> ifxyo = .true. >> call outpost(vx,vy,vz,pr,t,'ste') >> call exitt >> >> return >> end >> c----------------------------------------------------------------------- >> >> but this does not work as I expected, could somebody suggest me what I should do instead? >> >> Secondly, I would like to solve (in postprocessing mode) a Poisson problem for the velocity components, in the form -lapl(vx) = fx and -lapl(vy)=fy, with fx and fy known. >> Is it possible to do this within NEK? I think this could be done by adapting the Uzawa pressure solver in navier1.f, but I am not sure if this could work. >> Best regards, >> Giuseppe >> _______________________________________________ >> 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 Mon Apr 7 09:13:41 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 7 Apr 2014 18:43:41 +0430 Subject: [Nek5000-users] Prenek Problem Message-ID: Dear Neks, I would like to use prenek to refine a generated mesh. Whenever I try to use prenek, after typing prex command a new window will appear. It has a red bar in the right side and a black window in the left side. After that the following scripts are appeared: -Adobe-Helvetica-Medium-R-Normal--12-120-75-75-P-67-ISO8859-1 I/O Error: No String Terminator sent to PRS NEKTON Version 2.6 cp: cannot stat ~/.nekdefaults': No such file or directory (6144,6144,6144) (61440,61440,61440) (61440, 0, 0) (61440,61440, 0) (30720,30720,30720) ( 0, 0,61440) (61440, 0,43008) (61440,61440, 0) (43008,61440, 0) (12288,61440,12288) ( 0,61440,61440) ( 0,18432,61440) (61440, 0,61440) (61440, 0,12288) (36864,36864,36864) (30720,30720,43008) Choose a Name for This Session: , And no graphical menu is appeared. Besides, by typing any key to choose a name for the session, nothing will be done! Could you please guide me how to fix the problem and use graphical menu? Best Regards, Omid Atlaschian -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Apr 7 12:27:03 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 7 Apr 2014 19:27:03 +0200 Subject: [Nek5000-users] Prenek Problem In-Reply-To: References: Message-ID: Hi, Omid, It is normal. You should type the name of the session on the new graphical screen and 'enter'. Then you look at the terminal window in which you launched prenek. You will see new lines appears which demands you for furthur steps. Prenek and postx are a very old tools, and not graphically adapted in debian-based systems. You can install some libraries. It will fix several the problem, but not all. I think the best way is to write a script, which can be read by prenek. You can find the example ext_cyl, in which the file mkmesh is a simple example. It is not easy, and needs a lot of time to try and adjust by yourself, since the prenek is too difficult to be used graphically and interactively. Good luck! mesa-utils libx11-* libxt-dev xfonts-100dpi xfonts-100dpi-transcoded xfonts-75dpi xfonts-75dpi-transcoded Tubois On Mon, Apr 7, 2014 at 4:13 PM, wrote: > Dear Neks, > > > > I would like to use prenek to refine a generated mesh. > Whenever I try to use prenek, after typing prex command a new window will > appear. It has a red bar in the right side and a black window in the left > side. After that the following scripts are appeared: > > -Adobe-Helvetica-Medium-R-Normal--12-120-75-75-P-67-ISO8859-1 > > I/O Error: No String Terminator sent to PRS > > NEKTON Version > 2.6 > > cp: cannot stat ~/.nekdefaults': No such file or directory > > (6144,6144,6144) > > (61440,61440,61440) > > (61440, 0, 0) > > (61440,61440, 0) > > (30720,30720,30720) > > ( 0, 0,61440) > > (61440, 0,43008) > > (61440,61440, 0) > > (43008,61440, 0) > > (12288,61440,12288) > > ( 0,61440,61440) > > ( 0,18432,61440) > > (61440, 0,61440) > > (61440, 0,12288) > > (36864,36864,36864) > > (30720,30720,43008) > > Choose a Name for This Session: > > , > > And no graphical menu is appeared. Besides, by typing any key to choose a > name for the session, nothing will be done! > > Could you please guide me how to fix the problem and use graphical menu? > > > Best Regards, > Omid Atlaschian > > > > _______________________________________________ > 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 Apr 9 07:23:09 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 09 Apr 2014 08:23:09 -0400 Subject: [Nek5000-users] Test expansion exitting Message-ID: Hi, When I run the expansion example, it stops with the following message: call exitt: dying ... backtrace(): obtained 6 stack frames. ./nek5000(print_stack_+0x75) [0x6651cd] ./nek5000(exitt_+0x39f) [0x76aad3] ./nek5000(MAIN__+0x82) [0x44d4ce] ./nek5000(main+0x46) [0x44c926] /lib64/libc.so.6(__libc_start_main+0xfd) [0x39ad21ecdd] ./nek5000() [0x44c819] total elapsed time : 8.44085E+02 sec total solver time incl. I/O : 8.33374E+02 sec time/timestep : 8.33374E+00 sec CPU seconds/timestep/gridpt : 1.75151E-04 sec I am confused because it does not give a reason for the exit. The prior messages are: end of time-step loop runtime statistics: total time 833.373782019479 inv3 time 200 0.255646467208862 3.067608709616051E-004 invc time 432300 0.812657833099365 9.751420678606974E-004 mltd time 300 12.5136275291443 1.501562420024847E-002 cdtp time 300 5.82422852516174 6.988735008015416E-003 eslv time 0 0.000000000000000E+000 0.000000000000000E+000 pres time 100 541.141169071198 0.649337885048259 crsl time 1411 4.03384947776794 4.840384428692834E-003 crsl min 3.67473864555359 crsl max 4.51544284820557 crsl avg 4.06963658332825 hmhz time 303 650.444540500641 0.780495564576613 spro time 101 0.366436719894409 4.397027213964407E-004 usbc time 100 3.17075777053833 3.804724649310142E-003 usbc min 3.17075777053833 usbc max 3.60764217376709 usb avg 3.30022418498993 axhm time 5496 220.912309885025 0.265081905204286 advc time 300 52.1149857044220 6.253494749754901E-002 vdss time 301 2.21998190879822 2.663848991527703E-003 vdss min 2.21998190879822 vdss max 2.35859322547913 vdss avg 2.29367226362228 dsum time 6784 14.5266296863556 1.743110954505171E-002 dsum min 14.0492208003998 dsum max 14.5668377876282 dsum avg 14.3548709750175 dadd time 0 24.6760597229004 2.960983445279973E-002 ddsl time 0 0.000000000000000E+000 0.000000000000000E+000 solv time 0 0.000000000000000E+000 0.000000000000000E+000 prep time 100 0.362718105316162 4.352406004868580E-004 # nid tusbc tdadd tcrsl tvdss tdsum tgop qqq F 0 3.1708E+00 2.4676E+01 4.0338E+00 2.2200E+00 1.4527E+01 2.6212E-03 qqq 1 3.6076E+00 2.5966E+01 4.5154E+00 2.3586E+00 1.4049E+01 8.9169E-04 qqq 2 3.2093E+00 2.5622E+01 4.0545E+00 2.2720E+00 1.4277E+01 3.8743E-04 qqq 3 3.2132E+00 2.5637E+01 3.6747E+00 2.3241E+00 1.4567E+01 3.7360E-04 qqq call exitt: dying ... Its running on 4 processors, hence the various nids. Is there anything wrong, and if so, how should I fix it? Thanks, Tania -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Apr 10 09:49:03 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 10 Apr 2014 22:49:03 +0800 (GMT+08:00) Subject: [Nek5000-users] How to create .usr file Message-ID: Dear All, I am trying nek5000 under ubuntu. As a beginner, I just wonder which is the best way to create the .usr file, should I copy one from the examples and change it for my case or use a tool just like genbox, genmap, etc. to generate it? I have the same question for creation of SIZE By the way, I can only find the usage of prenek and demonstrative cases from the old manual of nekton, what is the current way of generating meshes for public uses? Thank you very much in advance. Zhenyu -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Apr 9 10:17:25 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 09 Apr 2014 17:17:25 +0200 Subject: [Nek5000-users] How to create .usr file In-Reply-To: References: Message-ID: Hi Zhenyu, The *.usr is to be copied from the examples and change it according to your needs like Boundary condition and Initial condition. The SIZE file too should be copied (change the number of element per processor according to yours) . See the example 'Expansion ' --> mkmesh file, which will give you an insight about how to write a script to create a mesh using prenek. Best Regards, Kamal. On 10/04/2014 16:49, nek5000-users at lists.mcs.anl.gov wrote: > Dear All, > > I am trying nek5000 under ubuntu. > > As a beginner, I just wonder which is the best way to create the .usr > file, should I copy one from the examples and change it for my case or > use a tool just like genbox, genmap, etc. to generate it? I have the > same question for creation of SIZE > > By the way, I can only find the usage of prenek and demonstrative > cases from the old manual of nekton, what is the current way of > generating meshes for public uses? > > Thank you very much in advance. > > Zhenyu > > > _______________________________________________ > 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 Apr 10 21:23:24 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 11 Apr 2014 10:23:24 +0800 (GMT+08:00) Subject: [Nek5000-users] How to create .usr file In-Reply-To: References: Message-ID: Dear Kamal, It's so nice to get your quick and fully functional reply. In fact, last night I examined the expansion case carefully and ran once with nekbmpi. the script mkmesh gives me a very good example for pushing myself further. Now I'm working on dealing the result with Visit. So Thank you so much for your help. Yours, Zhenyu -----????----- ???: nek5000-users at lists.mcs.anl.gov ????: 2014-04-09 23:17:25 (???) ???: nek5000-users at lists.mcs.anl.gov ??: ??: Re: [Nek5000-users] How to create .usr file Hi Zhenyu, The *.usr is to be copied from the examples and change it according to your needs like Boundary condition and Initial condition. The SIZE file too should be copied (change the number of element per processor according to yours) . See the example 'Expansion ' --> mkmesh file, which will give you an insight about how to write a script to create a mesh using prenek. Best Regards, Kamal. On 10/04/2014 16:49, nek5000-users at lists.mcs.anl.gov wrote: Dear All, I am trying nek5000 under ubuntu. As a beginner, I just wonder which is the best way to create the .usr file, should I copy one from the examples and change it for my case or use a tool just like genbox, genmap, etc. to generate it? I have the same question for creation of SIZE By the way, I can only find the usage of prenek and demonstrative cases from the old manual of nekton, what is the current way of generating meshes for public uses? Thank you very much in advance. Zhenyu _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.govhttps://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 Apr 10 07:13:22 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 10 Apr 2014 14:13:22 +0200 Subject: [Nek5000-users] Restart option failed Message-ID: Hello Neks, I tried to restart my simulation from a previous output *.f file but it failed I set the restart option in *.rea to 1 and added the file name. Could some please tell me what might be the possible cause for this ? *********************************************************************** nekuic (1) for ifld 1 Reading checkpoint data 0 0 OPEN: extens0.f00250 extens0.f00250 byte_read() :: fopen failure2! ERROR: Error reading restart header in mfi_prepare ierr= 1 call exitt: dying ... ************************************************************************ Thanks in advance. Kamal From nek5000-users at lists.mcs.anl.gov Fri Apr 11 07:18:43 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 11 Apr 2014 14:18:43 +0200 Subject: [Nek5000-users] Restart option failed In-Reply-To: References: Message-ID: Hi Kamal, Check out the parameters 64 or 65 in your .rea file. It is very likely that it is set to -4 instead of a positive number. Cheers, JC 2014-04-10 14:13 GMT+02:00 : > Hello Neks, > > I tried to restart my simulation from a previous output *.f file but it > failed > > I set the restart option in *.rea to 1 and added the file name. > > Could some please tell me what might be the possible cause for this ? > > *********************************************************************** > nekuic (1) for ifld 1 > Reading checkpoint data > 0 0 OPEN: extens0.f00250 > extens0.f00250 > byte_read() :: fopen failure2! > ERROR: Error reading restart header in mfi_prepare ierr= 1 > > call exitt: dying ... > > ************************************************************************ > > Thanks in advance. > > Kamal > > _______________________________________________ > 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 Thu Apr 10 09:09:00 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 10 Apr 2014 16:09:00 +0200 Subject: [Nek5000-users] Restart option failed In-Reply-To: References: Message-ID: Hi JC, Thanks for the reply The parameters are positive 0.00000 p064 =1 --> perturbation restart 1.00000 p065 #iofiles (eg, 0 or 64); <0 --> sep. dirs 6.00000 p066 output : <0=ascii, else binary 6.00000 p067 restart: <0=ascii, else binary Regards, Kamal On 11/04/2014 14:18, nek5000-users at lists.mcs.anl.gov wrote: > Hi Kamal, > > Check out the parameters 64 or 65 in your .rea file. It is very likely > that it is set to -4 instead of a positive number. > > Cheers, > JC > > > 2014-04-10 14:13 GMT+02:00 >: > > Hello Neks, > > I tried to restart my simulation from a previous output *.f file > but it failed > > I set the restart option in *.rea to 1 and added the file name. > > Could some please tell me what might be the possible cause for this ? > > *********************************************************************** > nekuic (1) for ifld 1 > Reading checkpoint data > 0 0 OPEN: extens0.f00250 > extens0.f00250 > byte_read() :: fopen failure2! > ERROR: Error reading restart header in mfi_prepare ierr= 1 > > call exitt: dying ... > > ************************************************************************ > > Thanks in advance. > > Kamal > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > > > -- > Jean-Christophe Loiseau > Homepage > > > _______________________________________________ > 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 Apr 11 09:52:02 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 11 Apr 2014 14:52:02 +0000 Subject: [Nek5000-users] Restart option failed In-Reply-To: References: , Message-ID: Hi Kamal, Make certain tey aren't reset in your .usr file. 