From nek5000-users at lists.mcs.anl.gov Wed Aug 3 04:41:19 2011 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 3 Aug 2011 11:41:19 +0200 Subject: [Nek5000-users] Using OIFS Message-ID: Hi neks, I'm trying to simulate a turbulent channel flow like in the presentation "A comparison of Nek5000 and OpenFOAM for DNS of turbulent channel flow" of Michael A. Sprague from the last user meeting ( http://www.mcs.anl.gov/~fischer/nek5000/sprague_nek5000_dec2010.pdf "mid"-case). In the presentation it is mentioned that the CFL number is approx. 2 so I have choosen the BDF3/OIFS3 scheme. However the solution blows up and Nek5000 stops the computation after 49 steps. Are there any parameters I have to set in the rea-file to get it work? TCHAR is true and p026 is set to 3. Dealiasing is turned on as well, but I'm not sure if the weight of the filter may be wrong. The files of the case are attached. Thanks! Alex -------------- next part -------------- An HTML attachment was scrubbed... URL: -------------- next part -------------- A non-text attachment was scrubbed... Name: sprague3D.tar.gz Type: application/x-gzip Size: 164402 bytes Desc: not available URL: From nek5000-users at lists.mcs.anl.gov Thu Aug 4 10:18:20 2011 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 4 Aug 2011 09:18:20 -0600 Subject: [Nek5000-users] Using OIFS In-Reply-To: References: Message-ID: Alex, I see that p26 is set to 3 -- this is the target courant number -- which should be 2, no? You might even make it smaller than that to start with. Also, for my nondimensionalization, I had 1.000000E+00 p054: direction of flow rate -- 1-X, 2-Y, 3-Z 12.56637E+00 p055: volumetric flow rate whereas you have -1.00000 p054 fixed flow rate dir: |p54|=1,2,3=x,y,z 1.00000 p055 vol.flow rate (p54>0) or Ubar (p54<0) finally, I have 4.000000E+00 p099 dealiasing 0.050 p103 filter weight of last mode whereas you have 3.00000 p099 dealiasing: <0--> off/3--> old/4--> new 0.100000E-01 p103 weight of stabilizing filter (.01) Let me know if making those changes helps. --Mike On Aug 3, 2011, at 3:41 AM, > wrote: Hi neks, I'm trying to simulate a turbulent channel flow like in the presentation "A comparison of Nek5000 and OpenFOAM for DNS of turbulent channel flow" of Michael A. Sprague from the last user meeting (http://www.mcs.anl.gov/~fischer/nek5000/sprague_nek5000_dec2010.pdf "mid"-case). In the presentation it is mentioned that the CFL number is approx. 2 so I have choosen the BDF3/OIFS3 scheme. However the solution blows up and Nek5000 stops the computation after 49 steps. Are there any parameters I have to set in the rea-file to get it work? TCHAR is true and p026 is set to 3. Dealiasing is turned on as well, but I'm not sure if the weight of the filter may be wrong. The files of the case are attached. Thanks! Alex From nek5000-users at lists.mcs.anl.gov Thu Aug 4 13:31:02 2011 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 4 Aug 2011 13:31:02 -0500 Subject: [Nek5000-users] Using OIFS In-Reply-To: References: Message-ID: Hi Alex, Lowering your DT (parameter 12) slightly will keep a more stable courant number and NEK won't blow up. -Katie On Thu, Aug 4, 2011 at 10:18 AM, wrote: > Alex, > > I see that p26 is set to 3 -- this is the target courant number -- which > should be 2, no? You might even make it smaller than that to start with. > > Also, for my nondimensionalization, I had > > 1.000000E+00 p054: direction of flow rate -- 1-X, 2-Y, 3-Z > 12.56637E+00 p055: volumetric flow rate > > whereas you have > > -1.00000 p054 fixed flow rate dir: |p54|=1,2,3=x,y,z > 1.00000 p055 vol.flow rate (p54>0) or Ubar (p54<0) > > finally, I have > > 4.000000E+00 p099 dealiasing > 0.050 p103 filter weight of last mode > > whereas you have > > 3.00000 p099 dealiasing: <0--> off/3--> old/4--> new > 0.100000E-01 p103 weight of stabilizing filter (.01) > > > Let me know if making those changes helps. > > --Mike > > > > > On Aug 3, 2011, at 3:41 AM, nek5000-users at lists.mcs.anl.gov>> wrote: > > Hi neks, > > I'm trying to simulate a turbulent channel flow like in the presentation "A > comparison > of Nek5000 and OpenFOAM for DNS of turbulent channel flow" of Michael A. > Sprague from the last > user meeting ( > http://www.mcs.anl.gov/~fischer/nek5000/sprague_nek5000_dec2010.pdf"mid"-case). > In the presentation it is mentioned that the CFL number is approx. 2 so I > have choosen the BDF3/OIFS3 > scheme. However the solution blows up and Nek5000 stops the computation > after 49 steps. > > Are there any parameters I have to set in the rea-file to get it work? > TCHAR is true and p026 is > set to 3. Dealiasing is turned on as well, but I'm not sure if the weight > of the filter may be wrong. > > The files of the case are attached. > > Thanks! > Alex > > > _______________________________________________ > 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 Aug 4 22:26:25 2011 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 04 Aug 2011 22:26:25 -0500 Subject: [Nek5000-users] Help With Basic NEK Configuration Message-ID: Hi, I am a new to NEK and I am trying to run a few examples for my OS scaling experiments. I went through the manual which is at: http://www.mcs.anl.gov/~fischer/new.pdf. In the chapter that speaks about a basic problem setup, there is a line in the 'Memory Requirements' section that says: Total Memory Required for simulation = E(N +1)^3 points ? 400(wds/pt) ? 8bytes/wd I have been playing around with the SIZE file a little bit and adjusting, lx1, lelt, lxd, lp and lelg parameters. However I am unable to find where I can adjust 'E' from the equation. I understand that 'lelt' is maximum elements per processor and 'lelg' is maximum elements per simulation? Is 'lelg' same as 'E'? is 'lelt = lelg / nprocs' ? I assumed that 'E = lelg' and changed 'lelg' for 'timing' example to run it on a 4096 node configuration (1 rack of BG/P:Intrepid in VN mode). I keep getting the error: Too many processors ( 4096 ) for to few elements ( 512 ) ... and the value 512 does not seem to change although I have changed 'lelg' and run 'makenek timing'. Is the value of 'E' picked up from the .re2 file? Would I have to generate it using 'genbox' after I change some other configuration? I understand that NEK has been scaled upto 40 racks of Intrepid at Argonne. I am also trying to run experiments of upto 32 racks if possible. But