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: Thursday, April 10, 2014 9:09 AM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Restart option failed Hi JC, Thanks for the reply The parameters are positive 0.00000 p064 =1 --> perturbation restart 1.00000 p065 #iofiles (eg, 0 or 64); <0 --> sep. dirs 6.00000 p066 output : <0=ascii, else binary 6.00000 p067 restart: <0=ascii, else binary Regards, Kamal On 11/04/2014 14:18, nek5000-users at lists.mcs.anl.gov wrote: Hi Kamal, Check out the parameters 64 or 65 in your .rea file. It is very likely that it is set to -4 instead of a positive number. Cheers, JC 2014-04-10 14:13 GMT+02:00 >: Hello Neks, I tried to restart my simulation from a previous output *.f file but it failed I set the restart option in *.rea to 1 and added the file name. Could some please tell me what might be the possible cause for this ? *********************************************************************** nekuic (1) for ifld 1 Reading checkpoint data 0 0 OPEN: extens0.f00250 extens0.f00250 byte_read() :: fopen failure2! ERROR: Error reading restart header in mfi_prepare ierr= 1 call exitt: dying ... ************************************************************************ Thanks in advance. Kamal _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -- Jean-Christophe Loiseau Homepage _______________________________________________ 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 Apr 10 09:57:52 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 10 Apr 2014 16:57:52 +0200 Subject: [Nek5000-users] Restart option failed In-Reply-To: References: , Message-ID: Hi Paul, I don't change parameters through the .usr file. Thank you Kamal On 11/04/2014 16:52, nek5000-users at lists.mcs.anl.gov wrote: > > Hi Kamal, > > Make certain tey aren't reset in your .usr file. > > 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:* Thursday, April 10, 2014 9:09 AM > *To:* nek5000-users at lists.mcs.anl.gov > *Subject:* Re: [Nek5000-users] Restart option failed > > > Hi JC, > > Thanks for the reply > > The parameters are positive > 0.00000 p064 =1 --> perturbation restart > 1.00000 p065 #iofiles (eg, 0 or 64); <0 --> sep. dirs > 6.00000 p066 output : <0=ascii, else binary > 6.00000 p067 restart: <0=ascii, else binary > > Regards, > Kamal > > > On 11/04/2014 14:18, nek5000-users at lists.mcs.anl.gov wrote: >> Hi Kamal, >> >> Check out the parameters 64 or 65 in your .rea file. It is very >> likely that it is set to -4 instead of a positive number. >> >> Cheers, >> JC >> >> >> 2014-04-10 14:13 GMT+02:00 > >: >> >> Hello Neks, >> >> I tried to restart my simulation from a previous output *.f file >> but it failed >> >> I set the restart option in *.rea to 1 and added the file name. >> >> Could some please tell me what might be the possible cause for this ? >> >> *********************************************************************** >> nekuic (1) for ifld 1 >> Reading checkpoint data >> 0 0 OPEN: extens0.f00250 >> extens0.f00250 >> byte_read() :: fopen failure2! >> ERROR: Error reading restart header in mfi_prepare ierr= 1 >> >> call exitt: dying ... >> >> ************************************************************************ >> >> Thanks in advance. >> >> Kamal >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> >> >> >> >> -- >> Jean-Christophe Loiseau >> Homepage >> >> >> _______________________________________________ >> 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 Apr 11 10:43:17 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 11 Apr 2014 10:43:17 -0500 Subject: [Nek5000-users] Restart option failed In-Reply-To: References: Message-ID: Hi, Is your restart file a 0.f00000 format? If the param (67) is not set in the .usr file, the default is set to 0 . f00000. Katie Katie On Apr 11, 2014 9:56 AM, wrote: > Hi Paul, > > I don't change parameters through the .usr file. > Thank you > > Kamal > > On 11/04/2014 16:52, nek5000-users at lists.mcs.anl.gov wrote: > > > Hi Kamal, > > Make certain tey aren't reset in your .usr file. > > 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:* Thursday, April 10, 2014 9:09 AM > *To:* nek5000-users at lists.mcs.anl.gov > *Subject:* Re: [Nek5000-users] Restart option failed > > > Hi JC, > > Thanks for the reply > > The parameters are positive > 0.00000 p064 =1 --> perturbation restart > 1.00000 p065 #iofiles (eg, 0 or 64); <0 --> sep. dirs > 6.00000 p066 output : <0=ascii, else binary > 6.00000 p067 restart: <0=ascii, else binary > > Regards, > Kamal > > > On 11/04/2014 14:18, nek5000-users at lists.mcs.anl.gov wrote: > > Hi Kamal, > > Check out the parameters 64 or 65 in your .rea file. It is very likely > that it is set to -4 instead of a positive number. > > Cheers, > JC > > > 2014-04-10 14:13 GMT+02:00 : > >> Hello Neks, >> >> I tried to restart my simulation from a previous output *.f file but it >> failed >> >> I set the restart option in *.rea to 1 and added the file name. >> >> Could some please tell me what might be the possible cause for this ? >> >> *********************************************************************** >> nekuic (1) for ifld 1 >> Reading checkpoint data >> 0 0 OPEN: extens0.f00250 >> extens0.f00250 >> byte_read() :: fopen failure2! >> ERROR: Error reading restart header in mfi_prepare ierr= 1 >> >> call exitt: dying ... >> >> ************************************************************************ >> >> Thanks in advance. >> >> Kamal >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> > > > > -- > Jean-Christophe Loiseau > Homepage > > > _______________________________________________ > Nek5000-users mailing listNek5000-users at lists.mcs.anl.govhttps://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 Thu Apr 10 10:48:11 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 10 Apr 2014 17:48:11 +0200 Subject: [Nek5000-users] Restart option failed In-Reply-To: References: Message-ID: Hi Katie, yes, my restart file is 0.f00000 format and the parameter in *.rea file is ' 6.00000 p067 restart: <0=ascii, else binary ' Thanks for your reply. Kamal On 11/04/2014 17:43, nek5000-users at lists.mcs.anl.gov wrote: > > Hi, > > Is your restart file a 0.f00000 format? > If the param (67) is not set in the .usr file, the default is set to 0 > . f00000. > > Katie > > Katie > > On Apr 11, 2014 9:56 AM, > wrote: > > Hi Paul, > > I don't change parameters through the .usr file. > Thank you > > Kamal > > On 11/04/2014 16:52, nek5000-users at lists.mcs.anl.gov > wrote: >> >> Hi Kamal, >> >> Make certain tey aren't reset in your .usr file. >> >> 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:* Thursday, April 10, 2014 9:09 AM >> *To:* nek5000-users at lists.mcs.anl.gov >> >> *Subject:* Re: [Nek5000-users] Restart option failed >> >> >> Hi JC, >> >> Thanks for the reply >> >> The parameters are positive >> 0.00000 p064 =1 --> perturbation restart >> 1.00000 p065 #iofiles (eg, 0 or 64); <0 --> sep. dirs >> 6.00000 p066 output : <0=ascii, else binary >> 6.00000 p067 restart: <0=ascii, else binary >> >> Regards, >> Kamal >> >> >> On 11/04/2014 14:18, nek5000-users at lists.mcs.anl.gov >> wrote: >>> Hi Kamal, >>> >>> Check out the parameters 64 or 65 in your .rea file. It is very >>> likely that it is set to -4 instead of a positive number. >>> >>> Cheers, >>> JC >>> >>> >>> 2014-04-10 14:13 GMT+02:00 >> >: >>> >>> Hello Neks, >>> >>> I tried to restart my simulation from a previous output *.f >>> file but it failed >>> >>> I set the restart option in *.rea to 1 and added the file name. >>> >>> Could some please tell me what might be the possible cause >>> for this ? >>> >>> *********************************************************************** >>> nekuic (1) for ifld 1 >>> Reading checkpoint data >>> 0 0 OPEN: extens0.f00250 >>> extens0.f00250 >>> byte_read() :: fopen failure2! >>> ERROR: Error reading restart header in mfi_prepare ierr= 1 >>> >>> call exitt: dying ... >>> >>> ************************************************************************ >>> >>> Thanks in advance. >>> >>> Kamal >>> >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>> >>> >>> >>> >>> -- >>> Jean-Christophe Loiseau >>> Homepage >>> >>> >>> _______________________________________________ >>> 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 Fri Apr 11 18:24:51 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sat, 12 Apr 2014 01:24:51 +0200 Subject: [Nek5000-users] Restart option failed In-Reply-To: References: Message-ID: Hello Neks, I did a SVN update of the nek files to be sure that I don't miss some updates. I got the version 1021. But this time when I launch my code, I get this error ************************************************************ verify mesh topology 0.0000000000000000 6.2831853071795862 Xrange 0.0000000000000000 6.2831853071795862 Yrange 0.0000000000000000 0.0000000000000000 Zrange ERROR (proc 0002, /Users/kamalselvam/nek5_svn/trunk/nek/jl/gs.c:1234): gs_op: op 4 not in valid range 1-3 ERROR (proc 0003, /Users/kamalselvam/nek5_svn/trunk/nek/jl/gs.c:1234): gs_op: op 4 not in valid range 1-3 ERROR (proc 0000, /Users/kamalselvam/nek5_svn/trunk/nek/jl/gs.c:1234): gs_op: op 4 not in valid range 1-3 ERROR (proc 0001, /Users/kamalselvam/nek5_svn/trunk/nek/jl/gs.c:1234): gs_op: op 4 not in valid range 1-3 ******************************************************************** Thank you in advance, Kamal On 10 Apr 2014, at 17:48, nek5000-users at lists.mcs.anl.gov wrote: > Hi Katie, > > yes, my restart file is 0.f00000 format and the parameter in *.rea file is ' 6.00000 p067 restart: <0=ascii, else binary ' > Thanks for your reply. > > > Kamal > > On 11/04/2014 17:43, nek5000-users at lists.mcs.anl.gov wrote: >> Hi, >> >> Is your restart file a 0.f00000 format? >> If the param (67) is not set in the .usr file, the default is set to 0 . f00000. >> Katie >> >> Katie >> >> On Apr 11, 2014 9:56 AM, wrote: >> Hi Paul, >> >> I don't change parameters through the .usr file. >> Thank you >> >> Kamal >> >> On 11/04/2014 16:52, nek5000-users at lists.mcs.anl.gov wrote: >>> >>> Hi Kamal, >>> >>> Make certain tey aren't reset in your .usr file. >>> >>> 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: Thursday, April 10, 2014 9:09 AM >>> To: nek5000-users at lists.mcs.anl.gov >>> Subject: Re: [Nek5000-users] Restart option failed >>> >>> >>> Hi JC, >>> >>> Thanks for the reply >>> >>> The parameters are positive >>> 0.00000 p064 =1 --> perturbation restart >>> 1.00000 p065 #iofiles (eg, 0 or 64); <0 --> sep. dirs >>> 6.00000 p066 output : <0=ascii, else binary >>> 6.00000 p067 restart: <0=ascii, else binary >>> >>> Regards, >>> Kamal >>> >>> >>> On 11/04/2014 14:18, nek5000-users at lists.mcs.anl.gov wrote: >>>> Hi Kamal, >>>> >>>> Check out the parameters 64 or 65 in your .rea file. It is very likely that it is set to -4 instead of a positive number. >>>> >>>> Cheers, >>>> JC >>>> >>>> >>>> 2014-04-10 14:13 GMT+02:00 : >>>> Hello Neks, >>>> >>>> I tried to restart my simulation from a previous output *.f file but it failed >>>> >>>> I set the restart option in *.rea to 1 and added the file name. >>>> >>>> Could some please tell me what might be the possible cause for this ? >>>> >>>> *********************************************************************** >>>> nekuic (1) for ifld 1 >>>> Reading checkpoint data >>>> 0 0 OPEN: extens0.f00250 >>>> extens0.f00250 >>>> byte_read() :: fopen failure2! >>>> ERROR: Error reading restart header in mfi_prepare ierr= 1 >>>> >>>> call exitt: dying ... >>>> >>>> ************************************************************************ >>>> >>>> Thanks in advance. >>>> >>>> Kamal >>>> >>>> _______________________________________________ >>>> Nek5000-users mailing list >>>> Nek5000-users at lists.mcs.anl.gov >>>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>>> >>>> >>>> >>>> -- >>>> Jean-Christophe Loiseau >>>> Homepage >>>> >>>> >>>> _______________________________________________ >>>> 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 Sun Apr 13 10:47:28 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 13 Apr 2014 11:47:28 -0400 Subject: [Nek5000-users] usr file - Vol 62, Issue 9 In-Reply-To: References: Message-ID: Zhenyu, Hi... In general, you do the following: Use an existing run files as templates to start with. You need the .rea, SIZE, .box, and .usr files. Rename the rea,box, and usr files to a unique name for your run, like your_run.rea, your_run.box, your_run.usr. * Edit the .box file to define your grid, geometry, and BCs. * Edit the .rea file with all the basic run parameters. If you have an .rea template that is ascii (without the .re2 option) and it has geometry information at the end, ignore this information as it will be regenerated. * Edit the SIZE file to set your array sizes and GLL DOF (this must also be set correctly in .rea). * Edit the .usr file per instructions, including the information for boundary conditions if applicable. Then, you generate a new .rea file with the grid geometry by running genbox: "genbox ./your_run.box". This will create the files box.rea and box.tmp. You rename box.rea to your_run.rea. This will overwrite the one you edited with a new one with all your changes in the settings sections intact, and new geometry information at the end. Delete box.tmp. Next, you run genmap to create a new map file: "genmap ./your_run". This will create the new map file. Next, compile the code with: "./makenek ./your_run". If successful, you will get a new binary copy of nek5000. Then you run with one of the scripts like: "./nekbmpi ./your_run 24" You will probably get a lot of errors initially based on improper makenek setting for your compiler and target platform, geometry issues, etc... Read all the documentation and look at the examples to figure this stuff out for your application... See Ya, Murph mlodea at oakland.edu > > ForwardedMessage.eml > > Subject: > [Nek5000-users] How to create .usr file > From: > nek5000-users at lists.mcs.anl.gov > Date: > 4/10/2014 10:49 AM > > To: > Nek5000-users at lists.mcs.anl.gov > > > Dear All, > > I am trying nek5000 under ubuntu. > > As a beginner, I just wonder which is the best way to create the .usr > file, should I copy one from the examples and change it for my case or > use a tool just like genbox, genmap, etc. to generate it? I have the > same question for creation of SIZE > > By the way, I can only find the usage of prenek and demonstrative > cases from the old manual of nekton, what is the current way of > generating meshes for public uses? > > Thank you very much in advance. > > Zhenyu > > ForwardedMessage.eml > > Subject: > Re: [Nek5000-users] How to create .usr file > From: > nek5000-users at lists.mcs.anl.gov > Date: > 4/9/2014 11:17 AM > > To: > nek5000-users at lists.mcs.anl.gov > > > Hi Zhenyu, > > The *.usr is to be copied from the examples and change it according to > your needs like Boundary condition and Initial condition. > > The SIZE file too should be copied (change the number of element per > processor according to yours) . > > See the example 'Expansion ' --> mkmesh file, which will give you an > insight about how to write a script to create a mesh using prenek. > > Best Regards, > Kamal. > > > On 10/04/2014 16:49, nek5000-users at lists.mcs.anl.gov wrote: >> Dear All, >> >> I am trying nek5000 under ubuntu. >> >> As a beginner, I just wonder which is the best way to create the >> .usr file, should I copy one from the examples and change it for my >> case or use a tool just like genbox, genmap, etc. to generate it? I >> have the same question for creation of SIZE >> >> By the way, I can only find the usage of prenek and demonstrative >> cases from the old manual of nekton, what is the current way of >> generating meshes for public uses? >> >> Thank you very much in advance. >> >> Zhenyu >> >> >> _______________________________________________ >> 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 Sun Apr 13 19:30:27 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 14 Apr 2014 08:30:27 +0800 (GMT+08:00) Subject: [Nek5000-users] usr file - Vol 62, Issue 9 In-Reply-To: References: Message-ID: Dear Murph, I carried on along your suggested way and at least got some expected results for case expanson. Thank you very much for your guidance. Yours, Zhenyu -----????----- ???: nek5000-users at lists.mcs.anl.gov ????: 2014-04-13 23:47:28 (???) ???: nek5000-users at lists.mcs.anl.gov ??: ??: Re: [Nek5000-users] usr file - Vol 62, Issue 9 Zhenyu, Hi... In general, you do the following: Use an existing run files as templates to start with. You need the .rea, SIZE, .box, and .usr files. Rename the rea,box, and usr files to a unique name for your run, like your_run.rea, your_run.box, your_run.usr. Edit the .box file to define your grid, geometry, and BCs. Edit the .rea file with all the basic run parameters. If you have an .rea template that is ascii (without the .re2 option) and it has geometry information at the end, ignore this information as it will be regenerated. Edit the SIZE file to set your array sizes and GLL DOF (this must also be set correctly in .rea). Edit the .usr file per instructions, including the information for boundary conditions if applicable. Then, you generate a new .rea file with the grid geometry by running genbox: "genbox ./your_run.box". This will create the files box.rea and box.tmp. You rename box.rea to your_run.rea. This will overwrite the one you edited with a new one with all your changes in the settings sections intact, and new geometry information at the end. Delete box.tmp. Next, you run genmap to create a new map file: "genmap ./your_run". This will create the new map file. Next, compile the code with: "./makenek ./your_run". If successful, you will get a new binary copy of nek5000. Then you run with one of the scripts like: "./nekbmpi ./your_run 24" You will probably get a lot of errors initially based on improper makenek setting for your compiler and target platform, geometry issues, etc... Read all the documentation and look at the examples to figure this stuff out for your application... See Ya, Murph mlodea at oakland.edu ForwardedMessage.eml | Subject: [Nek5000-users] How to create .usr file | | From: nek5000-users at lists.mcs.anl.gov | | Date: 4/10/2014 10:49 AM | | To: Nek5000-users at lists.mcs.anl.gov | Dear All, I am trying nek5000 under ubuntu. As a beginner, I just wonder which is the best way to create the .usr file, should I copy one from the examples and change it for my case or use a tool just like genbox, genmap, etc. to generate it? I have the same question for creation of SIZE By the way, I can only find the usage of prenek and demonstrative cases from the old manual of nekton, what is the current way of generating meshes for public uses? Thank you very much in advance. Zhenyu ForwardedMessage.eml | Subject: Re: [Nek5000-users] How to create .usr file | | From: nek5000-users at lists.mcs.anl.gov | | Date: 4/9/2014 11:17 AM | | To: nek5000-users at lists.mcs.anl.gov | Hi Zhenyu, The *.usr is to be copied from the examples and change it according to your needs like Boundary condition and Initial condition. The SIZE file too should be copied (change the number of element per processor according to yours) . See the example 'Expansion ' --> mkmesh file, which will give you an insight about how to write a script to create a mesh using prenek. Best Regards, Kamal. On 10/04/2014 16:49, nek5000-users at lists.mcs.anl.gov wrote: Dear All, I am trying nek5000 under ubuntu. As a beginner, I just wonder which is the best way to create the .usr file, should I copy one from the examples and change it for my case or use a tool just like genbox, genmap, etc. to generate it? I have the same question for creation of SIZE By the way, I can only find the usage of prenek and demonstrative cases from the old manual of nekton, what is the current way of generating meshes for public uses? Thank you very much in advance. Zhenyu _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.govhttps://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.govhttps://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Sun Apr 13 06:55:14 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 13 Apr 2014 13:55:14 +0200 Subject: [Nek5000-users] Restart option failed In-Reply-To: References: Message-ID: Hello Neks, I figured out where the error of restart fail comes from. Its because the code is not looking in to the working directory for the file. In " byte.c " file I made a small change to the byte_read () function, instead of having the variable " name " I changed it to the path of my restart file ---------------------------------------------------------------------------------------------------- if (!fp) { if (!(fp=fopen("/home/2014012/jpeixi01/neksamples/eddy/eddy_uv0.f00012","rb"))) { printf("%s\n",name); printf("byte_read() :: fopen failure2!\n"); *ierr=1; return; } flag=READ; } ----------------------------------------------------------------------------------------------------- this worked for me. Now I would like to know why is the code not looking into the working directory, If so where do I change it to overcome this problem so that I don't have to change the path every single time. Thanks a lot, BOW On 11/04/2014 17:43, nek5000-users at lists.mcs.anl.gov wrote: > > Hi, > > Is your restart file a 0.f00000 format? > If the param (67) is not set in the .usr file, the default is set to 0 > . f00000. > > Katie > > Katie > > On Apr 11, 2014 9:56 AM, > wrote: > > Hi Paul, > > I don't change parameters through the .usr file. > Thank you > > Kamal > > On 11/04/2014 16:52, nek5000-users at lists.mcs.anl.gov > wrote: >> >> Hi Kamal, >> >> Make certain tey aren't reset in your .usr file. >> >> 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:* Thursday, April 10, 2014 9:09 AM >> *To:* nek5000-users at lists.mcs.anl.gov >> >> *Subject:* Re: [Nek5000-users] Restart option failed >> >> >> Hi JC, >> >> Thanks for the reply >> >> The parameters are positive >> 0.00000 p064 =1 --> perturbation restart >> 1.00000 p065 #iofiles (eg, 0 or 64); <0 --> sep. dirs >> 6.00000 p066 output : <0=ascii, else binary >> 6.00000 p067 restart: <0=ascii, else binary >> >> Regards, >> Kamal >> >> >> On 11/04/2014 14:18, nek5000-users at lists.mcs.anl.gov >> wrote: >>> Hi Kamal, >>> >>> Check out the parameters 64 or 65 in your .rea file. It is very >>> likely that it is set to -4 instead of a positive number. >>> >>> Cheers, >>> JC >>> >>> >>> 2014-04-10 14:13 GMT+02:00 >> >: >>> >>> Hello Neks, >>> >>> I tried to restart my simulation from a previous output *.f >>> file but it failed >>> >>> I set the restart option in *.rea to 1 and added the file name. >>> >>> Could some please tell me what might be the possible cause >>> for this ? >>> >>> *********************************************************************** >>> nekuic (1) for ifld 1 >>> Reading checkpoint data >>> 0 0 OPEN: extens0.f00250 >>> extens0.f00250 >>> byte_read() :: fopen failure2! >>> ERROR: Error reading restart header in mfi_prepare ierr= 1 >>> >>> call exitt: dying ... >>> >>> ************************************************************************ >>> >>> Thanks in advance. >>> >>> Kamal >>> >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>> >>> >>> >>> >>> -- >>> Jean-Christophe Loiseau >>> Homepage >>> >>> >>> _______________________________________________ >>> 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 Apr 14 08:49:25 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 14 Apr 2014 13:49:25 +0000 Subject: [Nek5000-users] Restart option failed In-Reply-To: References: , Message-ID: Hi Kamal, If you use one of the nek scripts in tools/scripts (e.g., nek, nekb, nekmpi, nekbmpi, etc.), the path issues should be resolved for you. That's the normal approach. I believe some of this is outlined in the "quick start" section of the manual. 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: Sunday, April 13, 2014 6:55 AM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Restart option failed Hello Neks, I figured out where the error of restart fail comes from. Its because the code is not looking in to the working directory for the file. In " byte.c " file I made a small change to the byte_read () function, instead of having the variable " name " I changed it to the path of my restart file ---------------------------------------------------------------------------------------------------- if (!fp) { if (!(fp=fopen("/home/2014012/jpeixi01/neksamples/eddy/eddy_uv0.f00012","rb"))) { printf("%s\n",name); printf("byte_read() :: fopen failure2!\n"); *ierr=1; return; } flag=READ; } ----------------------------------------------------------------------------------------------------- this worked for me. Now I would like to know why is the code not looking into the working directory, If so where do I change it to overcome this problem so that I don't have to change the path every single time. Thanks a lot, BOW On 11/04/2014 17:43, nek5000-users at lists.mcs.anl.gov wrote: Hi, Is your restart file a 0.f00000 format? If the param (67) is not set in the .usr file, the default is set to 0 . f00000. Katie Katie On Apr 11, 2014 9:56 AM, > wrote: Hi Paul, I don't change parameters through the .usr file. Thank you Kamal On 11/04/2014 16:52, nek5000-users at lists.mcs.anl.gov wrote: Hi Kamal, Make certain tey aren't reset in your .usr file. 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: Thursday, April 10, 2014 9:09 AM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Restart option failed Hi JC, Thanks for the reply The parameters are positive 0.00000 p064 =1 --> perturbation restart 1.00000 p065 #iofiles (eg, 0 or 64); <0 --> sep. dirs 6.00000 p066 output : <0=ascii, else binary 6.00000 p067 restart: <0=ascii, else binary Regards, Kamal On 11/04/2014 14:18, nek5000-users at lists.mcs.anl.gov wrote: Hi Kamal, Check out the parameters 64 or 65 in your .rea file. It is very likely that it is set to -4 instead of a positive number. Cheers, JC 2014-04-10 14:13 GMT+02:00 >: Hello Neks, I tried to restart my simulation from a previous output *.f file but it failed I set the restart option in *.rea to 1 and added the file name. Could some please tell me what might be the possible cause for this ? *********************************************************************** nekuic (1) for ifld 1 Reading checkpoint data 0 0 OPEN: extens0.f00250 extens0.f00250 byte_read() :: fopen failure2! ERROR: Error reading restart header in mfi_prepare ierr= 1 call exitt: dying ... ************************************************************************ Thanks in advance. Kamal _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -- Jean-Christophe Loiseau Homepage _______________________________________________ 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 Sun Apr 13 10:12:46 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 13 Apr 2014 17:12:46 +0200 Subject: [Nek5000-users] Restart option failed In-Reply-To: References: , Message-ID: Dear Paul, I use the ' nekbmpi ' scripts from the tools/script and nothing else. I guess the some where the PATH variable to working directory is getting changed. It's weird the same code works properly on my ubuntu and not my Mac. Thank you, Kamal On 14/04/2014 15:49, nek5000-users at lists.mcs.anl.gov wrote: > > Hi Kamal, > > If you use one of the nek scripts in tools/scripts (e.g., nek, nekb, > nekmpi, nekbmpi, etc.), the > path issues should be resolved for you. That's the normal approach. > I believe some of this > is outlined in the "quick start" section of the manual. > > 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:* Sunday, April 13, 2014 6:55 AM > *To:* nek5000-users at lists.mcs.anl.gov > *Subject:* Re: [Nek5000-users] Restart option failed > > Hello Neks, > > I figured out where the error of restart fail comes from. Its because > the code is not looking in to the working directory for the file. > > > In " byte.c " file I made a small change to the byte_read () function, > instead of having the variable " name " I changed it to the path of my > restart file > ---------------------------------------------------------------------------------------------------- > if (!fp) > { > if > (!(fp=fopen("/home/2014012/jpeixi01/neksamples/eddy/eddy_uv0.f00012","rb"))) > { > printf("%s\n",name); > printf("byte_read() :: fopen failure2!