I want to get started with smaller runs. Is there a repository of configurations or tarred files where I could get larger, successfully run problem instances? Thanks. Regards, Harish Naik Predoctoral Appointee Mathematics & Computer Science Division Argonne National Laboratory P: (630) 252-2029 W: http://www.mcs.anl.gov/~hnaik From nek5000-users at lists.mcs.anl.gov Fri Aug 5 04:09:36 2011 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 5 Aug 2011 11:09:36 +0200 Subject: [Nek5000-users] Help With Basic NEK Configuration In-Reply-To: References: Message-ID: Hi Harish I don't think the manual you are refering to is up-to-date. To get a rough idea about your memory footprint use 'size nek5000' on the command line. The size tool will report the total size of a static data items. Note, the actual size of the memory footprint will be different: - Static data items which are not "touched" duing execution will not be allocated, hence the acutal memory usage is lower. This is not true on Blue Gene as the CNK-kernel does not use an over-optimistic memory model. - Dynamically allocated variables within Nek (gs-code) increase the actual memory usage (I don't think more than 50MB but this depends on the particular setup) - Memory allocated by MPI (size depends on the MPI implemenation). On Blue Gene this can be significant fraction considering the fact that a communicator is ~6MB on 72 Racks. Note, Nek's AMG solver uses 50-80 communicators depending on the number of AMG levels. This can be tricky but there are ways to reduce the memory footprint of a communicator. Contact me again if you need more details on that. The SIZE file is used to size all static data within Nek. Hence, all numbers are considered as 'upper limits'. For more details check the wiki: http://nek5000.mcs.anl.gov/index.php/SIZEu You can run Nek on any number of processors. However, the implemented domain decompostion (RSB) works best if the number of processors is a power of two. Here you'll find some parallel scaling data: http://nek5000.mcs.anl.gov/index.php/Scaling Cheers, Stefan On 8/5/11, nek5000-users at lists.mcs.anl.gov wrote: > Hi, > > I am a new to NEK and I am trying to run a few examples for my OS scaling > experiments. I went through the manual which is at: > http://www.mcs.anl.gov/~fischer/new.pdf. In the chapter that speaks about > a basic problem setup, there is a line in the 'Memory Requirements' > section that says: > > Total Memory Required for simulation = E(N +1)^3 points ? 400(wds/pt) ? > 8bytes/wd > > I have been playing around with the SIZE file a little bit and adjusting, > lx1, lelt, lxd, lp and lelg parameters. However I am unable to find where > I can adjust 'E' from the equation. I understand that 'lelt' is maximum > elements per processor and 'lelg' is maximum elements per simulation? Is > 'lelg' same as 'E'? is 'lelt = lelg / nprocs' ? I assumed that 'E = lelg' > and changed 'lelg' for 'timing' example to run it on a 4096 node > configuration (1 rack of BG/P:Intrepid in VN mode). I keep getting the > error: > > Too many processors ( 4096 ) for to few elements ( 512 ) > > ... and the value 512 does not seem to change although I have changed > 'lelg' and run 'makenek timing'. Is the value of 'E' picked up from the > .re2 file? Would I have to generate it using 'genbox' after I change some > other configuration? > > I understand that NEK has been scaled upto 40 racks of Intrepid at > Argonne. I am also trying to run experiments of upto 32 racks if possible. > But I want to get started with smaller runs. Is there a repository of > configurations or tarred files where I could get larger, successfully run > problem instances? > > Thanks. > > Regards, > Harish Naik > Predoctoral Appointee > Mathematics & Computer Science Division > Argonne National Laboratory > P: (630) 252-2029 > W: http://www.mcs.anl.gov/~hnaik > _______________________________________________ > 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 Aug 5 09:08:01 2011 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 5 Aug 2011 09:08:01 -0500 (CDT) Subject: [Nek5000-users] Help With Basic NEK Configuration In-Reply-To: References: Message-ID: Harish, We can help you with the larger runs. The memory constraint is only one constraint, and it does not limit how _small_ a problem can be. There is a different constraint on problem size/processor count, which is that you must have at least one element per processor. So if the problem has E=512 elements, then P_max = 512. It sounds like you've done a pretty good job of exploring the parameter space for the memory footprint etc. Memory requirements on a processor for a given compilation is, to leading order, given by the product: S*lx1*ly1*lz1*lelt where S is between 200 and 400 words, each word being 8 bytes. There are other terms that can be important in some specific cases, particularly for large element (and hence, processor) counts. But these are pretty well under control. Specifically, there are two (4 byte) integer arrays that scale as lelg. Your total problem size (E==nelt in the .rea file) is constrained by: E =< min(lelg,P*lelt) where P is the number of processors at run time. Similarly, P is constrained by: P =< lp There should be no memory impact for having a large value of lp. Paul On Thu, 4 Aug 2011, nek5000-users at lists.mcs.anl.gov wrote: > Hi, > > I am a new to NEK and I am trying to run a few examples for my OS scaling > experiments. I went through the manual which is at: > http://www.mcs.anl.gov/~fischer/new.pdf. In the chapter that speaks about > a basic problem setup, there is a line in the 'Memory Requirements' > section that says: > > Total Memory Required for simulation = E(N +1)^3 points ?? 