\n"); > *ierr=1; > return; > } > flag=READ; > } > ----------------------------------------------------------------------------------------------------- > > this worked for me. > > Now I would like to know why is the code not looking into the working > directory, If so where do I change it to overcome this problem so that > I don't have to change the path every single time. > > > Thanks a lot, > BOW > > > > On 11/04/2014 17:43, nek5000-users at lists.mcs.anl.gov wrote: >> >> Hi, >> >> Is your restart file a 0.f00000 format? >> If the param (67) is not set in the .usr file, the default is set to >> 0 . f00000. >> >> Katie >> >> Katie >> >> On Apr 11, 2014 9:56 AM, > > wrote: >> >> Hi Paul, >> >> I don't change parameters through the .usr file. >> Thank you >> >> Kamal >> >> On 11/04/2014 16:52, nek5000-users at lists.mcs.anl.gov >> wrote: >>> >>> Hi Kamal, >>> >>> Make certain tey aren't reset in your .usr file. >>> >>> 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:* Thursday, April 10, 2014 9:09 AM >>> *To:* nek5000-users at lists.mcs.anl.gov >>> >>> *Subject:* Re: [Nek5000-users] Restart option failed >>> >>> >>> Hi JC, >>> >>> Thanks for the reply >>> >>> The parameters are positive >>> 0.00000 p064 =1 --> perturbation restart >>> 1.00000 p065 #iofiles (eg, 0 or 64); <0 --> sep. dirs >>> 6.00000 p066 output : <0=ascii, else binary >>> 6.00000 p067 restart: <0=ascii, else binary >>> >>> Regards, >>> Kamal >>> >>> >>> On 11/04/2014 14:18, nek5000-users at lists.mcs.anl.gov >>> wrote: >>>> Hi Kamal, >>>> >>>> Check out the parameters 64 or 65 in your .rea file. It is very >>>> likely that it is set to -4 instead of a positive number. >>>> >>>> Cheers, >>>> JC >>>> >>>> >>>> 2014-04-10 14:13 GMT+02:00 >>> >: >>>> >>>> Hello Neks, >>>> >>>> I tried to restart my simulation from a previous output *.f >>>> file but it failed >>>> >>>> I set the restart option in *.rea to 1 and added the file name. >>>> >>>> Could some please tell me what might be the possible cause >>>> for this ? >>>> >>>> *********************************************************************** >>>> nekuic (1) for ifld 1 >>>> Reading checkpoint data >>>> 0 0 OPEN: extens0.f00250 >>>> extens0.f00250 >>>> byte_read() :: fopen failure2! >>>> ERROR: Error reading restart header in mfi_prepare ierr= 1 >>>> >>>> call exitt: dying ... >>>> >>>> ************************************************************************ >>>> >>>> Thanks in advance. >>>> >>>> Kamal >>>> >>>> _______________________________________________ >>>> Nek5000-users mailing list >>>> Nek5000-users at lists.mcs.anl.gov >>>> >>>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>>> >>>> >>>> >>>> >>>> -- >>>> Jean-Christophe Loiseau >>>> Homepage >>>> >>>> >>>> _______________________________________________ >>>> 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 Apr 14 10:17:24 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 14 Apr 2014 19:47:24 +0430 Subject: [Nek5000-users] Outlet boundary treatment Message-ID: Dear Neks, I want to simulate turbulent flow in a stenosis, and use outflow boundary condition at the outlet. Because of the possible backflow at the outlet in this case, I want to impose div U>0 at the last layer of the outlet. I have already seen an example in NEK5000 website (peris) which uses the same boundary condition as I want to impose. In this example, three subroutines are mentioned as the names of the following to apply this boundary condition: *fill_div(div)* *set_outflow_dist* *get_div_const(cdiv)* Now, I intend to use the same outlet B.C for a case the same as stenosis in pipe example. The both examples; pipe and peris, have similar geometries. So, may I use these subroutines exactly in the .usr file of stenosis case? or I should do any modification in this case. Thanks so much in advance. Omid -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Apr 14 10:26:06 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 14 Apr 2014 17:26:06 +0200 Subject: [Nek5000-users] Outlet boundary treatment In-Reply-To: References: Message-ID: Hi omid, To simulate turbulent flows, I guess you can use the sub routine turb_outflow(). Take a look at expansion.usr file in expansion example. Best,Kamal On 14/04/2014 17:17, nek5000-users at lists.mcs.anl.gov wrote: > Dear Neks, > > I want to simulate turbulent flow in a stenosis, and use outflow > boundary condition at the outlet. Because of the possible backflow at > the outlet in this case, I want to impose div U>0 at the last layer of > the outlet. > > I have already seen an example in NEK5000 website (peris) which uses > the same boundary condition as I want to impose. > In this example, three subroutines are mentioned as the names of the > following to apply this boundary condition: > *fill_div(div)* > *set_outflow_dist* > *get_div_const(cdiv)* > Now, I intend to use the same outlet B.C for a case the same as > stenosis in pipe example. The both examples; pipe and peris, have > similar geometries. So, may I use these subroutines exactly in the > .usr file of stenosis case? or I should do any modification in this case. > > Thanks so much in advance. > > Omid > > > _______________________________________________ > 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 Apr 14 15:39:05 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 14 Apr 2014 16:39:05 -0400 Subject: [Nek5000-users] Conjugate heat transfer problem In-Reply-To: References: Message-ID: Hi, Following your instruction, my case is running well and the result looks reasonable. I am curious about the meaning of p94. p94 in my previous case (only fluid) set to 3 and it works well. However it cannot work in conjugate problem with positive number. Is there any problem if I set p94 to zero for my previous case? Mu Xu On Mon, Mar 24, 2014 at 11:33 AM, wrote: > > Mu, > > Set p94 and 95 to zero. That will eliminate that issue. > > The result not being right is a separate issue. > > 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, March 24, 2014 10:20 AM > *To:* nek5000-users at lists.mcs.anl.gov > *Subject:* Re: [Nek5000-users] Conjugate heat transfer problem > > Hi, Andrea > > Thank you for your help. With your instruction, I can build a domain for > conjugate heat transfer problem now. However the problem is always crash in > the middle of running. I think the problem is during the Helmholtz solver > for velocity which is controlled by flag P94 in .rea file. Flag P95 > controls the Helmholtz solver for pressure. If I set both P94 and P95 to > zero, the case can run but the result is not right. If I set P94 to > positive integer and P95 to zero which is I used to, the case is crash. If > I set P95 to positive integer and P94 to zero, the case can run and the > result looks fine. I have never use this setting before. I want to know is > it fine to run the conjugate heat transfer problem with this setting which > is P94 to zero and P95 to positive integer. > > Mu Xu > > > On Fri, Mar 14, 2014 at 6:15 PM, wrote: > >> Hi Xu, >> >> in Conjugate Heat Transfer problems there is no boundary condition for >> the energy equation at the interface between fluid and solid. The interface >> behaves like the one of any other internal element, which means that the >> boundary is just marked with 'E '. >> I worked a lot with Conjugate Heat Transfer. If you need help don't >> hesitate to contact me. >> >> Cheers, >> Andrea. >> ________________________________ >> 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, March 14, 2014 7:22 PM >> To: nek5000-users at lists.mcs.anl.gov >> Subject: [Nek5000-users] Conjugate heat transfer problem >> >> Hi, Neks >> >> I want to set up a 3-D conjugate heat transfer problem. The procedure I >> used is as below: >> 1) generate a mesh for fluid domain. >> 2) generate a mesh for solid domain. >> 3)merge the element from 1) into 2). >> >> I have one question during the steps 1 and 2. What the boundary condition >> I need to set in step 1 and 2 at the interface between fluid and solid? >> >> Mu Xu >> _______________________________________________ >> 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 Sun Apr 13 20:16:49 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 14 Apr 2014 09:16:49 +0800 (GMT+08:00) Subject: [Nek5000-users] usr file - Vol 62, Issue 9 In-Reply-To: References: Message-ID: I just built a flow chart based on case expansion. I hope it useful for all beginner later. Zhenyu -----????----- ???: nek5000-users at lists.mcs.anl.gov ????: 2014-04-14 08:30:27 (???) ???: nek5000-users at lists.mcs.anl.gov ??: ??: Re: [Nek5000-users] usr file - Vol 62, Issue 9 Dear Murph, I carried on along your suggested way and at least got some expected results for case expanson. Thank you very much for your guidance. Yours, Zhenyu -----????----- ???:nek5000-users at lists.mcs.anl.gov ????: 2014-04-13 23:47:28 (???) ???:nek5000-users at lists.mcs.anl.gov ??: ??: Re: [Nek5000-users] usr file - Vol 62, Issue 9 Zhenyu, Hi... In general, you do the following: Use an existing run files as templates to start with. You need the .rea, SIZE, .box, and .usr files. Rename the rea,box, and usr files to a unique name for your run, like your_run.rea, your_run.box, your_run.usr. Edit the .box file to define your grid, geometry, and BCs. Edit the .rea file with all the basic run parameters. If you have an .rea template that is ascii (without the .re2 option) and it has geometry information at the end, ignore this information as it will be regenerated. Edit the SIZE file to set your array sizes and GLL DOF (this must also be set correctly in .rea). Edit the .usr file per instructions, including the information for boundary conditions if applicable. Then, you generate a new .rea file with the grid geometry by running genbox: "genbox ./your_run.box". This will create the files box.rea and box.tmp. You rename box.rea to your_run.rea. This will overwrite the one you edited with a new one with all your changes in the settings sections intact, and new geometry information at the end. Delete box.tmp. Next, you run genmap to create a new map file: "genmap ./your_run". This will create the new map file. Next, compile the code with: "./makenek ./your_run". If successful, you will get a new binary copy of nek5000. Then you run with one of the scripts like: "./nekbmpi ./your_run 24" You will probably get a lot of errors initially based on improper makenek setting for your compiler and target platform, geometry issues, etc... Read all the documentation and look at the examples to figure this stuff out for your application... See Ya, Murph mlodea at oakland.edu ForwardedMessage.eml | Subject: [Nek5000-users] How to create .usr file | | From: nek5000-users at lists.mcs.anl.gov | | Date: 4/10/2014 10:49 AM | | To: Nek5000-users at lists.mcs.anl.gov | Dear All, I am trying nek5000 under ubuntu. As a beginner, I just wonder which is the best way to create the .usr file, should I copy one from the examples and change it for my case or use a tool just like genbox, genmap, etc. to generate it? I have the same question for creation of SIZE By the way, I can only find the usage of prenek and demonstrative cases from the old manual of nekton, what is the current way of generating meshes for public uses? Thank you very much in advance. Zhenyu ForwardedMessage.eml | Subject: Re: [Nek5000-users] How to create .usr file | | From: nek5000-users at lists.mcs.anl.gov | | Date: 4/9/2014 11:17 AM | | To: nek5000-users at lists.mcs.anl.gov | Hi Zhenyu, The *.usr is to be copied from the examples and change it according to your needs like Boundary condition and Initial condition. The SIZE file too should be copied (change the number of element per processor according to yours) . See the example 'Expansion ' --> mkmesh file, which will give you an insight about how to write a script to create a mesh using prenek. Best Regards, Kamal. On 10/04/2014 16:49, nek5000-users at lists.mcs.anl.gov wrote: Dear All, I am trying nek5000 under ubuntu. As a beginner, I just wonder which is the best way to create the .usr file, should I copy one from the examples and change it for my case or use a tool just like genbox, genmap, etc. to generate it? I have the same question for creation of SIZE By the way, I can only find the usage of prenek and demonstrative cases from the old manual of nekton, what is the current way of generating meshes for public uses? Thank you very much in advance. Zhenyu _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.govhttps://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.govhttps://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: -------------- next part -------------- A non-text attachment was scrubbed... Name: nek-case-flow-chart.pdf Type: application/pdf Size: 66590 bytes Desc: not available URL: From nek5000-users at lists.mcs.anl.gov Mon Apr 21 18:12:07 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 21 Apr 2014 19:12:07 -0400 Subject: [Nek5000-users] Internal boundary condition Message-ID: Dear all, I have a question regarding the internal boundary condition in the code. My problem consists of a fan-shaped nozzle, which parts of its walls are located within the flow domain (a cylindrical tank with inflow/ outflow boundary conditions). The question is how to set the boundary conditions for such internal zero-thickness walls? I thought the walls could be defined as internal faces by creating a side-set (in the Cubit) and setting the velocity and the temperature fields of these faces to 'W ' and 'E ', respectively, similar to the solid-fluid interface in the conjugate heat transfer example. Nevertheless, there is a fluid at both sides of the interface in this case. Below is part of the boundary conditions in .rea file. ..... ..... 1 0 ! 1 fluid set, 0 other/solid sets 10 ! fluid set is 10 1 ! block 10 is material 1 10 ! no. bc sets (side-sets); bc set id, 100 1 W , (external walls) 100 2 I , (external walls) 120 1 W , (internal walls corresponding to the nozzle) 120 2 E , (internal walls corresponding to the nozzle) 200 1 v , (inflow) 200 2 t , (inflow) 300 1 O , (outflow) 300 2 O , (outflow) 400 1 SYM, 400 2 SYM, ..... ..... When I run this case, warning messages appear during assigning the sidesets to the element faces, saying that: "face shared by 2 Hexes (say) 2331 5227". It seems that this warning is only because I defined some faces as "internal", however, no "other solid/fluids" has been defined in the input file. Nevertheless, the issue with such definition is that, although, the velocity field is zero at the internal walls, there seems to be a pressure gradient across the wall, which is not physically consistent with internal walls, and drives a flow through the walls. It would be appreciated if anyone could help me on this problem. Thanks, Mohsen -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Apr 21 19:00:44 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 22 Apr 2014 00:00:44 +0000 Subject: [Nek5000-users] Internal boundary condition In-Reply-To: References: Message-ID: Dear Mohsen, Years ago we did support internal walls, but that's no longer the case with the current workflow. The issue is that the gridpoints across the interface are identified as being one and the same if they are physically adjacent. It would be possible to hack into your vertex numbering to make these different (i.e., after they are generated by genmap), or to make a geometry in which they are distinct by having a finite-thickness wall, but either way requires some application specific coding in your usr file or modifications to your map 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: Monday, April 21, 2014 6:12 PM To: Nek 5000 Subject: [Nek5000-users] Internal boundary condition Dear all, I have a question regarding the internal boundary condition in the code. My problem consists of a fan-shaped nozzle, which parts of its walls are located within the flow domain (a cylindrical tank with inflow/outflow boundary conditions). The question is how to set the boundary conditions for such internal zero-thickness walls? I thought the walls could be defined as internal faces by creating a side-set (in the Cubit) and setting the velocity and the temperature fields of these faces to 'W ' and 'E ', respectively, similar to the solid-fluid interface in the conjugate heat transfer example. Nevertheless, there is a fluid at both sides of the interface in this case. Below is part of the boundary conditions in .rea file. ..... ..... 1 0 ! 1 fluid set, 0 other/solid sets 10 ! fluid set is 10 1 ! block 10 is material 1 10 ! no. bc sets (side-sets); bc set id, 100 1 W , (external walls) 100 2 I , (external walls) 120 1 W , (internal walls corresponding to the nozzle) *** * * * (internal walls corresponding to the nozzle) 200 1 v , (inflow) 200 2 t , (inflow) 300 1 O , (outflow) 300 2 O , (outflow) 400 1 SYM, 400 2 SYM, ..... ..... When I run this case, warning messages appear during assigning the sidesets to the element faces, saying that: "face shared by 2 Hexes (say) 2331 5227". It seems that this warning is only because I defined some faces as "internal", however, no "other solid/fluids" has been defined in the input file. Nevertheless, the issue with such definition is that, although, the velocity field is zero at the internal walls, there seems to be a pressure gradient across the wall, which is not physically consistent with internal walls, and drives a flow through the walls. It would be appreciated if anyone could help me on this problem. Thanks, Mohsen -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Apr 22 03:19:26 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 22 Apr 2014 13:49:26 +0530 Subject: [Nek5000-users] State space representation Message-ID: Hello neks Are there any examples which show how to obtain the state space representation of linearized navier-stokes, i.e., of the form M dx/dt = Ax + Bu where x = (velocity, pressure) and u represents some boundary control, e.g., blowing/suction. I would need to save these matrices M, A, B to a file, import into matlab and do some computations. My problem at present is not very big and in 2d only. Thanks praveen -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Apr 22 09:19:41 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 22 Apr 2014 10:19:41 -0400 Subject: [Nek5000-users] Internal boundary condition In-Reply-To: References: Message-ID: Thanks Paul! I am also thinking of having a precursor simulation of flow inside nozzle and therefore, replacing it with a prescribed inflow BC. Mohsen On 21-Apr-14, at 8:00 PM, wrote: > > Dear Mohsen, > > Years ago we did support internal walls, but that's no longer the > case with the current workflow. > > The issue is that the gridpoints across the interface are > identified as being one and the same if > they are physically adjacent. It would be possible to hack into > your vertex numbering to make > these different (i.e., after they are generated by genmap), or to > make a geometry in which they > are distinct by having a finite-thickness wall, but either way > requires some application specific > coding in your usr file or modifications to your map 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: Monday, April 21, 2014 6:12 PM > To: Nek 5000 > Subject: [Nek5000-users] Internal boundary condition > > Dear all, > I have a question regarding the internal boundary condition in the > code. > My problem consists of a fan-shaped nozzle, which parts of its > walls are located within the flow domain (a cylindrical tank with > inflow/outflow boundary conditions). The question is how to set the > boundary conditions for such internal zero-thickness walls? > > I thought the walls could be defined as internal faces by creating > a side-set (in the Cubit) and setting the velocity and the > temperature fields of these faces to 'W ' and 'E ', respectively, > similar to the solid-fluid interface in the conjugate heat > transfer example. Nevertheless, there is a fluid at both sides of > the interface in this case. > Below is part of the boundary conditions in .rea file. > ..... > ..... > 1 0 ! 1 fluid set, 0 other/solid sets > 10 ! fluid set is 10 > 1 ! block 10 is material 1 > 10 ! no. bc sets (side-sets); bc set id, > 100 1 W , (external walls) > 100 2 I , (external walls) > 120 1 W , (internal walls corresponding to the nozzle) > 120 2 E , (internal walls corresponding to the nozzle) > 200 1 v , (inflow) > 200 2 t , (inflow) > 300 1 O , (outflow) > 300 2 O , (outflow) > 400 1 SYM, > 400 2 SYM, > ..... > ..... > > When I run this case, warning messages appear during assigning the > sidesets to the element faces, saying that: "face shared by 2 Hexes > (say) 2331 5227". It seems that this warning is only because I > defined some faces as "internal", however, no "other solid/fluids" > has been defined in the input file. > Nevertheless, the issue with such definition is that, although, the > velocity field is zero at the internal walls, there seems to be a > pressure gradient across the wall, which is not physically > consistent with internal walls, and drives a flow through the walls. > > It would be appreciated if anyone could help me on this problem. > > Thanks, > Mohsen > > _______________________________________________ > 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 Apr 23 23:31:29 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 24 Apr 2014 10:01:29 +0530 Subject: [Nek5000-users] Setting viscosity in usr file Message-ID: Hello neks Which is the place to set viscosity (param(2)) in the usr file ? In example fs_2, it is done in usrdat2, but the param seems to be read after usrdat2 is called. Thanks praveen -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Apr 24 00:28:52 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 24 Apr 2014 13:28:52 +0800 (GMT+08:00) Subject: [Nek5000-users] Prex problem Message-ID: Dear All, I am trying nek5000 under ubuntu. Now I adapted mkmesh from case expansion for my own case, which is a flat plane boundary layer with a slot. I build one box for the jet slot and 23 boxes for the plane wall around it (mbox in SIZE of genbox.f was changed for it). Now when I use pretex to merge both 2d mesh together, pretex show no picture for the mesh (but just an empty menubar and a black window, no errors shown) then I cannot assign properly B.C. for the boundaries. Could anyone give any hints? Thank you very much in advance. If you need, I can send the setup files to you. Zhenyu Zhang -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Apr 24 01:37:19 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 24 Apr 2014 08:37:19 +0200 Subject: [Nek5000-users] Setting viscosity in usr file Message-ID: Hello Praveen, Try to set parameter 'udiff' for field 1 ('ifield.eq.1', i.e. velocity field) in subroutine uservp. Param(30) in .rea file has to be equal to 1.. Regards, Donato From: nek5000-users-bounces at lists.mcs.anl.gov [mailto:nek5000-users-bounces at lists.mcs.anl.gov] On Behalf Of nek5000-users at lists.mcs.anl.gov Sent: 24 April 2014 06:31 To: nek5000 Subject: [Nek5000-users] Setting viscosity in usr file Hello neks Which is the place to set viscosity (param(2)) in the usr file ? In example fs_2, it is done in usrdat2, but the param seems to be read after usrdat2 is called. Thanks praveen -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Apr 24 06:23:00 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 24 Apr 2014 19:23:00 +0800 (GMT+08:00) Subject: [Nek5000-users] Multiple velocity inlets Message-ID: Hi, Does nek5000 now support boundary conditions for multiple velocity inlets? I am really interested in esp. two or more inlets with unsteady velocities. Cheers, Zhenyu -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Apr 24 06:43:31 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 24 Apr 2014 11:43:31 +0000 Subject: [Nek5000-users] Multiple velocity inlets In-Reply-To: References: Message-ID: Hi Zhenyu, Yes, as a long as you have a singly connected fluid domain. One way is to use coordinates to differentiate between the inlets. 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: Thursday, April 24, 2014 6:23 AM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] Multiple velocity inlets Hi, Does nek5000 now support boundary conditions for multiple velocity inlets? I am really interested in esp. two or more inlets with unsteady velocities. Cheers, Zhenyu -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Apr 24 06:34:16 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 24 Apr 2014 19:34:16 +0800 (GMT+08:00) Subject: [Nek5000-users] Multiple velocity inlets In-Reply-To: References: Message-ID: Dear Aleks, I 'd like to simulate a laminar bounary layer with a mini slot jet. Do you mean I have to use a if...else... block in userbc to set the local inlet velocity? Zhenyu -----????----- ???: nek5000-users at lists.mcs.anl.gov ????: 2014-04-24 19:43:31 (???) ???: "nek5000-users at lists.mcs.anl.gov" ??: ??: Re: [Nek5000-users] Multiple velocity inlets Hi Zhenyu, Yes, as a long as you have a singly connected fluid domain. One way is to use coordinates to differentiate between the inlets. 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: Thursday, April 24, 2014 6:23 AM To:nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] Multiple velocity inlets Hi, Does nek5000 now support boundary conditions for multiple velocity inlets? I am really interested in esp. two or more inlets with unsteady velocities. Cheers, Zhenyu -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Apr 24 10:00:19 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 24 Apr 2014 20:30:19 +0530 Subject: [Nek5000-users] Setting viscosity in usr file In-Reply-To: References: Message-ID: On Thu, Apr 24, 2014 at 12:07 PM, wrote: > Hello Praveen, > > > > Try to set parameter 'udiff' for field 1 ('ifield.eq.1', i.e. velocity > field) in subroutine uservp. > > Param(30) in .rea file has to be equal to 1.. > > > > Regards, > > Donato > Thanks Donato. I know this method. My viscosity is a constant, so I want to set it just once. I have done it in usrdat2 and it seems to work, but wanted to confirm that it is the right place to set a constant viscosity. I do the following in usrdat2 param(2) = 1.0/1000.0 cpfld(1,1) = param(2) Best praveen -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Apr 24 13:47:30 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 24 Apr 2014 13:47:30 -0500 Subject: [Nek5000-users] Prex problem In-Reply-To: References: Message-ID: Hi, Are you using pretex or prex? pretex doesn't have a gui associated with it, so you must use the terminal menu to make changes to your mesh. If you want the graphical interface, you would want prex Katherine On Thu, Apr 24, 2014 at 12:28 AM, wrote: > Dear All, > > I am trying nek5000 under ubuntu. Now I adapted mkmesh from case > expansion for my own case, which is a flat plane boundary layer with a slot. > > I build one box for the jet slot and 23 boxes for the plane wall around it > (mbox in SIZE of genbox.f was changed for it). Now when I use pretex to > merge both 2d mesh together, pretex show no picture for the mesh (but just > an empty menubar and a black window, no errors shown) then I cannot assign > properly B.C. for the boundaries. > > Could anyone give any hints? Thank you very much in advance. > > If you need, I can send the setup files to you. > > > Zhenyu Zhang > _______________________________________________ > 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 Apr 24 18:53:38 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 25 Apr 2014 07:53:38 +0800 (GMT+08:00) Subject: [Nek5000-users] Prex problem In-Reply-To: References: Message-ID: Dear Katherine, Thank you for the reply and sorry for the unclear description in last email. I tried both actually. For pretex, somtimes I have to give proper BC type for shown element no. and face index. Yes I can set them up once I checked the element corner list in .rea file according to their numbers. But I hate to say it is rally clumsy esp. when there are tens or even higher numbers of boundary elements to set. This is why I also tried prex, and then I got the problem I showed in last email. A black window without showing the topology of my mesh looks strange, since there are no X11 compatibility problem (I am using Ubuntu 13.10 & 14.04). Meanwhile, I can show the mesh by opening a .rea file from postx, but you know I cannot set BCs there. Best regards, Zhenyu -----????----- ???: nek5000-users at lists.mcs.anl.gov ????: 2014-04-25 02:47:30 (???) ???: nek5000-users at lists.mcs.anl.gov ??: ??: Re: [Nek5000-users] Prex problem Hi, Are you using pretex or prex? pretex doesn't have a gui associated with it, so you must use the terminal menu to make changes to your mesh. If you want the graphical interface, you would want prex Katherine On Thu, Apr 24, 2014 at 12:28 AM, wrote: Dear All, I am trying nek5000 under ubuntu. Now I adapted mkmesh from case expansion for my own case, which is a flat plane boundary layer with a slot. I build one box for the jet slot and 23 boxes for the plane wall around it (mbox in SIZE of genbox.f was changed for it). Now when I use pretex to merge both 2d mesh together, pretex show no picture for the mesh (but just an empty menubar and a black window, no errors shown) then I cannot assign properly B.C. for the boundaries. Could anyone give any hints? Thank you very much in advance. If you need, I can send the setup files to you. Zhenyu Zhang _______________________________________________ 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 Apr 24 19:01:39 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 25 Apr 2014 08:01:39 +0800 (GMT+08:00) Subject: [Nek5000-users] Question on drawing streamlines for Nek5000 data Message-ID: Dear All, I am sorry to launch this question about VisIt here. I submitted it in visit-user.org. But it seems nobody there uses Nek5000. So may I ask any help from you. I tried to use Visit 2.7.2 to draw streamlines for a flow field through a backward step from Nek5000. Parameters in Visit: step length: 0.1 (size of my mesh between 0.05 and 0.2) max steps: 10000 source type: line (1 -0.99 1.5) to (1 0.99 1.5) (this line is well inside the flow field down stream of the step (at x=0)) 50 sample along line uniformly integration: forward scheme: Forward Euler (default Dromand-Prince diverged ) Now the questions is: 1. Only part of the line is positioned with seeds. part of the line is blank with No streamlines at all. 2. According to Visit user manual, step length should agree with average size of mesh, in my case even I reduce the step to 0.01. The integration is broken . 