400(wds/pt) ?? > 8bytes/wd > > I have been playing around with the SIZE file a little bit and adjusting, > lx1, lelt, lxd, lp and lelg parameters. However I am unable to find where > I can adjust 'E' from the equation. I understand that 'lelt' is maximum > elements per processor and 'lelg' is maximum elements per simulation? Is > 'lelg' same as 'E'? is 'lelt = lelg / nprocs' ? I assumed that 'E = lelg' > and changed 'lelg' for 'timing' example to run it on a 4096 node > configuration (1 rack of BG/P:Intrepid in VN mode). I keep getting the > error: > > Too many processors ( 4096 ) for to few elements ( 512 ) > > ... and the value 512 does not seem to change although I have changed > 'lelg' and run 'makenek timing'. Is the value of 'E' picked up from the > .re2 file? Would I have to generate it using 'genbox' after I change some > other configuration? > > I understand that NEK has been scaled upto 40 racks of Intrepid at > Argonne. I am also trying to run experiments of upto 32 racks if possible. > But I want to get started with smaller runs. Is there a repository of > configurations or tarred files where I could get larger, successfully run > problem instances? > > Thanks. > > Regards, > Harish Naik > Predoctoral Appointee > Mathematics & Computer Science Division > Argonne National Laboratory > P: (630) 252-2029 > W: http://www.mcs.anl.gov/~hnaik > _______________________________________________ > 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 Aug 5 10:04:32 2011 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 05 Aug 2011 10:04:32 -0500 Subject: [Nek5000-users] Help With Basic NEK Configuration In-Reply-To: References: Message-ID: Stefan & Paul, Thank you both for all the hints. I will make use of these in my runs and will ask more questions if I have any. Regards, Harish On Fri, 05 Aug 2011 09:08:01 -0500, wrote: > > Harish, > > We can help you with the larger runs. > > The memory constraint is only one constraint, and it does > not limit how _small_ a problem can be. > > There is a different constraint on problem size/processor > count, which is that you must have at least one element > per processor. So if the problem has E=512 elements, > then P_max = 512. > > It sounds like you've done a pretty good job of exploring > the parameter space for the memory footprint etc. > > Memory requirements on a processor for a given compilation > is, to leading order, given by the product: > > S*lx1*ly1*lz1*lelt > > where S is between 200 and 400 words, each word being 8 bytes. > > There are other terms that can be important in some specific > cases, particularly for large element (and hence, processor) > counts. But these are pretty well under control. Specifically, > there are two (4 byte) integer arrays that scale as lelg. > > Your total problem size (E==nelt in the .rea file) is constrained > by: > > E =< min(lelg,P*lelt) > > where P is the number of processors at run time. Similarly, P > is constrained by: > > P =< lp > > > There should be no memory impact for having a large value of lp. > > Paul > > > > On Thu, 4 Aug 2011, nek5000-users at lists.mcs.anl.gov wrote: > >> Hi, >> >> I am a new to NEK and I am trying to run a few examples for my OS >> scaling >> experiments. I went through the manual which is at: >> http://www.mcs.anl.gov/~fischer/new.pdf. In the chapter that speaks >> about >> a basic problem setup, there is a line in the 'Memory Requirements' >> section that says: >> >> Total Memory Required for simulation = E(N +1)^3 points ?? 400(wds/pt) >> ?? >> 8bytes/wd >> >> I have been playing around with the SIZE file a little bit and >> adjusting, >> lx1, lelt, lxd, lp and lelg parameters. However I am unable to find >> where >> I can adjust 'E' from the equation. I understand that 'lelt' is maximum >> elements per processor and 'lelg' is maximum elements per simulation? Is >> 'lelg' same as 'E'? is 'lelt = lelg / nprocs' ? I assumed that 'E = >> lelg' >> and changed 'lelg' for 'timing' example to run it on a 4096 node >> configuration (1 rack of BG/P:Intrepid in VN mode). I keep getting the >> error: >> >> Too many processors ( 4096 ) for to few elements ( 512 ) >> >> ... and the value 512 does not seem to change although I have changed >> 'lelg' and run 'makenek timing'. Is the value of 'E' picked up from the >> .re2 file? Would I have to generate it using 'genbox' after I change >> some >> other configuration? >> >> I understand that NEK has been scaled upto 40 racks of Intrepid at >> Argonne. I am also trying to run experiments of upto 32 racks if >> possible. >> But I want to get started with smaller runs. Is there a repository of >> configurations or tarred files where I could get larger, successfully >> run >> problem instances? >> >> Thanks. >> >> Regards, >> Harish Naik >> Predoctoral Appointee >> Mathematics & Computer Science Division >> Argonne National Laboratory >> P: (630) 252-2029 >> W: http://www.mcs.anl.gov/~hnaik >> _______________________________________________ >> 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 Aug 5 14:33:25 2011 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 5 Aug 2011 14:33:25 -0500 (CDT) Subject: [Nek5000-users] Using OIFS In-Reply-To: References: Message-ID: Hi Alex, The issue seems to be that the given initial conditions lead to high CFL numbers at early times, which is why the code was blowing up. It looks like your case will work if you just set dt > 0, (param 12 in the .rea file). This will allow the variable dt to kick in and will keep the CFL number in the proper range, and at all times will keep dt =< .034, your chosen value. Also, I noticed a small bug in the .usr file, which I have now fixed in the examples/ directory. There should be no call of the form: call avg1(ffx_avg,ffx_new,alpha,beta,1,'ffxa',ifverbose) The routine avg1() is designed to work on arrays, whereas ffx_avg and ffx_new are scalars. It's unclear what the consequences of the call are -- they would vary from one platform to the next, but could result in undesirable memory overwrites. Paul PS - attached is a set of files that should work. On Wed, 3 Aug 2011, nek5000-users at lists.mcs.anl.gov wrote: > Hi neks, > > I'm trying to simulate a turbulent channel flow like in the presentation "A > comparison > of Nek5000 and OpenFOAM for DNS of turbulent channel flow" of Michael A. > Sprague from the last > user meeting ( > http://www.mcs.anl.gov/~fischer/nek5000/sprague_nek5000_dec2010.pdf > "mid"-case). > In the presentation it is mentioned that the CFL number is approx. 