3. To my knowledge, RK4 is good for its stability. But in this case it cannot even give a good result . However, the 1st -order forward Euler can be used. don't know why yet. 4. Generally before visualizing spectral element results, interpolation is necessary a priori. Sorry I did not do this work here just for simplicity, so the accuracy of streamline may not be quite good. But I don't think this broke the streamline generation. 5. There is a laminar separation vortex just downstream (about x=2) of the seeding line (x=1), if I want to plot the stream lines across the whole flow field, could you please leave me any hints to do that? In fact, what ever the max steps is set, my streamline seems never extend up to x=1.3 6. Is it possible to introduce adaptive local time step for streamline production? this tech. is quite well known for steady CFD problems. If you need , I can upload a picture later to show above questions. I'll appreciate any hints from you. Zhenyu Zhang -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Fri Apr 25 10:00:00 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 25 Apr 2014 17:00:00 +0200 Subject: [Nek5000-users] Rules of thumb for element aspect ratio limits Message-ID: Hello, I am looking to do simulations of flow past a wing in 3D using nek5000 and I have been thinking more about potential issues with high aspect ratio elements. In general we have very fine resolution near the wing and then as we get further away the wall normal and wall parallel spacing increases. As a first try we will extend the domain in the cross stream direction which will result in small dz values. I know that in general the best performance is obtained with elements having dx=dy=dz and that as the aspect ratio increases the performance will degrade. I'm wondering if there are general rules of thumb for the performance degradation with increased aspect ratio. For example, is an aspect ratio of 10 ok but an aspect ratio of 100 unacceptable? Is this even something we can estimate in general or does it vary so much problem to problem that no general estimate is possible? I saw an earlier post that referred to the paper "An Overlapping Schwarz Method for Spectral Element Solution of the Incompressible Navier-Stokes Equations", P. Fischer JCP 1997. From the paper I see two general strategies. 1. limit the maximum aspect ratio to a critical value 2. design a grid for our case, run it for a short time and then iteratively add more grid points to decrease the aspect ratio until optimal performance is achieved. Does anyone have a general or specific suggestion regarding how we should handle the grid generation in terms of selecting the largest aspect ratio possible with low computational cost? Thanks, Matt -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Fri Apr 25 11:02:13 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 25 Apr 2014 18:02:13 +0200 Subject: [Nek5000-users] Rules of thumb for element aspect ratio limits In-Reply-To: References: Message-ID: ?HI Matt, Till now I have no experiments on 3D problem, what I am interested in is how you generate the 3D or 2D airfoil mesh for nek5000? I spend 2 weeks in generated a 2d airfoil flow mesh without any good results. would you like tell me some informations? thank you a lot! Wei 2014-04-25 17:00 GMT+02:00 : > Hello, > > I am looking to do simulations of flow past a wing in 3D using nek5000 and > I have been thinking more about potential issues with high aspect ratio > elements. In general we have very fine resolution near the wing and then as > we get further away the wall normal and wall parallel spacing increases. As > a first try we will extend the domain in the cross stream direction which > will result in small dz values. I know that in general the best performance > is obtained with elements having dx=dy=dz and that as the aspect ratio > increases the performance will degrade. > > I'm wondering if there are general rules of thumb for the performance > degradation with increased aspect ratio. For example, is an aspect ratio of > 10 ok but an aspect ratio of 100 unacceptable? Is this even something we > can estimate in general or does it vary so much problem to problem that no > general estimate is possible? > > I saw an earlier post that referred to the paper "An Overlapping Schwarz > Method for Spectral Element Solution of the Incompressible Navier-Stokes > Equations", P. Fischer JCP 1997. From the paper I see two general > strategies. > 1. limit the maximum aspect ratio to a critical value > 2. design a grid for our case, run it for a short time and then > iteratively add more grid points to decrease the aspect ratio until optimal > performance is achieved. > > Does anyone have a general or specific suggestion regarding how we should > handle the grid generation in terms of selecting the largest aspect ratio > possible with low computational cost? > > Thanks, > > Matt > > _______________________________________________ > 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 Apr 25 15:17:03 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 25 Apr 2014 22:17:03 +0200 Subject: [Nek5000-users] Rules of thumb for element aspect ratio limits In-Reply-To: References: Message-ID: Hi matt, Sorry that I cannot fully answer your question, I know that at least the smallest edge length in the mesh is a measure for the stiffness of the full problem, so maybe you should avoid too small element heights in the boundary layer. However, I also would like to know how you are generating the airfoil mesh, since the mesh has to be coarser than a standard meshes and the boundary layer elements need to have curved boundaries, no? Which mesh generator you use and how do you convert the mesh to Nek format? The 3d problem should boil down to a 2d problem, since I assume that you want simulate a small part of the wing with periodic boundary conditions in spanwise direction... But wei, for the 2d mesh, did you resolve the issue to curve the boundary layer elements? Florian > Am 25.04.2014 um 18:02 schrieb nek5000-users at lists.mcs.anl.gov: > > ?HI Matt, > > Till now I have no experiments on 3D problem, what I am interested in is how you generate the 3D or 2D airfoil mesh for nek5000? I spend 2 weeks in generated a 2d airfoil flow mesh without any good results. would you like tell me some informations? thank you a lot! > > Wei > > > 2014-04-25 17:00 GMT+02:00 : >> Hello, >> >> I am looking to do simulations of flow past a wing in 3D using nek5000 and I have been thinking more about potential issues with high aspect ratio elements. In general we have very fine resolution near the wing and then as we get further away the wall normal and wall parallel spacing increases. As a first try we will extend the domain in the cross stream direction which will result in small dz values. I know that in general the best performance is obtained with elements having dx=dy=dz and that as the aspect ratio increases the performance will degrade. >> >> I'm wondering if there are general rules of thumb for the performance degradation with increased aspect ratio. For example, is an aspect ratio of 10 ok but an aspect ratio of 100 unacceptable? Is this even something we can estimate in general or does it vary so much problem to problem that no general estimate is possible? >> >> I saw an earlier post that referred to the paper "An Overlapping Schwarz Method for Spectral Element Solution of the Incompressible Navier-Stokes Equations", P. Fischer JCP 1997. From the paper I see two general strategies. >> 1. limit the maximum aspect ratio to a critical value >> 2. design a grid for our case, run it for a short time and then iteratively add more grid points to decrease the aspect ratio until optimal performance is achieved. >> >> Does anyone have a general or specific suggestion regarding how we should handle the grid generation in terms of selecting the largest aspect ratio possible with low computational cost? >> >> Thanks, >> >> Matt >> >> _______________________________________________ >> 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 Apr 25 17:02:06 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 25 Apr 2014 17:02:06 -0500 Subject: [Nek5000-users] Prex problem In-Reply-To: References: Message-ID: Thanks for the clarification. To be sure I understand, when you open prex from your terminal, the viewing frame appears,and you can start the session ok (choosing a name for the session, clicking read previous parameters...etc)? Or does the viewing frame appear blank and there is no text in the terminal log? If you can start the session but not load the files, please send me the stdout on the terminal of the session. (send off list to heisey at anl.gov) If you cannot even start the session, you should check where X11 is installed and that the path is set correctly in the prenek/makefile. Best, Katherine On Thu, Apr 24, 2014 at 6:53 PM, wrote: > Dear Katherine, > > Thank you for the reply and sorry for the unclear description in last > email. > > I tried both actually. For pretex, somtimes I have to give proper BC type > for shown element no. and face index. Yes I can set them up once I checked > the element corner list in .rea file according to their numbers. But I hate > to say it is rally clumsy esp. when there are tens or even higher numbers > of boundary elements to set. > > This is why I also tried prex, and then I got the problem I showed in last > email. A black window without showing the topology of my mesh looks > strange, since there are no X11 compatibility problem (I am using Ubuntu > 13.10 & 14.04). Meanwhile, I can show the mesh by opening a .rea file from > postx, but you know I cannot set BCs there. > > Best regards, > > > Zhenyu > > -----????----- > *???:* nek5000-users at lists.mcs.anl.gov > *????:* 2014-04-25 02:47:30 (???) > *???:* nek5000-users at lists.mcs.anl.gov > *??:* > *??:* Re: [Nek5000-users] Prex problem > > > Hi, > > Are you using pretex or prex? pretex doesn't have a gui associated with > it, so you must use the terminal menu to make changes to your mesh. If you > want the graphical interface, you would want prex > > Katherine > > > > On Thu, Apr 24, 2014 at 12:28 AM, wrote: > >> Dear All, >> >> I am trying nek5000 under ubuntu. Now I adapted mkmesh from case >> expansion for my own case, which is a flat plane boundary layer with a slot. >> >> I build one box for the jet slot and 23 boxes for the plane wall around >> it (mbox in SIZE of genbox.f was changed for it). Now when I use pretex to >> merge both 2d mesh together, pretex show no picture for the mesh (but just >> an empty menubar and a black window, no errors shown) then I cannot assign >> properly B.C. for the boundaries. >> >> Could anyone give any hints? Thank you very much in advance. >> >> If you need, I can send the setup files to you. >> >> >> Zhenyu Zhang >> _______________________________________________ >> 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 Apr 28 03:38:10 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 28 Apr 2014 10:38:10 +0200 Subject: [Nek5000-users] Rules of thumb for element aspect ratio limits In-Reply-To: References: Message-ID: Hi Florian, For the 2D airfoil profile, I guess, the profile in nek5000 is connected by small straight lines not the curved lines. But even this, I have no idea to make a mesh for 2d airfoil flow. in the Genbox introduction there is something words on segments mesh without a sample For Multiple Segmented Geometries This feature allows users to enter a complex sequence of segments for each of the x,y,z directions. Each segment set is defined in x,y,z sections. So, Lines 6-8 would all pertain to x-dimension, 9-12 to y-dimension, ect. Line 5: The line following the string name, is the number of segments, nsegs, in the x_direction Line 6: The next line is the number of elements in each segment, so there should be nsegs numbers. (nelx_1,nelx_2...) Line 7: The next line is the start(and end) coordinates for each segment in this direction. There should be nsegs+1. (x(0),x(1)...x(nsegs)) Line 8: The following line is the distribution of each segment, uniform spacing corresponds to 1, otherwise a geometric sequence is generated. -In conclusion, a segment between x(e-1) and x(e) is filled with nelx_e elements determined by the geometric ratio given for that segment. Repeat (Lines 5-8) for dimensions 2 and, if applicable, 3. can anyone give us a sample? regards Wei On Apr 25, 2014, at 10:17 PM, nek5000-users at lists.mcs.anl.gov wrote: > Hi matt, > Sorry that I cannot fully answer your question, I know that at least the smallest edge length in the mesh is a measure for the stiffness of the full problem, so maybe you should avoid too small element heights in the boundary layer. > However, I also would like to know how you are generating the airfoil mesh, since the mesh has to be coarser than a standard meshes and the boundary layer elements need to have curved boundaries, no? Which mesh generator you use and how do you convert the mesh to Nek format? > The 3d problem should boil down to a 2d problem, since I assume that you want simulate a small part of the wing with periodic boundary conditions in spanwise direction... But wei, for the 2d mesh, did you resolve the issue to curve the boundary layer elements? > > Florian > > Am 25.04.2014 um 18:02 schrieb nek5000-users at lists.mcs.anl.gov: > >> ?HI Matt, >> >> Till now I have no experiments on 3D problem, what I am interested in is how you generate the 3D or 2D airfoil mesh for nek5000? I spend 2 weeks in generated a 2d airfoil flow mesh without any good results. would you like tell me some informations? thank you a lot! >> >> Wei >> >> >> 2014-04-25 17:00 GMT+02:00 : >> Hello, >> >> I am looking to do simulations of flow past a wing in 3D using nek5000 and I have been thinking more about potential issues with high aspect ratio elements. In general we have very fine resolution near the wing and then as we get further away the wall normal and wall parallel spacing increases. As a first try we will extend the domain in the cross stream direction which will result in small dz values. I know that in general the best performance is obtained with elements having dx=dy=dz and that as the aspect ratio increases the performance will degrade. >> >> I'm wondering if there are general rules of