2 so I > have choosen the BDF3/OIFS3 > scheme. However the solution blows up and Nek5000 stops the computation > after 49 steps. > > Are there any parameters I have to set in the rea-file to get it work? TCHAR > is true and p026 is > set to 3. Dealiasing is turned on as well, but I'm not sure if the weight of > the filter may be wrong. > > The files of the case are attached. > > Thanks! > Alex > -------------- next part -------------- A non-text attachment was scrubbed... Name: t.tar.gz Type: application/octet-stream Size: 145659 bytes Desc: URL: From nek5000-users at lists.mcs.anl.gov Sat Aug 6 21:05:32 2011 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sat, 6 Aug 2011 21:05:32 -0500 (CDT) Subject: [Nek5000-users] Using OIFS In-Reply-To: References: Message-ID: PS -- In the files I sent, I had a line: ubar = glsum(vx,bm1,n)/volvm1 which should read: ubar = glsc2(vx,bm1,n)/volvm1 Paul On Fri, 5 Aug 2011, nek5000-users at lists.mcs.anl.gov wrote: > > Hi Alex, > > The issue seems to be that the given initial conditions lead > to high CFL numbers at early times, which is why the code > was blowing up. > > It looks like your case will work if you just set dt > 0, > (param 12 in the .rea file). > > This will allow the variable dt to kick in and will keep > the CFL number in the proper range, and at all times will > keep dt =< .034, your chosen value. > > Also, I noticed a small bug in the .usr file, which I have > now fixed in the examples/ directory. There should be no > call of the form: > > call avg1(ffx_avg,ffx_new,alpha,beta,1,'ffxa',ifverbose) > > The routine avg1() is designed to work on arrays, whereas > ffx_avg and ffx_new are scalars. > > It's unclear what the consequences of the call are -- they > would vary from one platform to the next, but could result > in undesirable memory overwrites. > > Paul > > PS - attached is a set of files that should work. > > On Wed, 3 Aug 2011, nek5000-users at lists.mcs.anl.gov wrote: > >> Hi neks, >> >> I'm trying to simulate a turbulent channel flow like in the presentation "A >> comparison >> of Nek5000 and OpenFOAM for DNS of turbulent channel flow" of Michael A. >> Sprague from the last >> user meeting ( >> http://www.mcs.anl.gov/~fischer/nek5000/sprague_nek5000_dec2010.pdf >> "mid"-case). >> In the presentation it is mentioned that the CFL number is approx. 2 so I >> have choosen the BDF3/OIFS3 >> scheme. However the solution blows up and Nek5000 stops the computation >> after 49 steps. >> >> Are there any parameters I have to set in the rea-file to get it work? >> TCHAR >> is true and p026 is >> set to 3. Dealiasing is turned on as well, but I'm not sure if the weight >> of >> the filter may be wrong. >> >> The files of the case are attached. >> >> Thanks! >> Alex > From nek5000-users at lists.mcs.anl.gov Mon Aug 8 06:09:56 2011 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 8 Aug 2011 13:09:56 +0200 Subject: [Nek5000-users] Using OIFS In-Reply-To: References: Message-ID: Thanks for your replies! I think, it works now. The flow looks good, but there is/was an error in the post-processing part. The?initialization?made some problems and the wrong wall size was in the userfile. I changed the parameters like Mike suggested and took DT=0.02 what seems to be fine. I'm currently running a simulation with param(12) = 0.034 so the time step size can be varied by Nek. I hope the post-processing will do its job this time. Alex 2011/8/7 > > PS -- > > In the files I sent, I had a line: > > ? ? ?ubar = glsum(vx,bm1,n)/volvm1 > > which should read: > > ? ? ?ubar = glsc2(vx,bm1,n)/volvm1 > > > Paul > > > On Fri, 5 Aug 2011, nek5000-users at lists.mcs.anl.gov wrote: > >> >> Hi Alex, >> >> The issue seems to be that the given initial conditions lead >> to high CFL numbers at early times, which is why the code >> was blowing up. >> >> It looks like your case will work if you just set dt > 0, >> (param 12 in the .rea file). >> >> This will allow the variable dt to kick in and will keep >> the CFL number in the proper range, and at all times will >> keep dt =< .034, your chosen value. >> >> Also, I noticed a small bug in the .usr file, which I have >> now fixed in the examples/ directory. ?There should be no >> call of the form: >> >> ?call avg1(ffx_avg,ffx_new,alpha,beta,1,'ffxa',ifverbose) >> >> The routine avg1() is designed to work on arrays, whereas >> ffx_avg and ffx_new are scalars. >> >> It's unclear what the consequences of the call are -- they >> would vary from one platform to the next, but could result >> in undesirable memory overwrites. >> >> Paul >> >> PS - attached is a set of files that should work. >> >> On Wed, 3 Aug 2011, nek5000-users at lists.mcs.anl.gov wrote: >> >>> Hi neks, >>> >>> I'm trying to simulate a turbulent channel flow like in the presentation "A >>> comparison >>> of Nek5000 and OpenFOAM for DNS of turbulent channel flow" of Michael A. >>> Sprague from the last >>> user meeting ( >>> http://www.mcs.anl.gov/~fischer/nek5000/sprague_nek5000_dec2010.pdf >>> "mid"-case). >>> In the presentation it is mentioned that the CFL number is approx. 2 so I >>> have choosen the BDF3/OIFS3 >>> scheme. However the solution blows up and Nek5000 stops the computation >>> after 49 steps. >>> >>> Are there any parameters I have to set in the rea-file to get it work? TCHAR >>> is true and p026 is >>> set to 3. Dealiasing is turned on as well, but I'm not sure if the weight of >>> the filter may be wrong. >>> >>> The files of the case are attached. >>> >>> Thanks! >>> Alex >> > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Tue Aug 9 16:43:15 2011 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 9 Aug 2011 16:43:15 -0500 Subject: [Nek5000-users] userf/userq in .usr file Message-ID: Hello Neks, I had a couple of questions regarding userf and userq. 1) If we add something to, for example, ffx in userf, is that "something" subsequently multiplied by the mass matrix later on in the source code, or is that on the user to multiply ffx(i,j,k,e) by its appropriate bm1 entry? 2) In userq, is "source" used for anything? I tried looking through the source code, and I can see where "qvol" is used, but not where "source" is used. Thanks, -- Josh Camp "All that is necessary for the triumph of evil is that good men do nothing" -- Edmund Burke From nek5000-users at lists.mcs.anl.gov Thu Aug 11 05:41:20 2011 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 11 Aug 2011 16:11:20 +0530 Subject: [Nek5000-users] Solving for fluid flows on a sphere Message-ID: <5fb20c0abcda26f44ece832f761c8e18.squirrel@webmail.iitk.ac.in> Hi Nek devs, Is it possible to use NEK to solve for Navier Stokes equations on the surface of a sphere, where r is fixed and the velocity varies in theta and phi? Thanks, Mani Chandra From nek5000-users at lists.mcs.anl.gov Thu Aug 11 07:16:12 2011 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 11 Aug 2011 07:16:12 -0500 (CDT) Subject: [Nek5000-users] Solving for fluid flows on a sphere In-Reply-To: <5fb20c0abcda26f44ece832f761c8e18.squirrel@webmail.iitk.ac.in> References: <5fb20c0abcda26f44ece832f761c8e18.squirrel@webmail.iitk.ac.in> Message-ID: Hi Mani, Probably your best bet is to use a very thin layer of elements in a 3D spherical shell with SYM bcs on faces 5 & 6, plus the stress formulation. I would imagine that a shell of thickness .001 with R=1.0 might be feasible. Instructions for constructing a 3D shell can be found in www.mcs.anl.gov/~fischer/primer.pdf (Some of this info may already have been transferred into current manual.) We can help with this if you need any assistance. Regards, Paul On Thu, 11 Aug 2011, nek5000-users at lists.mcs.anl.gov wrote: > Hi Nek devs, > > Is it possible to use NEK to solve for Navier Stokes equations on the > surface of a sphere, where r is fixed and the velocity varies in theta and > phi? > > Thanks, > Mani Chandra > _______________________________________________ > 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 Aug 11 08:12:39 2011 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 11 Aug 2011 18:42:39 +0530 Subject: [Nek5000-users] Solving for fluid flows on a sphere In-Reply-To: References: <5fb20c0abcda26f44ece832f761c8e18.squirrel@webmail.iitk.ac.in> Message-ID: <63d85810fb7e3d63e8ebe8ca3d62dfc5.squirrel@webmail.iitk.ac.in> Hi Paul, Thanks for the response. I'll give it a shot and will post to the mailing list again for help. Regards, Mani > > Hi Mani, > > Probably your best bet is to use a very thin layer of elements > in a 3D spherical shell with SYM bcs on faces 5 & 6, plus the > stress formulation. I would imagine that a shell of thickness > .001 with R=1.0 might be feasible. > > Instructions for constructing a 3D shell can be found in > www.mcs.anl.gov/~fischer/primer.pdf > > (Some of this info may already have been transferred into > current manual.) We can help with this if you need any > assistance. > > Regards, > > Paul > > > On Thu, 11 Aug 2011, nek5000-users at lists.mcs.anl.gov wrote: > >> Hi Nek devs, >> >> Is it possible to use NEK to solve for Navier Stokes equations on the >> surface of a sphere, where r is fixed and the velocity varies in theta >> and >> phi? >> >> Thanks, >> Mani Chandra >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > From nek5000-users at lists.mcs.anl.gov Thu Aug 11 15:15:49 2011 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 11 Aug 2011 15:15:49 -0500 Subject: [Nek5000-users] Error stemming from genbox Message-ID: Neks, I was getting an odd error in Nek when using geometry generated from the newest version of genbox (repo 718) that I did not get from repo 713 (the log file from the run using genbox from repo 718 is attached--the error message appears at the top). After comparing the two generated .rea files, I found the issue. On older versions of genbox, it seems that it took the base.rea file specified and used the upper portion of it to generate the header of your new .rea file. But, on the new version, it doesn't appear to do this for the logical flags. So, the issue I was running into (while running the example turbChannel) was that IFTRAN T in base.rea was being replaced by IFHEAT F in the generated box.rea file, where in the older version it kept them the same. Manually changing IFHEAT F back to IFTRAN T removed the error message and the case ran fine as normal. I'm not sure if this was an intentional change or not, or if anyone else has run into this issue, but I thought this might help clear up any confusion if anyone else runs into this same problem (took me a while to figure out what exactly was going wrong :) ). -- Josh Camp "All that is necessary for the triumph of evil is that good men do nothing" -- Edmund Burke -------------- next part -------------- A non-text attachment was scrubbed... Name: turbChannel.log Type: application/octet-stream Size: 8536 bytes Desc: not available URL: From nek5000-users at lists.mcs.anl.gov Thu Aug 11 15:56:19 2011 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 11 Aug 2011 15:56:19 -0500 Subject: [Nek5000-users] Error stemming from genbox In-Reply-To: References: Message-ID: HI Josh, Yes, the current version of genbox should be set up to set the logical flags a little differently than before. Now, the user is able to create a .rea file for heat only simulations by setting the number of fields (line 3 in the .box file) to negative, so part of the logical flags are written out differently than before. However, it shouldn't overwrite the IFTRAN logical, that is an error. I will take care of it and update the repo. Thanks!! Katie On Thu, Aug 11, 2011 at 3:15 PM, wrote: > Neks, > > I was getting an odd error in Nek when using geometry generated from > the newest version of genbox (repo 718) that I did not get from repo > 713 (the log file from the run using genbox from repo 718 is > attached--the error message appears at the top). > > After comparing the two generated .rea files, I found the issue. On > older versions of genbox, it seems that it took the base.rea file > specified and used the upper portion of it to generate the header of > your new .rea file. But, on the new version, it doesn't appear to do > this for the logical flags. So, the issue I was running into (while > running the example turbChannel) was that > > IFTRAN T > > in base.rea was being replaced by > > IFHEAT F > > in the generated box.rea file, where in the older version it kept them > the same. Manually changing IFHEAT F back to IFTRAN T > removed the error message and the case ran fine as normal. > > I'm not sure if this was an intentional change or not, or if anyone > else has run into this issue, but I thought this might help clear up > any confusion if anyone else runs into this same problem (took me a > while to figure out what exactly was going wrong :) ). > > -- > Josh Camp > > "All that is necessary for the triumph of evil is that good men do > nothing" -- Edmund Burke > > _______________________________________________ > 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 Aug 11 17:07:22 2011 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 11 Aug 2011 17:07:22 -0500 (CDT) Subject: [Nek5000-users] userf/userq in .usr file In-Reply-To: Message-ID: <2036997801.213339.1313100442444.JavaMail.root@zimbra.anl.gov> Hi Josh, Yes, you are right that the variable SOURCE in userq seems to be outdated -- only qvol is used in nekuq(). As far as multiplication of ffx,... by masss matrix is concerned -- it's done in makeuf() (after calling nekuf() which calls userf()), so there is no need to do the multiplication in userf(): subroutine makeuf ... CALL NEKUF (BFX,BFY,BFZ) CALL OPCOLV (BFX,BFY,BFZ,BM1) Best, Aleks ----- Original Message ----- From: nek5000-users at lists.mcs.anl.gov To: "nek5000-users" Sent: Tuesday, August 9, 2011 4:43:15 PM Subject: [Nek5000-users] userf/userq in .usr file Hello Neks, I had a couple of questions regarding userf and userq. 