thumb for the performance degradation with increased aspect ratio. For example, is an aspect ratio of 10 ok but an aspect ratio of 100 unacceptable? Is this even something we can estimate in general or does it vary so much problem to problem that no general estimate is possible? >> >> I saw an earlier post that referred to the paper "An Overlapping Schwarz Method for Spectral Element Solution of the Incompressible Navier-Stokes Equations", P. Fischer JCP 1997. From the paper I see two general strategies. >> 1. limit the maximum aspect ratio to a critical value >> 2. design a grid for our case, run it for a short time and then iteratively add more grid points to decrease the aspect ratio until optimal performance is achieved. >> >> Does anyone have a general or specific suggestion regarding how we should handle the grid generation in terms of selecting the largest aspect ratio possible with low computational cost? >> >> Thanks, >> >> Matt >> >> _______________________________________________ >> 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 Apr 28 05:16:17 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 28 Apr 2014 12:16:17 +0200 Subject: [Nek5000-users] Rules of thumb for element aspect ratio limits In-Reply-To: References: Message-ID: Hi Wei and Florian, In general you can first generate a 2D grid for flow past a wing if it is a straight wing (of if you represent the 3 dimensionality by a forcing in the z direction to indicate a fixed sweep angle). This is not optimal though for a larger problem even if you have periodic boundary conditions because your dz spacing will be fixed at a small value by the BL region requirements. For DNS of the boundary layer region close to the wing you generally want dx+~10 dy+ ~ 0.5 next to the wall, less than dz+ away from the wall dz+ ~ dx+/2 This gives a maximum aspect ratio of about 20 near the wall (dx/dz). In the wake / separated flow region you generally want max(dx,dy,dz)/eta < 4 where eta is the kolmogorov lengthscale. The problem is that with a wake calculation such as an airofil you generally also want the boundaries to be far away. You can do this by growing dx and dy away from the airfoil. However, you will eventually reach a point where your aspect ratio is 10-1,000 far away from the wing as well since dz is small. The problem with doing this is that when you are far away from the wing then dz will still be very small. With a structured mesh there appears to be no way to fix this issue without a multiblock method. For an unstructured mesh there is a possibility of coarsening more in all 3 directions but this is quite challenging to generate. Also, it is not as simple as just thinking about the maximum value of (dx,dy,dz) divided by the minimum value of (dx,dy,dz). The relative ratios of dx,dy,dz all matter and with a wake you generally have regions where you have all 6 cases of dx < dy < dz dx < dz < dy, dy < dx < dz dy < dz < dx dz < dx < dy dz < dy < dx All these areas create problems for an iterative solver. You can write a more robust / complex solver (such as a semi-coarsening multigrid algorithm) to handle these different aspect ratio regions but then much more work is required per iteration. It is a trade-off between # of iterations required and computing time per iteration. For generating the mesh itself. We have an inhouse generated method based on gridgen-c. https://code.google.com/p/gridgen-c/ . It is not ideal but it can be made to work. We also looked into using cubit for unstructured meshes but we are still testing that. With cubit you can either use moab to load in the mesh to nek but then you have some limitations. For both options you can write your own converter as well... we do this for now. To curve the boundary layer elements we first generate the element locations themselves and then the GLL points are created on straight line segments. We go back in and manually correct the location of the GLL points located closest to the wall using a spline of the wing. Then we solve a laplace equation to smooth out the GLL points in the rest of the domain. Matt On Fri, Apr 25, 2014 at 10:17 PM, wrote: > Hi matt, > Sorry that I cannot fully answer your question, I know that at least the > smallest edge length in the mesh is a measure for the stiffness of the > full problem, so maybe you should avoid too small element heights in the > boundary layer. > However, I also would like to know how you are generating the airfoil > mesh, since the mesh has to be coarser than a standard meshes and the > boundary layer elements need to have curved boundaries, no? Which mesh > generator you use and how do you convert the mesh to Nek format? > The 3d problem should boil down to a 2d problem, since I assume that you > want simulate a small part of the wing with periodic boundary conditions in > spanwise direction... But wei, for the 2d mesh, did you resolve the issue > to curve the boundary layer elements? > > Florian > > Am 25.04.2014 um 18:02 schrieb nek5000-users at lists.mcs.anl.gov: > > ?HI Matt, > > Till now I have no experiments on 3D problem, what I am interested in is > how you generate the 3D or 2D airfoil mesh for nek5000? I spend 2 weeks in > generated a 2d airfoil flow mesh without any good results. would you like > tell me some informations? thank you a lot! > > Wei > > > 2014-04-25 17:00 GMT+02:00 : > >> Hello, >> >> I am looking to do simulations of flow past a wing in 3D using nek5000 >> and I have been thinking more about potential issues with high aspect ratio >> elements. In general we have very fine resolution near the wing and then as >> we get further away the wall normal and wall parallel spacing increases. As >> a first try we will extend the domain in the cross stream direction which >> will result in small dz values. I know that in general the best performance >> is obtained with elements having dx=dy=dz and that as the aspect ratio >> increases the performance will degrade. >> >> I'm wondering if there are general rules of thumb for the performance >> degradation with increased aspect ratio. For example, is an aspect ratio of >> 10 ok but an aspect ratio of 100 unacceptable? Is this even something we >> can estimate in general or does it vary so much problem to problem that no >> general estimate is possible? >> >> I saw an earlier post that referred to the paper "An Overlapping Schwarz >> Method for Spectral Element Solution of the Incompressible Navier-Stokes >> Equations", P. Fischer JCP 1997. From the paper I see two general >> strategies. >> 1. limit the maximum aspect ratio to a critical value >> 2. design a grid for our case, run it for a short time and then >> iteratively add more grid points to decrease the aspect ratio until optimal >> performance is achieved. >> >> Does anyone have a general or specific suggestion regarding how we should >> handle the grid generation in terms of selecting the largest aspect ratio >> possible with low computational cost? >> >> Thanks, >> >> Matt >> >> _______________________________________________ >> 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 Apr 28 05:20:12 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 28 Apr 2014 12:20:12 +0200 Subject: [Nek5000-users] Rules of thumb for element aspect ratio limits In-Reply-To: References: Message-ID: Hi Wei, I don't think genbox is the right tool to mesh airfoils, just because you need the curved elements for high order computations. We are using high order meshes for discontinuous Galerkin schemes. One technique is to construct them from agglomeration of fine structured grids (ICEM, Poitwise, Gridgen...), leading to coarse grids with the intermediate points used for the curved element mapping. But then I really don't know how this fits into the nek mesh format, since I think there is no possibility to define intermediate interpolation points for the elements. The only thing I saw is to prescribe a curvature of an edge, but I think this is restricted to 2D meshes and circular geometries, no? Our workaround for an airfoil computation was more or less a hack directly in Nek, where we read Gauss-Lobatto high order points of the elements from file (we produced ourselves, together with the Nek format with linear edges) and replaced (overwrote) the linear elements with the curved ones during grid setup. Maybe somebody knows a better way to do this... regards Florian Am 28.04.2014 10:38, schrieb nek5000-users at lists.mcs.anl.gov: > Hi Florian, > > For the 2D airfoil profile, I guess, the profile in nek5000 is > connected by small straight lines not the curved lines. But even this, > I have no idea to make a mesh for 2d airfoil flow. in the Genbox > introduction there is something words on segments mesh without a sample > > > For Multiple Segmented Geometries > > * This feature allows users to enter a complex sequence of segments > for each of the x,y,z directions. > * Each segment set is defined in x,y,z sections. So, Lines 6-8 would > all pertain to x-dimension, 9-12 to y-dimension, ect. > > *Line 5:* The line following the string name, is the number of > segments, /nsegs/, in the x_direction > *Line 6:* The next line is the number of elements in each segment, so > there should be /nsegs/ numbers. (nelx_1,nelx_2...) > *Line 7:* The next line is the start(and end) coordinates for each > segment in this direction. There should be /nsegs/+1. > (x(0),x(1)...x(nsegs)) > *Line 8:* The following line is the distribution of each segment, > uniform spacing corresponds to 1, otherwise a geometric sequence is > generated. > > -In conclusion, a segment between x(e-1) and x(e) is filled with > nelx_e elements determined by the geometric ratio given for that > segment. > > * Repeat (Lines 5-8) for dimensions 2 and, if applicable, 3. > > > can anyone give us a sample? > > regards > > Wei > On Apr 25, 2014, at 10:17 PM, nek5000-users at lists.mcs.anl.gov > wrote: > >> Hi matt, >> Sorry that I cannot fully answer your question, I know that at least >> the smallest edge length in the mesh is a measure for the stiffness >> of the full problem, so maybe you should avoid too small element >> heights in the boundary layer. >> However, I also would like to know how you are generating the >> airfoil mesh, since the mesh has to be coarser than a standard meshes >> and the boundary layer elements need to have curved boundaries, no? >> Which mesh generator you use and how do you convert the mesh to Nek >> format? >> The 3d problem should boil down to a 2d problem, since I assume that >> you want simulate a small part of the wing with periodic boundary >> conditions in spanwise direction... But wei, for the 2d mesh, did you >> resolve the issue to curve the boundary layer elements? >> >> Florian >> >> Am 25.04.2014 um 18:02 schrieb nek5000-users at lists.mcs.anl.gov >> : >> >>> ?HI Matt, >>> >>> Till now I have no experiments on 3D problem, what I am interested >>> in is how you generate the 3D or 2D airfoil mesh for nek5000? I >>> spend 2 weeks in generated a 2d airfoil flow mesh without any good >>> results. would you like tell me some informations? thank you a lot! >>> >>> Wei >>> >>> >>> 2014-04-25 17:00 GMT+02:00 >> >: >>> >>> Hello, >>> >>> I am looking to do simulations of flow past a wing in 3D using >>> nek5000 and I have been thinking more about potential issues >>> with high aspect ratio elements. In general we have very fine >>> resolution near the wing and then as we get further away the >>> wall normal and wall parallel spacing increases. As a first try >>> we will extend the domain in the cross stream direction which >>> will result in small dz values. I know that in general the best >>> performance is obtained with elements having dx=dy=dz and that >>> as the aspect ratio increases the performance will degrade. >>> >>> I'm wondering if there are general rules of thumb for the >>> performance degradation with increased aspect ratio. For >>> example, is an aspect ratio of 10 ok but an aspect ratio of 100 >>> unacceptable? Is this even something we can estimate in general >>> or does it vary so much problem to problem that no general >>> estimate is possible? >>> >>> I saw an earlier post that referred to the paper "An Overlapping >>> Schwarz Method for Spectral Element Solution of the >>> Incompressible Navier-Stokes Equations", P. Fischer JCP 1997. >>> From the paper I see two general strategies. >>> 1. limit the maximum aspect ratio to a critical value >>> 2. design a grid for our case, run it for a short time and then >>> iteratively add more grid points to decrease the aspect ratio >>> until optimal performance is achieved. >>> >>> Does anyone have a general or specific suggestion regarding how >>> we should handle the grid generation in terms of selecting the >>> largest aspect ratio possible with low computational cost? >>> >>> Thanks, >>> >>> Matt >>> >>> _______________________________________________ >>> 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 -- ----------------------------------------------------------------------------- Dipl. Ing. Florian Hindenlang Institut fuer Aerodynamik und Gasdynamik Phone: 0049 (0)711-685 63413 office 1.14 Pfaffenwaldring 21 70569 Stuttgart E-Mail: hindenlang at iag.uni-stuttgart.de --------------------------------------------------------------------------- -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Apr 28 08:13:02 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 28 Apr 2014 18:43:02 +0530 Subject: [Nek5000-users] Rules of thumb for element aspect ratio limits In-Reply-To: References: Message-ID: Dear all I have read on the list that you can read 3d gmsh meshes into nek via moab. Gmsh can generate higher order elements. Last time I checked, it was not possible to read 2d gmsh grids, only 3d. This would be a great option if the 2d case worked with gmsh. Best praveen On Mon, Apr 28, 2014 at 3:50 PM, wrote: > Hi Wei, > I don't think genbox is the right tool to mesh airfoils, just because you > need the curved elements for high order computations. We are using high > order meshes for discontinuous Galerkin schemes. One technique is to > construct them from agglomeration of fine structured grids (ICEM, Poitwise, > Gridgen...), leading to coarse grids with the intermediate points used for > the curved element mapping. > > But then I really don't know how this fits into the nek mesh format, since > I think there is no possibility to define intermediate interpolation points > for the elements. The only thing I saw is to prescribe a curvature of an > edge, but I think this is restricted to 2D meshes and circular geometries, > no? > > Our workaround for an airfoil computation was more or less a hack directly > in Nek, where we read Gauss-Lobatto high order points of the elements from > file (we produced ourselves, together with the Nek format with linear > edges) and replaced (overwrote) the linear elements with the curved ones > during grid setup. Maybe somebody knows a better way to do this... > > regards > > Florian > > > > Am 28.04.2014 10:38, schrieb nek5000-users at lists.mcs.anl.gov: > > Hi Florian, > > For the 2D airfoil profile, I guess, the profile in nek5000 is connected > by small straight lines not the curved lines. But even this, I have no idea > to make a mesh for 2d airfoil flow. in the Genbox introduction there is > something words on segments mesh without a sample > For Multiple Segmented Geometries > > - This feature allows users to enter a complex sequence of segments > for each of the x,y,z directions. > - Each segment set is defined in x,y,z sections. So, Lines 6-8 would > all pertain to x-dimension, 9-12 to y-dimension, ect. > > *Line 5:* The line following the string name, is the number of segments, > *nsegs*, in the x_direction > *Line 6:* The next line is the number of elements in each segment, so > there should be *nsegs* numbers. (nelx_1,nelx_2...) > *Line 7:* The next line is the start(and end) coordinates for each > segment in this direction. There should be *nsegs*+1. > (x(0),x(1)...x(nsegs)) > *Line 8:* The following line is the distribution of each segment, uniform > spacing corresponds to 1, otherwise a geometric sequence is generated. > -In conclusion, a segment between x(e-1) and x(e) is filled with nelx_e > elements determined by the geometric ratio given for that segment. > > - Repeat (Lines 5-8) for dimensions 2 and, if applicable, 3. > > > can anyone give us a sample? > > regards > > Wei > On Apr 25, 2014, at 10:17 PM, nek5000-users at lists.mcs.anl.gov wrote: > > Hi matt, > Sorry that I cannot fully answer your question, I know that at least the > smallest edge length in the mesh is a measure for the stiffness of the > full problem, so maybe you should avoid too small element heights in the > boundary layer. > However, I also would like to know how you are generating the airfoil > mesh, since the mesh has to be coarser than a standard meshes and the > boundary layer elements need to have curved boundaries, no? Which mesh > generator you use and how do you convert the mesh to Nek format? > The 3d problem should boil down to a 2d problem, since I assume that you > want simulate a small part of the wing with periodic boundary conditions in > spanwise direction... But wei, for the 2d mesh, did you resolve the issue > to curve the boundary layer elements? > > Florian > > Am 25.04.2014 um 18:02 schrieb nek5000-users at lists.mcs.anl.gov: > > ?HI Matt, > > Till now I have no experiments on 3D problem, what I am interested in is > how you generate the 3D or 2D airfoil mesh for nek5000? I spend 2 weeks in > generated a 2d airfoil flow mesh without any good results. would you like > tell me some informations? thank you a lot! > > Wei > > > 2014-04-25 17:00 GMT+02:00 : > >> Hello, >> >> I am looking to do simulations of flow past a wing in 3D using nek5000 >> and I have been thinking more about potential issues with high aspect ratio >> elements. In general we have very fine resolution near the wing and then as >> we get further away the wall normal and wall parallel spacing increases. As >> a first try we will extend the domain in the cross stream direction which >> will result in small dz values. I know that in general the best performance >> is obtained with elements having dx=dy=dz and that as the aspect ratio >> increases the performance will degrade. >> >> I'm wondering if there are general rules of thumb for the performance >> degradation with increased aspect ratio. For example, is an aspect ratio of >> 10 ok but an aspect ratio of 100 unacceptable? Is this even something we >> can estimate in general or does it vary so much problem to problem that no >> general estimate is possible? >> >> I saw an earlier post that referred to the paper "An Overlapping Schwarz >> Method for Spectral Element Solution of the Incompressible Navier-Stokes >> Equations", P. Fischer JCP 1997. From the paper I see two general >> strategies. >> 1. limit the maximum aspect ratio to a critical value >> 2. design a grid for our case, run it for a short time and then >> iteratively add more grid points to decrease the aspect ratio until optimal >> performance is achieved. >> >> Does anyone have a general or specific suggestion regarding how we >> should handle the grid generation in terms of selecting the largest aspect >> ratio possible with low computational cost? >> >> Thanks, >> >> Matt >> >> _______________________________________________ >> 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 listNek5000-users at lists.mcs.anl.govhttps://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > -- > ----------------------------------------------------------------------------- > Dipl. Ing. Florian Hindenlang > Institut fuer Aerodynamik und Gasdynamik > Phone: 0049 (0)711-685 63413 > office 1.14 > Pfaffenwaldring 21 > 70569 Stuttgart > E-Mail: hindenlang at iag.uni-stuttgart.de > --------------------------------------------------------------------------- > > > _______________________________________________ > 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 Apr 28 12:21:05 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 28 Apr 2014 19:21:05 +0200 Subject: [Nek5000-users] Rules of thumb for element aspect ratio limits In-Reply-To: References: Message-ID: Hi, it seems that the gmsh readin in moab only supports linear elements, am I right? I saw that in the newest version of moab, there is a spectral Hex module, but I don't know if this is already supported in Nek, and if moab is able to read / write spectral elements...? best Florian Am 28.04.2014 15:13, schrieb nek5000-users at lists.mcs.anl.gov: > Dear all > I have read on the list that you can read 3d gmsh meshes into nek via > moab. Gmsh can generate higher order elements. Last time I checked, it > was not possible to read 2d gmsh grids, only 3d. This would be a great > option if the 2d case worked with gmsh. > Best > praveen > > > On Mon, Apr 28, 2014 at 3:50 PM, > wrote: > > Hi Wei, > I don't think genbox is the right tool to mesh airfoils, just > because you need the curved elements for high order computations. > We are using high order meshes for discontinuous Galerkin schemes. > One technique is to construct them from agglomeration of fine > structured grids (ICEM, Poitwise, Gridgen...), leading to coarse > grids with the intermediate points used for the curved element > mapping. > > But then I really don't know how this fits into the nek mesh > format, since I think there is no possibility to define > intermediate interpolation points for the elements. The only thing > I saw is to prescribe a curvature of an edge, but I think this is > restricted to 2D meshes and circular geometries, no? > > Our workaround for an airfoil computation was more or less a hack > directly in Nek, where we read Gauss-Lobatto high order points of > the elements from file (we produced ourselves, together with the > Nek format with linear edges) and replaced (overwrote) the linear > elements with the curved ones during grid setup. Maybe somebody > knows a better way to do this... > > regards > > Florian > > > > Am 28.04.2014 10:38, schrieb nek5000-users at lists.mcs.anl.gov > : >> Hi Florian, >> >> For the 2D airfoil profile, I guess, the profile in nek5000 is >> connected by small straight lines not the curved lines. But even >> this, I have no idea to make a mesh for 2d airfoil flow. in the >> Genbox introduction there is something words on segments mesh >> without a sample >> >> >> For Multiple Segmented Geometries >> >> * This feature allows users to enter a complex sequence of >> segments for each of the x,y,z directions. >> * Each segment set is defined in x,y,z sections. So, Lines 6-8 >> would all pertain to x-dimension, 9-12 to y-dimension, ect. >> >> *Line 5:* The line following the string name, is the number of >> segments, /nsegs/, in the x_direction >> *Line 6:* The next line is the number of elements in each >> segment, so there should be /nsegs/ numbers. (nelx_1,nelx_2...) >> *Line 7:* The next line is the start(and end) coordinates for >> each segment in this direction. There should be /nsegs/+1. >> (x(0),x(1)...x(nsegs)) >> *Line 8:* The following line is the distribution of each segment, >> uniform spacing corresponds to 1, otherwise a geometric sequence >> is generated. >> >> -In conclusion, a segment between x(e-1) and x(e) is filled >> with nelx_e elements determined by the geometric ratio given >> for that segment. >> >> * Repeat (Lines 5-8) for dimensions 2 and, if applicable, 3. >> >> >> can anyone give us a sample? >> >> regards >> >> Wei >> On Apr 25, 2014, at 10:17 PM, nek5000-users at lists.mcs.anl.gov >> wrote: >> >>> Hi matt, >>> Sorry that I cannot fully answer your question, I know that at >>> least the smallest edge length in the mesh is a measure for the >>> stiffness of the full problem, so maybe you should avoid too >>> small element heights in the boundary layer. >>> However, I also would like to know how you are generating the >>> airfoil mesh, since the mesh has to be coarser than a standard >>> meshes and the boundary layer elements need to have curved >>> boundaries, no? Which mesh generator you use and how do you >>> convert the mesh to Nek format? >>> The 3d problem should boil down to a 2d problem, since I assume >>> that you want simulate a small part of the wing with periodic >>> boundary conditions in spanwise direction... But wei, for the 2d >>> mesh, did you resolve the issue to curve the boundary layer >>> elements? >>> >>> Florian >>> >>> Am 25.04.2014 um 18:02 schrieb nek5000-users at lists.mcs.anl.gov >>> : >>> >>>> ?HI Matt, >>>> >>>> Till now I have no experiments on 3D problem, what I am >>>> interested in is how you generate the 3D or 2D airfoil mesh for >>>> nek5000? I spend 2 weeks in generated a 2d airfoil flow mesh >>>> without any good results. would you like tell me some >>>> informations? thank you a lot! >>>> >>>> Wei >>>> >>>> >>>> 2014-04-25 17:00 GMT+02:00 >>> >: >>>> >>>> Hello, >>>> >>>> I am looking to do simulations of flow past a wing in 3D >>>> using nek5000 and I have been thinking more about potential >>>> issues with high aspect ratio elements. In general we have >>>> very fine resolution near the wing and then as we get >>>> further away the wall normal and wall parallel spacing >>>> increases. As a first try we will extend the domain in the >>>> cross stream direction which will result in small dz >>>> values. I know that in general the best performance is >>>> obtained with elements having dx=dy=dz and that as the >>>> aspect ratio increases the performance will degrade. >>>> >>>> I'm wondering if there are general rules of thumb for the >>>> performance degradation with increased aspect ratio. For >>>> example, is an aspect ratio of 10 ok but an aspect ratio of >>>> 100 unacceptable? Is this even something we can estimate in >>>> general or does it vary so much problem to problem that no >>>> general estimate is possible? >>>> >>>> I saw an earlier post that referred to the paper "An >>>> Overlapping Schwarz Method for Spectral Element Solution of >>>> the Incompressible Navier-Stokes Equations", P. Fischer JCP >>>> 1997. From the paper I see two general strategies. >>>> 1. limit the maximum aspect ratio to a critical value >>>> 2. design a grid for our case, run it for a short time and >>>> then iteratively add more grid points to decrease the >>>> aspect ratio until optimal performance is achieved. >>>> >>>> Does anyone have a general or specific suggestion regarding >>>> how we should handle the grid generation in terms of >>>> selecting the largest aspect ratio possible with low >>>> computational cost? >>>> >>>> Thanks, >>>> >>>> Matt >>>> >>>> _______________________________________________ >>>> 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 > > -- > ----------------------------------------------------------------------------- > Dipl. Ing. Florian Hindenlang > Institut fuer Aerodynamik und Gasdynamik > Phone: 0049 (0)711-685 63413 > office 1.14 > Pfaffenwaldring 21 > 70569 Stuttgart > E-Mail:hindenlang at iag.uni-stuttgart.de > --------------------------------------------------------------------------- > > > _______________________________________________ > 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 -- ----------------------------------------------------------------------------- Dipl. Ing. Florian Hindenlang Institut fuer Aerodynamik und Gasdynamik Phone: 0049 (0)711-685 63413 office 1.14 Pfaffenwaldring 21 70569 Stuttgart E-Mail: hindenlang at iag.uni-stuttgart.de --------------------------------------------------------------------------- -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Apr 30 11:01:33 2014 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 30 Apr 2014 18:01:33 +0200 Subject: [Nek5000-users] curved side in a block Message-ID: Dear Users, I'm trying to construct a 3D mesh which consist on a small portion of a sphere. First, I've constructed a single element. Now I'm trying to curve the edges using the "midpoint" routine, but nothing happens. What is the problem? This is my mesh: 1500.00 500.000 0.00000 0.00000 XFAC,YFAC,XZERO,YZERO **MESH DATA** 6 lines are X,Y,Z;X,Y,Z. Columns corners 1-4;5-8 1 3 1 NEL,NDIM,NELV ELEMENT 1 [ 1A] GROUP 0 144.3500 7.217500 8.838700 176.7750 -144.3500 -7.217500 0.000000 0.000000 -144.3500 -7.217500 -8.838700 -176.7750 0.000000 0.000000 0.000000 0.000000 -176.7750 -8.838700 0.000000 0.000000 -176.7750 -8.838700 -12.50000 -250.0000 ***** CURVED SIDE DATA ***** 8 Curved sides follow IEDGE,IEL,CURVE(I),I=1,5, CCURVE 2 1 8.829300 -3.6572E+00 -8.057200E+00 0.000000E+00 0.000000E+00 m 4 1 176.5864 -63.1445E+00 -1.611432E+02 0.000000E+00 0.000000E+00 m 6 1 0.000000 -1.1335E+01 5.269500E+00 0.000000E+00 0.000000E+00 m 8 1 0.000000 -2.2670E+02 1.053902E+02 0.000000E+00 0.000000E+00 m 9 1 73.14450 -1.7658E+02 -1.611443E+02 0.000000E+00 0.000000E+00 m 10 1 3.657200 -8.8293E+00 -8.057200E+00 0.000000E+00 0.000000E+00 m 11 1 11.33500 0.00000E+00 5.269500E+00 0.000000E+00 0.000000E+00 m 12 1 226.7000 0.00000E+00 1.053902E+02 0.000000E+00 0.000000E+00 m In 'CURVED SIDE DATA': Edge Element x y z dummy dummy m (x,y,z represent the coordinates of the mid point of the edge) Thank you in advance.