1) If we add something to, for example, ffx in userf, is that "something" subsequently multiplied by the mass matrix later on in the source code, or is that on the user to multiply ffx(i,j,k,e) by its appropriate bm1 entry? 2) In userq, is "source" used for anything? I tried looking through the source code, and I can see where "qvol" is used, but not where "source" is used. Thanks, -- Josh Camp "All that is necessary for the triumph of evil is that good men do nothing" -- Edmund Burke _______________________________________________ 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 Aug 12 08:18:21 2011 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 12 Aug 2011 08:18:21 -0500 Subject: [Nek5000-users] userf/userq in .usr file In-Reply-To: <2036997801.213339.1313100442444.JavaMail.root@zimbra.anl.gov> References: <2036997801.213339.1313100442444.JavaMail.root@zimbra.anl.gov> Message-ID: Thank you for the clarification Aleks. I wanted to make sure I wasn't unknowingly integrating my forcing function twice :). Josh On Thu, Aug 11, 2011 at 5:07 PM, wrote: > Hi Josh, > > Yes, you are right that the variable SOURCE in userq seems to be outdated -- only qvol is used in nekuq(). > > As far as multiplication of ffx,... by masss matrix is concerned -- it's done in makeuf() (after calling nekuf() which calls userf()), so there is no need to do the multiplication in userf(): > > > ? ? ?subroutine makeuf > ... > ? ? ?CALL NEKUF ? (BFX,BFY,BFZ) > ? ? ?CALL OPCOLV (BFX,BFY,BFZ,BM1) > > > Best, > Aleks > > > ----- Original Message ----- > From: nek5000-users at lists.mcs.anl.gov > To: "nek5000-users" > Sent: Tuesday, August 9, 2011 4:43:15 PM > Subject: [Nek5000-users] userf/userq in .usr file > > Hello Neks, > > I had a couple of questions regarding userf and userq. > > 1) ?If we add something to, for example, ffx in userf, is that > "something" subsequently multiplied by the mass matrix later on in the > source code, or is that on the user to multiply ffx(i,j,k,e) by its > appropriate bm1 entry? > > 2) ?In userq, is "source" used for anything? ?I tried looking through > the source code, and I can see where "qvol" is used, but not where > "source" is used. > > > Thanks, > > -- > Josh Camp > > "All that is necessary for the triumph of evil is that good men do > nothing" -- Edmund Burke > _______________________________________________ > 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 > -- Josh Camp "All that is necessary for the triumph of evil is that good men do nothing" -- Edmund Burke From nek5000-users at lists.mcs.anl.gov Fri Aug 12 08:19:20 2011 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 12 Aug 2011 08:19:20 -0500 Subject: [Nek5000-users] Error stemming from genbox In-Reply-To: References: Message-ID: Thanks for looking into it Katie! Josh On Thu, Aug 11, 2011 at 3:56 PM, wrote: > HI Josh, > > Yes, the current version of genbox should be set up to set the logical flags > a little differently than before. > > Now, the user is able to create a .rea file for heat only simulations by > setting the number of fields (line 3 in the .box file) to negative, so part > of the logical flags are written out differently than before. > > However, it shouldn't overwrite the IFTRAN logical, that is an error.? I > will take care of it and update the repo. > > Thanks!! > Katie > > On Thu, Aug 11, 2011 at 3:15 PM, wrote: >> >> Neks, >> >> I was getting an odd error in Nek when using geometry generated from >> the newest version of genbox (repo 718) that I did not get from repo >> 713 (the log file from the run using genbox from repo 718 is >> attached--the error message appears at the top). >> >> After comparing the two generated .rea files, I found the issue. ?On >> older versions of genbox, it seems that it took the base.rea file >> specified and used the upper portion of it to generate the header of >> your new .rea file. ?But, on the new version, it doesn't appear to do >> this for the logical flags. ?So, the issue I was running into (while >> running the example turbChannel) was that >> >> IFTRAN ? ?T >> >> in base.rea was being replaced by >> >> IFHEAT ? ?F >> >> in the generated box.rea file, where in the older version it kept them >> the same. ? Manually changing IFHEAT ? ?F ? back to IFTRAN ? ?T >> removed the error message and the case ran fine as normal. >> >> I'm not sure if this was an intentional change or not, or if anyone >> else has run into this issue, but I thought this might help clear up >> any confusion if anyone else runs into this same problem (took me a >> while to figure out what exactly was going wrong :) ). >> >> -- >> Josh Camp >> >> "All that is necessary for the triumph of evil is that good men do >> nothing" -- Edmund Burke >> >> _______________________________________________ >> 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 > > -- Josh Camp "All that is necessary for the triumph of evil is that good men do nothing" -- Edmund Burke From nek5000-users at lists.mcs.anl.gov Sun Aug 14 01:17:05 2011 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 14 Aug 2011 11:47:05 +0530 Subject: [Nek5000-users] Solving for fluid flows on a sphere In-Reply-To: References: <5fb20c0abcda26f44ece832f761c8e18.squirrel@webmail.iitk.ac.in> Message-ID: <4E476861.5030201@gmail.com> Hi Paul, I setup a simulation but I keep getting NaN's when I give nontrivial initial data. I'm attaching the relevant files. Could you please try it out? I checked that the initial data is divergence free and satisfies the boundary conditions (u_r = 0, du_theta/dr = 0, du_phi/dr = 0). Regards, Mani On 08/11/2011 05:46 PM, nek5000-users at lists.mcs.anl.gov wrote: > > Hi Mani, > > Probably your best bet is to use a very thin layer of elements > in a 3D spherical shell with SYM bcs on faces 5 & 6, plus the > stress formulation. I would imagine that a shell of thickness > .001 with R=1.0 might be feasible. > > Instructions for constructing a 3D shell can be found in > www.mcs.anl.gov/~fischer/primer.pdf > > (Some of this info may already have been transferred into > current manual.) We can help with this if you need any > assistance. > > Regards, > > Paul > > > On Thu, 11 Aug 2011, nek5000-users at lists.mcs.anl.gov wrote: > >> Hi Nek devs, >> >> Is it possible to use NEK to solve for Navier Stokes equations on the >> surface of a sphere, where r is fixed and the velocity varies in >> theta and >> phi? >> >> Thanks, >> Mani Chandra >> _______________________________________________ >> 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 embedded and charset-unspecified text was scrubbed... Name: shell.map URL: -------------- next part -------------- An embedded and charset-unspecified text was scrubbed... Name: shell.rea URL: -------------- next part -------------- An embedded and charset-unspecified text was scrubbed... Name: shell.usr URL: -------------- next part -------------- An embedded and charset-unspecified text was scrubbed... Name: SIZE URL: From nek5000-users at lists.mcs.anl.gov Sun Aug 14 07:01:56 2011 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 14 Aug 2011 07:01:56 -0500 (CDT) Subject: [Nek5000-users] Solving for fluid flows on a sphere In-Reply-To: <4E476861.5030201@gmail.com> References: <5fb20c0abcda26f44ece832f761c8e18.squirrel@webmail.iitk.ac.in> <4E476861.5030201@gmail.com> Message-ID: Hi Mani, I ran this with G="-g -Ktrap=fp" and the "nekd" script in serial (just gdb nek5000 after setting up requisite files). Here is the output: Program received signal SIGFPE, Arithmetic exception. 0x000000000040376c in useric_ (ix=1, iy=1, iz=1, ieg=3) at /homes/fischer/nek_debug/mani/z.f:83 83 utheta = 1.0/(x**2 + y**2)**0.5 (gdb) This makes sense -- you have a pole singularity in this formulation. I'm certain it's a removable singularity if you just rework your ux/uy velocity definition. Please let me know if this resolves the issue. Paul On Sun, 14 Aug 2011, nek5000-users at lists.mcs.anl.gov wrote: > Hi Paul, > > I setup a simulation but I keep getting NaN's when I give nontrivial initial > data. I'm attaching the relevant files. Could you please try it out? > > I checked that the initial data is divergence free and satisfies the boundary > conditions (u_r = 0, du_theta/dr = 0, du_phi/dr = 0). > > Regards, > Mani > > On 08/11/2011 05:46 PM, nek5000-users at lists.mcs.anl.gov wrote: >> >> Hi Mani, >> >> Probably your best bet is to use a very thin layer of elements >> in a 3D spherical shell with SYM bcs on faces 5 & 6, plus the >> stress formulation. I would imagine that a shell of thickness >> .001 with R=1.0 might be feasible. >> >> Instructions for constructing a 3D shell can be found in >> www.mcs.anl.gov/~fischer/primer.pdf >> >> (Some of this info may already have been transferred into >> current manual.) We can help with this if you need any >> assistance. >> >> Regards, >> >> Paul >> >> >> On Thu, 11 Aug 2011, nek5000-users at lists.mcs.anl.gov wrote: >> >>> Hi Nek devs, >>> >>> Is it possible to use NEK to solve for Navier Stokes equations on the >>> surface of a sphere, where r is fixed and the velocity varies in theta and >>> phi? >>> >>> Thanks, >>> Mani Chandra >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> > > From nek5000-users at lists.mcs.anl.gov Sun Aug 14 07:56:47 2011 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 14 Aug 2011 18:26:47 +0530 Subject: [Nek5000-users] Solving for fluid flows on a sphere In-Reply-To: References: <5fb20c0abcda26f44ece832f761c8e18.squirrel@webmail.iitk.ac.in> <4E476861.5030201@gmail.com> Message-ID: Hi Paul, Thanks for the diagnosing this problem. Indeed it is bad initial data. At the moment I do not have specific initial data or forcing to work with and so I'm just trying out the feasibility of using NEK to solve on the shell. I should have some concrete initial data in the next couple of days. When I try to repeat the run with ux = 0.0 uy = 0.0 uz = 0.0 and ffx = 0.0 ffy = 0.0 ffz = 1.0 NEK shows a lot of convergence errors. Could you check this out? I've attached the .rea file. Thanks, Mani On Sun, Aug 14, 2011 at 5:31 PM, wrote: > > Hi Mani, > > I ran this with > > G="-g -Ktrap=fp" > > and the "nekd" script in serial (just gdb nek5000 after > setting up requisite files). > > Here is the output: > > Program received signal SIGFPE, Arithmetic exception. > 0x000000000040376c in useric_ (ix=1, iy=1, iz=1, ieg=3) > at /homes/fischer/nek_debug/mani/**z.f:83 > 83 utheta = 1.0/(x**2 + y**2)**0.5 > (gdb) > > > This makes sense -- you have a pole singularity in > this formulation. I'm certain it's a removable singularity if you just > rework your ux/uy velocity > definition. > > Please let me know if this resolves the issue. > > Paul > > > > > > On Sun, 14 Aug 2011, nek5000-users at lists.mcs.anl.**govwrote: > > Hi Paul, >> >> I setup a simulation but I keep getting NaN's when I give nontrivial >> initial data. I'm attaching the relevant files. Could you please try it out? >> >> I checked that the initial data is divergence free and satisfies the >> boundary conditions (u_r = 0, du_theta/dr = 0, du_phi/dr = 0). >> >> Regards, >> Mani >> >> On 08/11/2011 05:46 PM, nek5000-users at lists.mcs.anl.**govwrote: >> >>> >>> Hi Mani, >>> >>> Probably your best bet is to use a very thin layer of elements >>> in a 3D spherical shell with SYM bcs on faces 5 & 6, plus the >>> stress formulation. I would imagine that a shell of thickness >>> .001 with R=1.0 might be feasible. >>> >>> Instructions for constructing a 3D shell can be found in >>> www.mcs.anl.gov/~fischer/**primer.pdf >>> >>> (Some of this info may already have been transferred into >>> current manual.) We can help with this if you need any >>> assistance. >>> >>> Regards, >>> >>> Paul >>> >>> >>> On Thu, 11 Aug 2011, nek5000-users at lists.mcs.anl.**govwrote: >>> >>> Hi Nek devs, >>>> >>>> Is it possible to use NEK to solve for Navier Stokes equations on the >>>> surface of a sphere, where r is fixed and the velocity varies in theta >>>> and >>>> phi? >>>> >>>> Thanks, >>>> Mani Chandra >>>> ______________________________**_________________ >>>> 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: -------------- next part -------------- A non-text attachment was scrubbed... Name: shell.rea Type: application/octet-stream Size: 30206 bytes Desc: not available URL: From nek5000-users at lists.mcs.anl.gov Sun Aug 14 07:57:38 2011 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 14 Aug 2011 18:27:38 +0530 Subject: [Nek5000-users] Solving for fluid flows on a sphere In-Reply-To: References: <5fb20c0abcda26f44ece832f761c8e18.squirrel@webmail.iitk.ac.in> <4E476861.5030201@gmail.com> Message-ID: Sorry, I should have attached the .usr file instead of the .rea file. On Sun, Aug 14, 2011 at 6:26 PM, Mani Chandra wrote: > Hi Paul, > > Thanks for the diagnosing this problem. Indeed it is bad initial data. At > the moment I do not have specific initial data or forcing to work with and > so I'm just trying out the feasibility of using NEK to solve on the shell. I > should have some concrete initial data in the next couple of days. > > When I try to repeat the run with > > ux = 0.0 > uy = 0.0 > uz = 0.0 > > and > > ffx = 0.0 > ffy = 0.0 > ffz = 1.0 > > NEK shows a lot of convergence errors. Could you check this out? > > I've attached the .rea file. > > Thanks, > Mani > > > On Sun, Aug 14, 2011 at 5:31 PM, wrote: > >> >> Hi Mani, >> >> I ran this with >> >> G="-g -Ktrap=fp" >> >> and the "nekd" script in serial (just gdb nek5000 after >> setting up requisite files). >> >> Here is the output: >> >> Program received signal SIGFPE, Arithmetic exception. >> 0x000000000040376c in useric_ (ix=1, iy=1, iz=1, ieg=3) >> at /homes/fischer/nek_debug/mani/**z.f:83 >> 83 utheta = 1.0/(x**2 + y**2)**0.5 >> (gdb) >> >> >> This makes sense -- you have a pole singularity in >> this formulation. I'm certain it's a removable singularity if you just >> rework your ux/uy velocity >> definition. >> >> Please let me know if this resolves the issue. >> >> Paul >> >> >> >> >> >> On Sun, 14 Aug 2011, nek5000-users at lists.mcs.anl.**govwrote: >> >> Hi Paul, >>> >>> I setup a simulation but I keep getting NaN's when I give nontrivial >>> initial data. I'm attaching the relevant files. Could you please try it out? >>> >>> I checked that the initial data is divergence free and satisfies the >>> boundary conditions (u_r = 0, du_theta/dr = 0, du_phi/dr = 0). >>> >>> Regards, >>> Mani >>> >>> On 08/11/2011 05:46 PM, nek5000-users at lists.mcs.anl.**govwrote: >>> >>>> >>>> Hi Mani, >>>> >>>> Probably your best bet is to use a very thin layer of elements >>>> in a 3D spherical shell with SYM bcs on faces 5 & 6, plus the >>>> stress formulation. I would imagine that a shell of thickness >>>> .001 with R=1.0 might be feasible. >>>> >>>> Instructions for constructing a 3D shell can be found in >>>> www.mcs.anl.gov/~fischer/**primer.pdf >>>> >>>> (Some of this info may already have been transferred into >>>> current manual.) We can help with this if you need any >>>> assistance. >>>> >>>> Regards, >>>> >>>> Paul >>>> >>>> >>>> On Thu, 11 Aug 2011, nek5000-users at lists.mcs.anl.**govwrote: >>>> >>>> Hi Nek devs, >>>>> >>>>> Is it possible to use NEK to solve for Navier Stokes equations on the >>>>> surface of a sphere, where r is fixed and the velocity varies in theta >>>>> and >>>>> phi? >>>>> >>>>> Thanks, >>>>> Mani Chandra >>>>> ______________________________**_________________ >>>>> 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: -------------- next part -------------- A non-text attachment was scrubbed... Name: shell.usr Type: application/octet-stream Size: 2857 bytes Desc: not available URL: From nek5000-users at lists.mcs.anl.gov Tue Aug 16 17:19:23 2011 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 16 Aug 2011 17:19:23 -0500 Subject: [Nek5000-users] Error stemming from genbox In-Reply-To: References: Message-ID: Hi, This has been fixed and the repo updated. Thanks! Katie On Fri, Aug 12, 2011 at 8:19 AM, wrote: > Thanks for looking into it Katie! > > Josh > > On Thu, Aug 11, 2011 at 3:56 PM, wrote: > > HI Josh, > > > > Yes, the current version of genbox should be set up to set the logical > flags > > a little differently than before. > > > > Now, the user is able to create a .rea file for heat only simulations by > > setting the number of fields (line 3 in the .box file) to negative, so > part > > of the logical flags are written out differently than before. > > > > However, it shouldn't overwrite the IFTRAN logical, that is an error. I > > will take care of it and update the repo. > > > > Thanks!! > > Katie > > > > On Thu, Aug 11, 2011 at 3:15 PM, > wrote: > >> > >> Neks, > >> > >> I was getting an odd error in Nek when using geometry generated from > >> the newest version of genbox (repo 718) that I did not get from repo > >> 713 (the log file from the run using genbox from repo 718 is > >> attached--the error message appears at the top). > >> > >> After comparing the two generated .rea files, I found the issue. On > >> older versions of genbox, it seems that it took the base.rea file > >> specified and used the upper portion of it to generate the header of > >> your new .rea file. But, on the new version, it doesn't appear to do > >> this for the logical flags. So, the issue I was running into (while > >> running the example turbChannel) was that > >> > >> IFTRAN T > >> > >> in base.rea was being replaced by > >> > >> IFHEAT F > >> > >> in the generated box.rea file, where in the older version it kept them > >> the same. Manually changing IFHEAT F back to IFTRAN T > >> removed the error message and the case ran fine as normal. > >> > >> I'm not sure if this was an intentional change or not, or if anyone > >> else has run into this issue, but I thought this might help clear up > >> any confusion if anyone else runs into this same problem (took me a > >> while to figure out what exactly was going wrong :) ). > >> > >> -- > >> Josh Camp > >> > >> "All that is necessary for the triumph of evil is that good men do > >> nothing" -- Edmund Burke > >> > >> _______________________________________________ > >> 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 > > > > > > > > -- > Josh Camp > > "All that is necessary for the triumph of evil is that good men do > nothing" -- Edmund Burke > _______________________________________________ > 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: