From nek5000-users at lists.mcs.anl.gov Wed Mar 1 04:18:35 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 1 Mar 2017 11:18:35 +0100 Subject: [Nek5000-users] Nek: abnormal termination by signal 11 In-Reply-To: References: Message-ID: The stenosis example is working fine with a restart. I found an older case from a few months ago that is still working fine, so I copied its .usr file to one of the new cases and it still failed, so I am suspecting that the error might be related to the grid. The parameters in the rea file are also largely the same. > Am 27.02.2017 um 11:31 schrieb nek5000-users at lists.mcs.anl.gov: > > I think this is somehow related to your case. Can you reproduce the SEGFAULT with say the pipe/stenosis example doing a restart? > > > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Wed Mar 1 16:32:41 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 01 Mar 2017 23:32:41 +0100 Subject: [Nek5000-users] Azimutal velocity on axisymmetric simulation Message-ID: Hi all, I have been running an axisymmetric case for some time now tricking the temperature array into storing azimutal velocity data (IFHEAT T, IFAZIV T). Right now, I have an initial condition on "temperature" of 1.0E-12 so that it is not zero and the results I have been getting are not consistent in a way where I can run the same case (same ".rea", same ".usr", same "SIZE") and get two very different results for the "temperature" field: either it diverges very quickly (around 30th time step) and shows "Inf" or it stays at around 1.0E-12 with some minor perturbations for the rest of the simulation. Just to be clear, simply stopping the simulation and re-running it from t=0 will "switch" between those two results. Any advice will be appreciated, MViturro From nek5000-users at lists.mcs.anl.gov Fri Mar 3 06:02:34 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 3 Mar 2017 13:02:34 +0100 Subject: [Nek5000-users] Problem with Spatial Derivatives of field Message-ID: Hi Neks, I'm having some problems with computing the gradients of vorticity. So what I do in the usercheck is something like : call call comp_vort3(vort,work1,work2,vxp,vyp,vzp) ! Computing vorticity of perturbations call gradm1(derivvortx,derivvorty,derivvortz,vort(1,1)) However, by doing this I do observe some abnormal results when I plot the fields : derivvortx, derivvorty, derivvortz. Attached you will find a snapshot of the magnitude of derivvortx and derivvorty (obtained using paraview) I am wondering why I am having extremely high values a the boudary of the elements. Has anyone noticed or faced such a problem? Even when I increase lx1, reduce dt and reduce the mesh size, the problem remains.. Thank you for your time, Best wishes, Arnold -- *Arnold Wakim* Doctorant, D?partement d?A?rodynamique Fondamentale et Exp?rimentale T?l: +33 1 46 23 51 83 ONERA - The French Aerospace Lab -Centre de Meudon 8, rue des Vertugadins - 92190 MEUDON Nous suivre sur : www.onera.fr | Twitter | LinkedIn | Facebook -------------- next part -------------- An HTML attachment was scrubbed... URL: -------------- next part -------------- A non-text attachment was scrubbed... Name: Image1 Type: image/jpeg Size: 2151 bytes Desc: not available URL: -------------- next part -------------- A non-text attachment was scrubbed... Name: magnitude_of_gradient.png Type: image/png Size: 162126 bytes Desc: not available URL: From nek5000-users at lists.mcs.anl.gov Fri Mar 3 06:32:10 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 3 Mar 2017 12:32:10 +0000 Subject: [Nek5000-users] Problem with Spatial Derivatives of field In-Reply-To: References: Message-ID: Hi Arnold, The velocity is only in C^0, which means it is continuous. The first derivative is defined everywhere, but is discontinuous, meaning that the vorticity is discontinuous. The derivative of the vorticity involves the second derivative of velocity, and this is not defined. All that being said, the vorticity will converge to a continuous function exponentially fast with increasing polynomial order. So if you want to differentiate the vorticity you have the option of increasing the polynomial order. Alternatively, you can try to regularize the vorticity prior to differentiating it. A common strategy is to call dsavg( . ) for each component of vorticity -- which makes it continuous, but this wouldn't necessarily make the derivatives better. Other alternatives would be to use a combination of dsavg() and some type of low-pass filtering, e.g., by solving a Helmholtz problem of the form (I-L^2 \nabla^2) vbar = v, where L is the filter length. Another option is to look at the context in which you want to use your differentiated vorticity. Perhaps this can be recast in a weak form, in which one of the derivatives is moved onto the (continuous and differentiable) test functions, etc. hth, 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, March 03, 2017 6:02 AM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] Problem with Spatial Derivatives of field Hi Neks, I'm having some problems with computing the gradients of vorticity. So what I do in the usercheck is something like : call call comp_vort3(vort,work1,work2,vxp,vyp,vzp) ! Computing vorticity of perturbations call gradm1(derivvortx,derivvorty,derivvortz,vort(1,1)) However, by doing this I do observe some abnormal results when I plot the fields : derivvortx, derivvorty, derivvortz. Attached you will find a snapshot of the magnitude of derivvortx and derivvorty (obtained using paraview) I am wondering why I am having extremely high values a the boudary of the elements. Has anyone noticed or faced such a problem? Even when I increase lx1, reduce dt and reduce the mesh size, the problem remains.. Thank you for your time, Best wishes, Arnold -- [cid:part1.AAFA1EB3.C1F7AC72 at onera.fr]Arnold Wakim Doctorant, D?partement d?A?rodynamique Fondamentale et Exp?rimentale T?l: +33 1 46 23 51 83 ONERA - The French Aerospace Lab -Centre de Meudon 8, rue des Vertugadins - 92190 MEUDON Nous suivre sur : www.onera.fr | Twitter | LinkedIn | Facebook -------------- next part -------------- An HTML attachment was scrubbed... URL: -------------- next part -------------- A non-text attachment was scrubbed... Name: Image1 Type: image/jpeg Size: 2151 bytes Desc: Image1 URL: From nek5000-users at lists.mcs.anl.gov Fri Mar 3 06:54:02 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 3 Mar 2017 12:54:02 +0000 Subject: [Nek5000-users] Azimutal velocity on axisymmetric simulation In-Reply-To: References: Message-ID: Have you tried starting with the vortex2 case? It is axisymmetric, with swirl. I've just verified that it is working correctly with the current repo version of the code (and all previous versions, as far as I'm aware). 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, March 01, 2017 4:32 PM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] Azimutal velocity on axisymmetric simulation Hi all, I have been running an axisymmetric case for some time now tricking the temperature array into storing azimutal velocity data (IFHEAT T, IFAZIV T). Right now, I have an initial condition on "temperature" of 1.0E-12 so that it is not zero and the results I have been getting are not consistent in a way where I can run the same case (same ".rea", same ".usr", same "SIZE") and get two very different results for the "temperature" field: either it diverges very quickly (around 30th time step) and shows "Inf" or it stays at around 1.0E-12 with some minor perturbations for the rest of the simulation. Just to be clear, simply stopping the simulation and re-running it from t=0 will "switch" between those two results. Any advice will be appreciated, MViturro _______________________________________________ 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 Mar 3 14:33:19 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 03 Mar 2017 14:33:19 -0600 Subject: [Nek5000-users] Problem with Spatial Derivatives of field In-Reply-To: References: Message-ID: Hi Arnold, I looked into this issue some when I was trying to calculate the curvature of some of my temperature isosurfaces. Aleks Obabko suggested that I tried smoothing the derivatives across the element boundaries. So basically, I tried doing this: ! Calculate the gradient of the temperature field ! This derivative will be continuous within the element, but there will be jumps across the element boundaries call gradm1(dTdx, dTdy, dTdz, t) ! Smooth the derivative (dT/dx) so that it is continuous across the element boundaries. call col2(dTdx,bm1,n) ! collocate with the mass matrix call dssum(dTdx,nx1,ny1,nz1) ! smooth call col2(dTdx,bintm1,n) ! collocate with the inverse mass matrix (Note: dssum just returns the sum of the shared GLL points across the element boundaries.) I ran a test case, and I found that, in that case, this procedure does generate good first and second derivatives. The test case was basically just an artificial sphere that I set up in Nek5000. The temperature varied with the radius of the sphere, and my goal was to calculate smooth first and second derivatives of the temperature so that I could accurately calculate the curvature of the sphere. I looked at some comparisons between the calculated first and second derivatives and the analytical solution. Generally, the accuracy was good given the pretty low resolution that I was using. (However, in order to find the curvature, I needed to multiply, raise to powers, and divide the derivatives, so that ultimately the relatively small derivative errors were magnified into unacceptably large curvature errors.) So, ultimately, I think that this smoothing procedure should definitely work well enough for most (but not all) purposes. If you just want smooth derivatives for visualization, or you just want to measure just the derivative itself, this will probably work. In your case of looking at the derivatives of the vorticity, you could try doing this two ways and see which one works better. 1) Calculate the vorticity, smooth the vorticity, take the derivative, then smooth the derivative 2) Calculate the vorticity, take the derivative, smooth the derivative The first option has more smoothing steps, but the second option preserves the representation of the vorticity within the element as you take the derivative. Aleks generally recommends the second option. What do you need the derivatives of the vorticity for exactly? Depending on your end goal, one of the methods Paul suggested may work better than this one. Elizabeth On 03/03/2017 06:32 AM, nek5000-users at lists.mcs.anl.gov wrote: > > Hi Arnold, > > The velocity is only in C^0, which means it is continuous. The first > derivative > is defined everywhere, but is discontinuous, meaning that the vorticity is > discontinuous. > > The derivative of the vorticity involves the second derivative of > velocity, and this > is not defined. > > All that being said, the vorticity will converge to a continuous > function exponentially > fast with increasing polynomial order. So if you want to > differentiate the vorticity > you have the option of increasing the polynomial order. > > Alternatively, you can try to regularize the vorticity prior to > differentiating it. > A common strategy is to call dsavg( . ) for each component of > vorticity -- which > makes it continuous, but this wouldn't necessarily make the > derivatives better. > Other alternatives would be to use a combination of dsavg() and some > type of > low-pass filtering, e.g., by solving a Helmholtz problem of the form > (I-L^2 \nabla^2) vbar = v, > where L is the filter length. Another option is to look at the > context in which > you want to use your differentiated vorticity. Perhaps this can be > recast in a weak > form, in which one of the derivatives is moved onto the (continuous > and differentiable) > test functions, etc. > > hth, > > 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, March 03, 2017 6:02 AM > *To:* nek5000-users at lists.mcs.anl.gov > *Subject:* [Nek5000-users] Problem with Spatial Derivatives of field > > Hi Neks, > > I'm having some problems with computing the gradients of vorticity. > > So what I do in the usercheck is something like : > > > > call call comp_vort3(vort,work1,work2,vxp,vyp,vzp) ! Computing > vorticity of perturbations > > call gradm1(derivvortx,derivvorty,derivvortz,vort(1,1)) > > > > However, by doing this I do observe some abnormal results when I plot > the fields : derivvortx, derivvorty, derivvortz. > > Attached you will find a snapshot of the magnitude of derivvortx and > derivvorty (obtained using paraview) > > I am wondering why I am having extremely high values a the boudary of > the elements. Has anyone noticed or faced such a problem? > > > Even when I increase lx1, reduce dt and reduce the mesh size, the > problem remains.. > > > Thank you for your time, > > Best wishes, > > > Arnold > > > > > -- > > *Arnold Wakim* > Doctorant, > D?partement d?A?rodynamique Fondamentale et Exp?rimentale > T?l: +33 1 46 23 51 83 > > > ONERA - The French Aerospace Lab -Centre de Meudon > 8, rue des Vertugadins - 92190 MEUDON > > Nous suivre sur : www.onera.fr | Twitter > | LinkedIn > | Facebook > > > > > _______________________________________________ > 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: Image1 Type: image/jpeg Size: 2151 bytes Desc: not available URL: From nek5000-users at lists.mcs.anl.gov Mon Mar 6 00:38:19 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 6 Mar 2017 07:38:19 +0100 Subject: [Nek5000-users] Problem with Spatial Derivatives of field In-Reply-To: References: Message-ID: Good Morning, Sorry for taking so long to answer. First I wanted to say that I really appreciate all of your help! I am currently trying all these methods : - as suggested by Paul Fischer, increasing LX1 and low pass filtering. - and smoothing the derivatives. I will keep you posted on the results. What I am trying to do is studying optimal perturbations using a DIRECT-ADJOINT approach so as to optimize quantities. However, when I am writing the equations, I have no choice but taking the spatial derivatives of vorticity. Computing the derivatives is made for every DIRECT Numerical Simulation of the perturbations. Then I call the ADJOINT solver of Nek5000 In order to converge towards optimum this may take several iterations let's say N ( roughly N=10 however since the gradients are not well resolved then I cannot tell whether I'm converged or not). The point is that I am computing vorticity, then computing the gradients of the same initial field, and this, N times. This leads to the problem I am facing. Hope that helps understanding the issue. If you have more questions, please do not hesitate to ask. Best wishes, Arnold Le 03/03/2017 ? 21:33, nek5000-users at lists.mcs.anl.gov a ?crit : > call col2(dTdx,bm1,n) ! collocate with the mass matrix > call dssum(dTdx,nx1,ny1,nz1) ! smooth > call col2(dTdx,bintm1,n) ! collocate with the inverse > mass matrix -- *Arnold Wakim* Doctorant, D?partement d?A?rodynamique Fondamentale et Exp?rimentale T?l: +33 1 46 23 51 83 ONERA - The French Aerospace Lab -Centre de Meudon 8, rue des Vertugadins - 92190 MEUDON Nous suivre sur : www.onera.fr | Twitter | LinkedIn | Facebook -------------- next part -------------- An HTML attachment was scrubbed... URL: -------------- next part -------------- A non-text attachment was scrubbed... Name: Image1 Type: image/jpeg Size: 2151 bytes Desc: not available URL: From nek5000-users at lists.mcs.anl.gov Mon Mar 6 04:31:35 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 6 Mar 2017 11:31:35 +0100 Subject: [Nek5000-users] Nek: abnormal termination by signal 11 In-Reply-To: References: Message-ID: Hello again, after some more trying around I got some of my cases to work again by doing a complete reset of the simulations - I was slowly increasing a forcing parameter, and by starting at zero again it seemed to work this time. Other simulations are still failing, even with the new Nek version 17.0. I directly copy the case folders between the clusters and only change the compilers in makenek and number of processors in SIZE, but the cases still work on Intel but fail on IBM. > Am 01.03.2017 um 11:18 schrieb nek5000-users at lists.mcs.anl.gov: > > The stenosis example is working fine with a restart. I found an older case from a few months ago that is still working fine, so I copied its .usr file to one of the new cases and it still failed, so I am suspecting that the error might be related to the grid. The parameters in the rea file are also largely the same. > > _______________________________________________ > 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 Mar 6 21:15:53 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 7 Mar 2017 03:15:53 +0000 Subject: [Nek5000-users] Nek: abnormal termination by signal 11 In-Reply-To: References: , Message-ID: Hi Jan, Sorry if you've already answered this question Which machine are you running on? 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 06, 2017 4:31 AM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 Hello again, after some more trying around I got some of my cases to work again by doing a complete reset of the simulations - I was slowly increasing a forcing parameter, and by starting at zero again it seemed to work this time. Other simulations are still failing, even with the new Nek version 17.0. I directly copy the case folders between the clusters and only change the compilers in makenek and number of processors in SIZE, but the cases still work on Intel but fail on IBM. > Am 01.03.2017 um 11:18 schrieb nek5000-users at lists.mcs.anl.gov: > > The stenosis example is working fine with a restart. I found an older case from a few months ago that is still working fine, so I copied its .usr file to one of the new cases and it still failed, so I am suspecting that the error might be related to the grid. The parameters in the rea file are also largely the same. > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Tue Mar 7 01:31:03 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 7 Mar 2017 08:31:03 +0100 Subject: [Nek5000-users] Nek: abnormal termination by signal 11 In-Reply-To: References: Message-ID: Hello Paul, I?m working on the Juqueen IBM BlueGene/Q in Juelich. (http://www.fz-juelich.de/ias/jsc/EN/Expertise/Supercomputers/JUQUEEN/Configuration/Configuration_node.html) Jan > Am 07.03.2017 um 04:15 schrieb nek5000-users at lists.mcs.anl.gov: > > > Hi Jan, > > Sorry if you've already answered this question Which machine are you running on? > > 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 06, 2017 4:31 AM > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 > > Hello again, > after some more trying around I got some of my cases to work again by doing a complete reset of the simulations - I was slowly increasing a forcing parameter, and by starting at zero again it seemed to work this time. Other simulations are still failing, even with the new Nek version 17.0. I directly copy the case folders between the clusters and only change the compilers in makenek and number of processors in SIZE, but the cases still work on Intel but fail on IBM. > >> Am 01.03.2017 um 11:18 schrieb nek5000-users at lists.mcs.anl.gov: >> >> The stenosis example is working fine with a restart. I found an older case from a few months ago that is still working fine, so I copied its .usr file to one of the new cases and it still failed, so I am suspecting that the error might be related to the grid. The parameters in the rea file are also largely the same. >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Tue Mar 7 07:17:56 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 7 Mar 2017 13:17:56 +0000 Subject: [Nek5000-users] Nek: abnormal termination by signal 11 In-Reply-To: References: , Message-ID: Hi Jan, I don't know if this helps, but this is the makenek script I use on BGQ. Paul ________________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Tuesday, March 07, 2017 1:31 AM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 Hello Paul, I?m working on the Juqueen IBM BlueGene/Q in Juelich. (http://www.fz-juelich.de/ias/jsc/EN/Expertise/Supercomputers/JUQUEEN/Configuration/Configuration_node.html) Jan > Am 07.03.2017 um 04:15 schrieb nek5000-users at lists.mcs.anl.gov: > > > Hi Jan, > > Sorry if you've already answered this question Which machine are you running on? > > 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 06, 2017 4:31 AM > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 > > Hello again, > after some more trying around I got some of my cases to work again by doing a complete reset of the simulations - I was slowly increasing a forcing parameter, and by starting at zero again it seemed to work this time. Other simulations are still failing, even with the new Nek version 17.0. I directly copy the case folders between the clusters and only change the compilers in makenek and number of processors in SIZE, but the cases still work on Intel but fail on IBM. > >> Am 01.03.2017 um 11:18 schrieb nek5000-users at lists.mcs.anl.gov: >> >> The stenosis example is working fine with a restart. I found an older case from a few months ago that is still working fine, so I copied its .usr file to one of the new cases and it still failed, so I am suspecting that the error might be related to the grid. The parameters in the rea file are also largely the same. >> >> _______________________________________________ >> 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 -------------- A non-text attachment was scrubbed... Name: makenek.bgq Type: application/octet-stream Size: 2381 bytes Desc: makenek.bgq URL: From nek5000-users at lists.mcs.anl.gov Tue Mar 7 07:21:28 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 7 Mar 2017 14:21:28 +0100 Subject: [Nek5000-users] Nek: abnormal termination by signal 11 In-Reply-To: References: Message-ID: I don't think his problem is related to compiler settings. The default should just work. Also it looks like it's a case specific problem as the NekExamples run fine. -----Original message----- > From:nek5000-users at lists.mcs.anl.gov > Sent: Tuesday 7th March 2017 14:18 > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 > > > Hi Jan, > > I don't know if this helps, but this is the makenek script I use on BGQ. > > Paul > > ________________________________________ > From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > Sent: Tuesday, March 07, 2017 1:31 AM > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 > > Hello Paul, > I?m working on the Juqueen IBM BlueGene/Q in Juelich. (http://www.fz-juelich.de/ias/jsc/EN/Expertise/Supercomputers/JUQUEEN/Configuration/Configuration_node.html) > Jan > > Am 07.03.2017 um 04:15 schrieb nek5000-users at lists.mcs.anl.gov: > > > > > > Hi Jan, > > > > Sorry if you've already answered this question Which machine are you running on? > > > > 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 06, 2017 4:31 AM > > To: nek5000-users at lists.mcs.anl.gov > > Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 > > > > Hello again, > > after some more trying around I got some of my cases to work again by doing a complete reset of the simulations - I was slowly increasing a forcing parameter, and by starting at zero again it seemed to work this time. Other simulations are still failing, even with the new Nek version 17.0. I directly copy the case folders between the clusters and only change the compilers in makenek and number of processors in SIZE, but the cases still work on Intel but fail on IBM. > > > >> Am 01.03.2017 um 11:18 schrieb nek5000-users at lists.mcs.anl.gov: > >> > >> The stenosis example is working fine with a restart. I found an older case from a few months ago that is still working fine, so I copied its .usr file to one of the new cases and it still failed, so I am suspecting that the error might be related to the grid. The parameters in the rea file are also largely the same. > >> > >> _______________________________________________ > >> Nek5000-users mailing list > >> Nek5000-users at lists.mcs.anl.gov > >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > > _______________________________________________ > > Nek5000-users mailing list > > Nek5000-users at lists.mcs.anl.gov > > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > _______________________________________________ > > Nek5000-users mailing list > > Nek5000-users at lists.mcs.anl.gov > > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > From nek5000-users at lists.mcs.anl.gov Tue Mar 7 13:55:32 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 7 Mar 2017 20:55:32 +0100 Subject: [Nek5000-users] VISIT visnek skip some timesteps Message-ID: Dear Neks, I generate blah0.00001, blah0.00002, .....blah0.f00101 on a remote computer. But, I transfer only blah0.f0*1 because of slow transfer speeds. When I run visit, it throw error from the second frame (timestep) Can someone kindly let me know how should the blah.nek5000 file be modified in order to visualize in VISIT? When I transfer all the files there is no problem in running VISIT. Thank you in advance. -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Mar 7 14:01:22 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 7 Mar 2017 21:01:22 +0100 Subject: [Nek5000-users] VISIT visnek skip some timesteps In-Reply-To: References: Message-ID: Hi, you can change the total number of time steps in the blah.nek5000 file. The example from the documentation for this case is: NEK5000 version: 1.0 filetemplate: example%02d.f%04d firsttimestep: 1 numtimesteps: 1 > Am 07.03.2017 um 20:55 schrieb nek5000-users at lists.mcs.anl.gov: > > Dear Neks, > I generate blah0.00001, blah0.00002, .....blah0.f00101 on a remote computer. But, I transfer only blah0.f0*1 because of slow transfer speeds. When I run visit, it throw error from the second frame (timestep) > Can someone kindly let me know how should the blah.nek5000 file be modified in order to visualize in VISIT? > When I transfer all the files there is no problem in running VISIT. > Thank you in advance. > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Mar 7 14:09:39 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 7 Mar 2017 20:09:39 +0000 Subject: [Nek5000-users] VISIT visnek skip some timesteps In-Reply-To: References: , Message-ID: I suspect that you can open only first file you transferred blah0.00001 To open the rest of file in VisIt, I typically create a separate file with sequentially numbered files *01, *02, etc. that point/link to the original transferred non-sequentially-numbered files Aleks ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Tuesday, March 07, 2017 2:01 PM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] VISIT visnek skip some timesteps Hi, you can change the total number of time steps in the blah.nek5000 file. The example from the documentation for this case is: NEK5000 version: 1.0 filetemplate: example%02d.f%04d firsttimestep: 1 numtimesteps: 1 Am 07.03.2017 um 20:55 schrieb nek5000-users at lists.mcs.anl.gov: Dear Neks, I generate blah0.00001, blah0.00002, .....blah0.f00101 on a remote computer. But, I transfer only blah0.f0*1 because of slow transfer speeds. When I run visit, it throw error from the second frame (timestep) Can someone kindly let me know how should the blah.nek5000 file be modified in order to visualize in VISIT? When I transfer all the files there is no problem in running VISIT. Thank you in advance. _______________________________________________ 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 Mar 8 05:32:31 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 8 Mar 2017 19:32:31 +0800 (GMT+08:00) Subject: [Nek5000-users] how to dumping velocity data in each processor to file Message-ID: hi, all I'm trying to write down velocity in each processor into files. Below is an sample in the subroutine userchk: open(unit=80,file='result.dat') write(80,*) 'x, y, z, u, v, z, p' do e=1,nelv do k=1,lz1 do j=1,ly1 do i=1,lx1 write(80,1) xm1(i,j,k,e),ym1(i,j,k,e),zm1(i,j,k,e), & vx(i,j,k,e),vy(i,j,k,e),vz(i,j,k,e),pr(i,j,k,e) enddo enddo enddo enddo 1 format(1p15e17.9) But in this case ,I can get the data only in one processor. When I use more than one processor, how to get velocity in all processors? Best regards! Hu -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Mar 8 18:36:24 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 8 Mar 2017 17:36:24 -0700 Subject: [Nek5000-users] how to dumping velocity data in each processor to file In-Reply-To: References: Message-ID: Hi Hu, Is there any specific reason why you cant use the outpost routine. call outpost(vx,vy,vz,pr,t,'his') might be a better option. Best Regards, Tanmoy On Wed, Mar 8, 2017 at 4:32 AM, wrote: > hi, all > > I'm trying to write down velocity in each processor into files. Below > is an sample in the subroutine userchk: > > open(unit=80,file='result.dat') > write(80,*) 'x, y, z, u, v, z, p' > do e=1,nelv > do k=1,lz1 > do j=1,ly1 > do i=1,lx1 > write(80,1) xm1(i,j,k,e),ym1(i,j,k,e),zm1(i,j,k,e), > & vx(i,j,k,e),vy(i,j,k,e),vz(i,j,k,e),pr(i,j,k,e) > enddo > enddo > enddo > enddo > 1 format(1p15e17.9) > > But in this case ,I can get the data only in one processor. When I use > more than one processor, how to get velocity in all processors? > > > > Best regards! > > Hu > > _______________________________________________ > 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 Mar 8 20:27:46 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 9 Mar 2017 10:27:46 +0800 (GMT+08:00) Subject: [Nek5000-users] how to dumping velocity data in each processor to file In-Reply-To: References: Message-ID: Hi Tanmoy, Thanks! In fact I can use the outpost routine, but I don't know how to read the hisxxxx.f0001 file except by VisIt . I want to write down the data in a familar format so that I can handle it very easy. Or can I transform the outpost format into ASCII that I can also read it easy? Best regards! Hu -----Original Messages----- From: nek5000-users at lists.mcs.anl.gov Sent Time: Thursday, March 9, 2017 To: nek5000-users at lists.mcs.anl.gov Cc: Subject: Re: [Nek5000-users] how to dumping velocity data in each processor to file Hi Hu, Is there any specific reason why you cant use the outpost routine. call outpost(vx,vy,vz,pr,t,'his') might be a better option. Best Regards, Tanmoy On Wed, Mar 8, 2017 at 4:32 AM, wrote: hi, all I'm trying to write down velocity in each processor into files. Below is an sample in the subroutine userchk: open(unit=80,file='result.dat') write(80,*) 'x, y, z, u, v, z, p' do e=1,nelv do k=1,lz1 do j=1,ly1 do i=1,lx1 write(80,1) xm1(i,j,k,e),ym1(i,j,k,e),zm1(i,j,k,e), & vx(i,j,k,e),vy(i,j,k,e),vz(i,j,k,e),pr(i,j,k,e) enddo enddo enddo enddo 1 format(1p15e17.9) But in this case ,I can get the data only in one processor. When I use more than one processor, how to get velocity in all processors? Best regards! Hu _______________________________________________ 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 Mar 8 22:14:42 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 9 Mar 2017 04:14:42 +0000 Subject: [Nek5000-users] how to dumping velocity data in each processor to file In-Reply-To: References: , Message-ID: You can set param(66)=0 in usrdat2: param(66)=0 this will cause the output to be in ascii, in a .fld file... I wouldn't recommend this for large parallel cases, however, as the ascii output is not fast. 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, March 08, 2017 8:27 PM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] how to dumping velocity data in each processor to file Hi Tanmoy, Thanks! In fact I can use the outpost routine, but I don't know how to read the hisxxxx.f0001 file except by VisIt . I want to write down the data in a familar format so that I can handle it very easy. Or can I transform the outpost format into ASCII that I can also read it easy? Best regards! Hu -----Original Messages----- From: nek5000-users at lists.mcs.anl.gov Sent Time: Thursday, March 9, 2017 To: nek5000-users at lists.mcs.anl.gov Cc: Subject: Re: [Nek5000-users] how to dumping velocity data in each processor to file Hi Hu, Is there any specific reason why you cant use the outpost routine. call outpost(vx,vy,vz,pr,t,'his') might be a better option. Best Regards, Tanmoy On Wed, Mar 8, 2017 at 4:32 AM, > wrote: hi, all I'm trying to write down velocity in each processor into files. Below is an sample in the subroutine userchk: open(unit=80,file='result.dat') write(80,*) 'x, y, z, u, v, z, p' do e=1,nelv do k=1,lz1 do j=1,ly1 do i=1,lx1 write(80,1) xm1(i,j,k,e),ym1(i,j,k,e),zm1(i,j,k,e), & vx(i,j,k,e),vy(i,j,k,e),vz(i,j,k,e),pr(i,j,k,e) enddo enddo enddo enddo 1 format(1p15e17.9) But in this case ,I can get the data only in one processor. When I use more than one processor, how to get velocity in all processors? Best regards! Hu _______________________________________________ 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 Mar 9 04:46:59 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 9 Mar 2017 18:46:59 +0800 (GMT+08:00) Subject: [Nek5000-users] how to dumping velocity data in each processor to file In-Reply-To: References: , Message-ID: Thanks Paul! I'll try. Best regards! Hu -----Original Messages----- From: nek5000-users at lists.mcs.anl.gov Sent Time: Thursday, March 9, 2017 To: "nek5000-users at lists.mcs.anl.gov" Cc: Subject: Re: [Nek5000-users] how to dumping velocity data in each processor to file You can set param(66)=0 in usrdat2: param(66)=0 this will cause the output to be in ascii, in a .fld file... I wouldn't recommend this for large parallel cases, however, as the ascii output is not fast. 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, March 08, 2017 8:27 PM To:nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] how to dumping velocity data in each processor to file Hi Tanmoy, Thanks! In fact I can use the outpost routine, but I don't know how to read the hisxxxx.f0001 file except by VisIt . I want to write down the data in a familar format so that I can handle it very easy. Or can I transform the outpost format into ASCII that I can also read it easy? Best regards! Hu -----Original Messages----- From:nek5000-users at lists.mcs.anl.gov Sent Time: Thursday, March 9, 2017 To:nek5000-users at lists.mcs.anl.gov Cc: Subject: Re: [Nek5000-users] how to dumping velocity data in each processor to file Hi Hu, Is there any specific reason why you cant use the outpost routine. call outpost(vx,vy,vz,pr,t,'his') might be a better option. Best Regards, Tanmoy On Wed, Mar 8, 2017 at 4:32 AM, wrote: hi, all I'm trying to write down velocity in each processor into files. Below is an sample in the subroutine userchk: open(unit=80,file='result.dat') write(80,*) 'x, y, z, u, v, z, p' do e=1,nelv do k=1,lz1 do j=1,ly1 do i=1,lx1 write(80,1) xm1(i,j,k,e),ym1(i,j,k,e),zm1(i,j,k,e), & vx(i,j,k,e),vy(i,j,k,e),vz(i,j,k,e),pr(i,j,k,e) enddo enddo enddo enddo 1 format(1p15e17.9) But in this case ,I can get the data only in one processor. When I use more than one processor, how to get velocity in all processors? Best regards! Hu _______________________________________________ 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 Mar 9 14:38:46 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 9 Mar 2017 15:38:46 -0500 Subject: [Nek5000-users] Compiling nek on Mira (BG/Q) Message-ID: Hi neks, I updated the code to the latest repo on Mira and tried to compile the code with the optimization for the BG/Q system but the code failed to compile. Here is my compiler file: -------------- next part -------------- A non-text attachment was scrubbed... Name: compiler.out Type: application/octet-stream Size: 31818 bytes Desc: not available URL: -------------- next part -------------- There seems to be a problem with the mxm_bgq.f routine. How might I go about fixing this? Thanks, Ravon From nek5000-users at lists.mcs.anl.gov Thu Mar 9 14:48:14 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 9 Mar 2017 20:48:14 +0000 Subject: [Nek5000-users] Compiling nek on Mira (BG/Q) In-Reply-To: References: Message-ID: Hi Ravon, I don't know about bgq_mxm.f , but about 3 days ago I attached my current bgq makenek file to an email posted to this list. Let me know if that works for you... 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, March 09, 2017 2:38 PM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] Compiling nek on Mira (BG/Q) Hi neks, I updated the code to the latest repo on Mira and tried to compile the code with the optimization for the BG/Q system but the code failed to compile. Here is my compiler file: There seems to be a problem with the mxm_bgq.f routine. How might I go about fixing this? Thanks, Ravon _______________________________________________ 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 Mar 9 14:51:38 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 9 Mar 2017 21:51:38 +0100 Subject: [Nek5000-users] Compiling nek on Mira (BG/Q) Message-ID: The BGQ optimization flag is only available for the IBM compilers. It looks like you are using GNU! -----Original message----- > From:nek5000-users at lists.mcs.anl.gov > Sent: Thursday 9th March 2017 21:46 > To: nek5000-users at lists.mcs.anl.gov > Subject: [Nek5000-users] Compiling nek on Mira (BG/Q) > > Hi neks, > I updated the code to the latest repo on Mira and tried to compile the code with the optimization for the BG/Q system > but the code failed to compile. > > Here is my compiler file: > > > There seems to be a problem with the mxm_bgq.f routine. > How might I go about fixing this? > > Thanks, > Ravon_______________________________________________ > 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 Mar 10 06:45:40 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 10 Mar 2017 13:45:40 +0100 Subject: [Nek5000-users] Nek: abnormal termination by signal 11 In-Reply-To: References: Message-ID: Hello, some more testing showed that the error is actually not dependent on the deformation of the grid in usrdat2. It occurs if I use a restart file and at the same time use a lower order lx1 etc. in SIZE. I sometimes do that when I suspect the resolution is too high. Increasing lx1 on the other hand is OK. Again, this error does not occur on an Intel system. The pipe/stenosis example is fine when reducing lx too, but it is also much smaller than my cases (around 10^4 Elements). I will try too find a small case that still reproduces the error. Jan > Am 07.03.2017 um 14:21 schrieb nek5000-users at lists.mcs.anl.gov: > > I don't think his problem is related to compiler settings. The default should just work. > Also it looks like it's a case specific problem as the NekExamples run fine. > > -----Original message----- >> From:nek5000-users at lists.mcs.anl.gov >> Sent: Tuesday 7th March 2017 14:18 >> To: nek5000-users at lists.mcs.anl.gov >> Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 >> >> >> Hi Jan, >> >> I don't know if this helps, but this is the makenek script I use on BGQ. >> >> Paul >> >> ________________________________________ >> From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] >> Sent: Tuesday, March 07, 2017 1:31 AM >> To: nek5000-users at lists.mcs.anl.gov >> Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 >> >> Hello Paul, >> I?m working on the Juqueen IBM BlueGene/Q in Juelich. (http://www.fz-juelich.de/ias/jsc/EN/Expertise/Supercomputers/JUQUEEN/Configuration/Configuration_node.html) >> Jan >>> Am 07.03.2017 um 04:15 schrieb nek5000-users at lists.mcs.anl.gov: >>> >>> >>> Hi Jan, >>> >>> Sorry if you've already answered this question Which machine are you running on? >>> >>> 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 06, 2017 4:31 AM >>> To: nek5000-users at lists.mcs.anl.gov >>> Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 >>> >>> Hello again, >>> after some more trying around I got some of my cases to work again by doing a complete reset of the simulations - I was slowly increasing a forcing parameter, and by starting at zero again it seemed to work this time. Other simulations are still failing, even with the new Nek version 17.0. I directly copy the case folders between the clusters and only change the compilers in makenek and number of processors in SIZE, but the cases still work on Intel but fail on IBM. >>> >>>> Am 01.03.2017 um 11:18 schrieb nek5000-users at lists.mcs.anl.gov: >>>> >>>> The stenosis example is working fine with a restart. I found an older case from a few months ago that is still working fine, so I copied its .usr file to one of the new cases and it still failed, so I am suspecting that the error might be related to the grid. The parameters in the rea file are also largely the same. >>>> >>>> _______________________________________________ >>>> Nek5000-users mailing list >>>> Nek5000-users at lists.mcs.anl.gov >>>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>> >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Fri Mar 10 07:12:20 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 10 Mar 2017 13:12:20 +0000 Subject: [Nek5000-users] Nek: abnormal termination by signal 11 In-Reply-To: References: , Message-ID: Hi Jan, By how much are you reducing your resolution? May I suggest compiling with a larger lelt and then trying ? I think that what is happening when you reduce lx1 is that there is not enough room to hold the restart field... increasing lelt will alleviate this problem. 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, March 10, 2017 6:45 AM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 Hello, some more testing showed that the error is actually not dependent on the deformation of the grid in usrdat2. It occurs if I use a restart file and at the same time use a lower order lx1 etc. in SIZE. I sometimes do that when I suspect the resolution is too high. Increasing lx1 on the other hand is OK. Again, this error does not occur on an Intel system. The pipe/stenosis example is fine when reducing lx too, but it is also much smaller than my cases (around 10^4 Elements). I will try too find a small case that still reproduces the error. Jan > Am 07.03.2017 um 14:21 schrieb nek5000-users at lists.mcs.anl.gov: > > I don't think his problem is related to compiler settings. The default should just work. > Also it looks like it's a case specific problem as the NekExamples run fine. > > -----Original message----- >> From:nek5000-users at lists.mcs.anl.gov >> Sent: Tuesday 7th March 2017 14:18 >> To: nek5000-users at lists.mcs.anl.gov >> Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 >> >> >> Hi Jan, >> >> I don't know if this helps, but this is the makenek script I use on BGQ. >> >> Paul >> >> ________________________________________ >> From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] >> Sent: Tuesday, March 07, 2017 1:31 AM >> To: nek5000-users at lists.mcs.anl.gov >> Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 >> >> Hello Paul, >> I?m working on the Juqueen IBM BlueGene/Q in Juelich. (http://www.fz-juelich.de/ias/jsc/EN/Expertise/Supercomputers/JUQUEEN/Configuration/Configuration_node.html) >> Jan >>> Am 07.03.2017 um 04:15 schrieb nek5000-users at lists.mcs.anl.gov: >>> >>> >>> Hi Jan, >>> >>> Sorry if you've already answered this question Which machine are you running on? >>> >>> 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 06, 2017 4:31 AM >>> To: nek5000-users at lists.mcs.anl.gov >>> Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 >>> >>> Hello again, >>> after some more trying around I got some of my cases to work again by doing a complete reset of the simulations - I was slowly increasing a forcing parameter, and by starting at zero again it seemed to work this time. Other simulations are still failing, even with the new Nek version 17.0. I directly copy the case folders between the clusters and only change the compilers in makenek and number of processors in SIZE, but the cases still work on Intel but fail on IBM. >>> >>>> Am 01.03.2017 um 11:18 schrieb nek5000-users at lists.mcs.anl.gov: >>>> >>>> The stenosis example is working fine with a restart. I found an older case from a few months ago that is still working fine, so I copied its .usr file to one of the new cases and it still failed, so I am suspecting that the error might be related to the grid. The parameters in the rea file are also largely the same. >>>> >>>> _______________________________________________ >>>> Nek5000-users mailing list >>>> Nek5000-users at lists.mcs.anl.gov >>>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>> >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Fri Mar 10 08:08:54 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 10 Mar 2017 15:08:54 +0100 Subject: [Nek5000-users] Nek: abnormal termination by signal 11 Message-ID: Do you restart from a single field file? Was the restart file generated on a big-endian system like BGQ? Are you using MPIIO? We read the data in chunks so there is no need to experiment with lelt. However, it might be still a good idea. You never know ;) What's the memory footprint before the crash? Just use getmaxrss() to print out the max persistent memory. Can you try again with today's master? Cheers, Stefan -----Original message----- > From:nek5000-users at lists.mcs.anl.gov > Sent: Friday 10th March 2017 14:13 > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 > > > Hi Jan, > > By how much are you reducing your resolution? > May I suggest compiling with a larger lelt and then trying ? > > I think that what is happening when you reduce lx1 is that there is not enough room > to hold the restart field... increasing lelt will alleviate this problem. > > 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, March 10, 2017 6:45 AM > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 > > Hello, > some more testing showed that the error is actually not dependent on the deformation of the grid in usrdat2. It occurs if I use a restart file and at the same time use a lower order lx1 etc. in SIZE. I sometimes do that when I suspect the resolution is too high. Increasing lx1 on the other hand is OK. Again, this error does not occur on an Intel system. The pipe/stenosis example is fine when reducing lx too, but it is also much smaller than my cases (around 10^4 Elements). I will try too find a small case that still reproduces the error. > Jan > > > Am 07.03.2017 um 14:21 schrieb nek5000-users at lists.mcs.anl.gov: > > > > I don't think his problem is related to compiler settings. The default should just work. > > Also it looks like it's a case specific problem as the NekExamples run fine. > > > > -----Original message----- > >> From:nek5000-users at lists.mcs.anl.gov > >> Sent: Tuesday 7th March 2017 14:18 > >> To: nek5000-users at lists.mcs.anl.gov > >> Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 > >> > >> > >> Hi Jan, > >> > >> I don't know if this helps, but this is the makenek script I use on BGQ. > >> > >> Paul > >> > >> ________________________________________ > >> From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > >> Sent: Tuesday, March 07, 2017 1:31 AM > >> To: nek5000-users at lists.mcs.anl.gov > >> Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 > >> > >> Hello Paul, > >> I?m working on the Juqueen IBM BlueGene/Q in Juelich. (http://www.fz-juelich.de/ias/jsc/EN/Expertise/Supercomputers/JUQUEEN/Configuration/Configuration_node.html) > >> Jan > >>> Am 07.03.2017 um 04:15 schrieb nek5000-users at lists.mcs.anl.gov: > >>> > >>> > >>> Hi Jan, > >>> > >>> Sorry if you've already answered this question Which machine are you running on? > >>> > >>> 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 06, 2017 4:31 AM > >>> To: nek5000-users at lists.mcs.anl.gov > >>> Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 > >>> > >>> Hello again, > >>> after some more trying around I got some of my cases to work again by doing a complete reset of the simulations - I was slowly increasing a forcing parameter, and by starting at zero again it seemed to work this time. Other simulations are still failing, even with the new Nek version 17.0. I directly copy the case folders between the clusters and only change the compilers in makenek and number of processors in SIZE, but the cases still work on Intel but fail on IBM. > >>> > >>>> Am 01.03.2017 um 11:18 schrieb nek5000-users at lists.mcs.anl.gov: > >>>> > >>>> The stenosis example is working fine with a restart. I found an older case from a few months ago that is still working fine, so I copied its .usr file to one of the new cases and it still failed, so I am suspecting that the error might be related to the grid. The parameters in the rea file are also largely the same. > >>>> > >>>> _______________________________________________ > >>>> Nek5000-users mailing list > >>>> Nek5000-users at lists.mcs.anl.gov > >>>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > >>> > >>> _______________________________________________ > >>> Nek5000-users mailing list > >>> Nek5000-users at lists.mcs.anl.gov > >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > >>> _______________________________________________ > >>> Nek5000-users mailing list > >>> Nek5000-users at lists.mcs.anl.gov > >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > >> > >> _______________________________________________ > >> Nek5000-users mailing list > >> Nek5000-users at lists.mcs.anl.gov > >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > >> _______________________________________________ > >> Nek5000-users mailing list > >> Nek5000-users at lists.mcs.anl.gov > >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > >> > > _______________________________________________ > > Nek5000-users mailing list > > Nek5000-users at lists.mcs.anl.gov > > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > From nek5000-users at lists.mcs.anl.gov Fri Mar 10 08:39:27 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 10 Mar 2017 15:39:27 +0100 Subject: [Nek5000-users] Nek: abnormal termination by signal 11 In-Reply-To: References: Message-ID: Hi Stefan and Paul, I just made a short test and it seems Pauls advice actually helped. I increased lelt so that the total memory available stayed the same and the run started fine. This was with a single restart file with MPIIO on the IBM big endian system, but I think I also had some restart files created on Intel. I will look into the memory footprint and the new master next week. Any idea why this only happens on IBM? Many thanks for the advice, Jan > From nek5000-users at lists.mcs.anl.gov Fri Mar 10 10:51:11 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 10 Mar 2017 16:51:11 +0000 Subject: [Nek5000-users] Nek: abnormal termination by signal 11 In-Reply-To: References: , Message-ID: Jan, Memory layout on different architectures is different... There is some sort of memory issue in the restart process under the scenario you described --- it is entirely my fault --- but I've not been able to readily track it down. Given that this situation does not often arise and that we have a standard fix, I've focused on other issues, but I apologize for causing you to lose time on this. 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, March 10, 2017 8:39 AM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 Hi Stefan and Paul, I just made a short test and it seems Pauls advice actually helped. I increased lelt so that the total memory available stayed the same and the run started fine. This was with a single restart file with MPIIO on the IBM big endian system, but I think I also had some restart files created on Intel. I will look into the memory footprint and the new master next week. Any idea why this only happens on IBM? Many thanks for the advice, Jan > _______________________________________________ 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 Mar 13 07:13:12 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 13 Mar 2017 13:13:12 +0100 Subject: [Nek5000-users] Problem with Spatial Derivatives of field In-Reply-To: References: Message-ID: Hello everyone, Sorry for the delay, I was exploring all the possibilities that you have provided to me! I believe that the problem was solved. Here is what I have done : I have increased lx1, I have computed the components of the vorticity field using wgradm1. Then when I compute gradient of vorticity for every iteration, I diffuse it over 5 time steps (with low values of dt) and this removes the problem at the interface of the elements! Thank you for your help, Best wishes, Arnold Le 06/03/2017 ? 07:38, Arnold Wakim a ?crit : > > Good Morning, > > > Sorry for taking so long to answer. First I wanted to say that I > really appreciate all of your help! > > I am currently trying all these methods : > > - as suggested by Paul Fischer, increasing LX1 and low pass filtering. > > - and smoothing the derivatives. I will keep you posted on the results. > > > What I am trying to do is studying optimal perturbations using a > DIRECT-ADJOINT approach so as to optimize quantities. > However, when I am writing the equations, I have no choice but taking > the spatial derivatives of vorticity. > > Computing the derivatives is made for every DIRECT Numerical > Simulation of the perturbations. Then I call the ADJOINT solver of Nek5000 > > In order to converge towards optimum this may take several iterations > let's say N ( roughly N=10 however since the gradients are not well > resolved then I cannot tell whether I'm converged or not). The point > is that I am computing vorticity, then computing the gradients of the > same initial field, and this, N times. This leads to the problem I am > facing. > > Hope that helps understanding the issue. If you have more questions, > please do not hesitate to ask. > > > Best wishes, > > > Arnold > > > > > > Le 03/03/2017 ? 21:33, nek5000-users at lists.mcs.anl.gov a ?crit : >> call col2(dTdx,bm1,n) ! collocate with the mass matrix >> call dssum(dTdx,nx1,ny1,nz1) ! smooth >> call col2(dTdx,bintm1,n) ! collocate with the inverse >> mass matrix > > -- > > *Arnold Wakim* > Doctorant, > D?partement d?A?rodynamique Fondamentale et Exp?rimentale > T?l: +33 1 46 23 51 83 > > > ONERA - The French Aerospace Lab -Centre de Meudon > 8, rue des Vertugadins - 92190 MEUDON > > Nous suivre sur : www.onera.fr | Twitter > | LinkedIn > | Facebook > > -- *Arnold Wakim* Doctorant, D?partement d?A?rodynamique Fondamentale et Exp?rimentale T?l: +33 1 46 23 51 83 ONERA - The French Aerospace Lab -Centre de Meudon 8, rue des Vertugadins - 92190 MEUDON Nous suivre sur : www.onera.fr | Twitter | LinkedIn | Facebook -------------- next part -------------- An HTML attachment was scrubbed... URL: -------------- next part -------------- A non-text attachment was scrubbed... Name: Image1 Type: image/jpeg Size: 2151 bytes Desc: not available URL: -------------- next part -------------- A non-text attachment was scrubbed... Name: Image1 Type: image/jpeg Size: 2151 bytes Desc: not available URL: From nek5000-users at lists.mcs.anl.gov Wed Mar 15 07:55:23 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 15 Mar 2017 13:55:23 +0100 Subject: [Nek5000-users] Nek: abnormal termination by signal 11 In-Reply-To: References: Message-ID: When you do a restart and it hangs, what's your old and new lx1? Is this a single or double precision field file? -----Original message----- > From:nek5000-users at lists.mcs.anl.gov > Sent: Friday 10th March 2017 17:52 > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 > > Jan, > > Memory layout on different architectures is different... > > There is some sort of memory issue in the restart process under the scenario > you described --- it is entirely my fault --- but I've not been able to readily track it down. > Given that this situation does not often arise and that we have a standard fix, I've > focused on other issues, but I apologize for causing you to lose time on this. > > 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, March 10, 2017 8:39 AM > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 > > Hi Stefan and Paul, > I just made a short test and it seems Pauls advice actually helped. I increased lelt so that the total memory available? stayed the same and the run started fine. > This was with a single restart file with MPIIO on the IBM big endian system, but I think? I also had some restart files created on Intel. > I will look into the memory footprint and the new master next week. > Any idea why this only happens on IBM? > Many thanks for the advice, > Jan > > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Wed Mar 15 22:28:41 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 15 Mar 2017 22:28:41 -0500 Subject: [Nek5000-users] Jacobian check Message-ID: . Can i please ask you a quick question : What source code in NEKforcould check jacobians.I believe it is jac1() routine,but I m not sure ..Where I can read more about it ? Sincerely Edward -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Mar 16 04:06:03 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 16 Mar 2017 10:06:03 +0100 Subject: [Nek5000-users] Nek: abnormal termination by signal 11 In-Reply-To: References: Message-ID: Hello, I typically work with a single precision restart file. lx1 is typically reduced from 12 to 10 or from 10 to 8. However, it seems that the error was eliminated in the newest release? I just tried to reproduce the error and it did not occur with the newest master from github, only with an older version. Jan > Am 15.03.2017 um 13:55 schrieb nek5000-users at lists.mcs.anl.gov: > > When you do a restart and it hangs, what's your old and new lx1? Is this a single or double precision field file? > > > -----Original message----- >> From:nek5000-users at lists.mcs.anl.gov >> Sent: Friday 10th March 2017 17:52 >> To: nek5000-users at lists.mcs.anl.gov >> Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 >> >> Jan, >> >> Memory layout on different architectures is different... >> >> There is some sort of memory issue in the restart process under the scenario >> you described --- it is entirely my fault --- but I've not been able to readily track it down. >> Given that this situation does not often arise and that we have a standard fix, I've >> focused on other issues, but I apologize for causing you to lose time on this. >> >> 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, March 10, 2017 8:39 AM >> To: nek5000-users at lists.mcs.anl.gov >> Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 >> >> Hi Stefan and Paul, >> I just made a short test and it seems Pauls advice actually helped. I increased lelt so that the total memory available stayed the same and the run started fine. >> This was with a single restart file with MPIIO on the IBM big endian system, but I think I also had some restart files created on Intel. >> I will look into the memory footprint and the new master next week. >> Any idea why this only happens on IBM? >> Many thanks for the advice, >> Jan >>> >> _______________________________________________ >> 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 Thu Mar 16 04:13:23 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 16 Mar 2017 10:13:23 +0100 Subject: [Nek5000-users] Nek: abnormal termination by signal 11 In-Reply-To: References: Message-ID: Hi, Hanging during restart (at least one of the possible reasons) was fixed in the commit merged yesterday. regards adam On 15/03/17 13:55, nek5000-users at lists.mcs.anl.gov wrote: > When you do a restart and it hangs, what's your old and new lx1? Is this a single or double precision field file? > > > -----Original message----- >> From:nek5000-users at lists.mcs.anl.gov >> Sent: Friday 10th March 2017 17:52 >> To: nek5000-users at lists.mcs.anl.gov >> Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 >> >> Jan, >> >> Memory layout on different architectures is different... >> >> There is some sort of memory issue in the restart process under the scenario >> you described --- it is entirely my fault --- but I've not been able to readily track it down. >> Given that this situation does not often arise and that we have a standard fix, I've >> focused on other issues, but I apologize for causing you to lose time on this. >> >> 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, March 10, 2017 8:39 AM >> To: nek5000-users at lists.mcs.anl.gov >> Subject: Re: [Nek5000-users] Nek: abnormal termination by signal 11 >> >> Hi Stefan and Paul, >> I just made a short test and it seems Pauls advice actually helped. I increased lelt so that the total memory available stayed the same and the run started fine. >> This was with a single restart file with MPIIO on the IBM big endian system, but I think I also had some restart files created on Intel. >> I will look into the memory footprint and the new master next week. >> Any idea why this only happens on IBM? >> Many thanks for the advice, >> Jan >> _______________________________________________ >> 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 Thu Mar 16 15:39:02 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 16 Mar 2017 21:39:02 +0100 Subject: [Nek5000-users] usrdat2 userchk Message-ID: Hello Neks, Does the code go into usrdat2 and modify the geometry first or does it go into userchk first? I initialize the passive scalar field at istep=0 i am running simulation with three passive scalars modifying conj_ht example. To save computational cost I run the fluid simulation and setting the IC of passive scalars to be zero and switching off the advection, so it remains zero and simulation runs quickly. T IFHEAT T IFTRAN T F F F F F F F F F F IFNAV & IFADVC (convection in P.S. fields) F F T T T F F F F F F F IFTMSH (IF mesh for this field is T mesh) After the simulation reach steadystate, I use the final fld file to start the passive scalar computations I have the following in userchk, where the initial conditions are imposed when istep=0 if(istep.eq.0) then x = xm1(i,1,1,1) y = ym1(i,1,1,1) R1 = sqrt(x*x+y*y) if((R1.le.Ro).and.(R1.ge.Ri)) then t(i,1,1,1,3) = fr*y/R1* (sin(2.0*pi*z/4.0)+sin(2.0*2.0*pi*z/4.0)) I scale the domain in usrdat2 as following: call rescale_x(xm1,-8.0,8.0) call rescale_x(ym1,-8.0,8.0) Thank you in advance Sincerely, Sandeep -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Mar 16 17:41:28 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 16 Mar 2017 22:41:28 +0000 Subject: [Nek5000-users] Jacobian check Message-ID: Hi Edward, The Jacobians are calculated in subroutine glmapm1 in coef.f and stored in array JACM1. Jacobian for each GLL point is essential calculated as the determinant of the Jacabi matrix which accounts for coordinates transformation. Ketan From nek5000-users at lists.mcs.anl.gov Thu Mar 16 17:46:34 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 16 Mar 2017 22:46:34 +0000 Subject: [Nek5000-users] usrdat2 userchk Message-ID: Hi Sandeep, usrdat2 is called before userchk at the beginning of every calculation. usrdat2 is where all the mesh information (GLL point distribution, mesh metrics etc?) is generated. Ketan From nek5000-users at lists.mcs.anl.gov Thu Mar 16 21:48:27 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 17 Mar 2017 10:48:27 +0800 (GMT+08:00) Subject: [Nek5000-users] How to use more than one box to generate one .rea file In-Reply-To: References: Message-ID: Hi all, I learnt a lot from the turbulent channel flow case study. When I want to combine .box file and base.rea file to get a .rea file, I find the maximum length of the user-specified coordinate line can be read from the .box file is about 133. How can I read more than this length coordinate? I wonder whether the Nek5000 can use more than one box to generate element information in .rea file? Or how to overcome the limit length? Best wishes! Hu -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Mar 16 23:37:39 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 17 Mar 2017 04:37:39 +0000 Subject: [Nek5000-users] How to use more than one box to generate one .rea file Message-ID: Hi Hu, Yes you can use multiple boxes to create a single mesh.. attached is an example of the box file that uses two boxes to mesh a 2D channel.. although, if you are breaking the box, you will not be able to use the periodic boundary conditions across two boxes i.e. if you break the box in the x-direction, both the boxes can have periodic faces in y-direction, but not in the x-direction because both the periodic faces are not attached to a single box. In that case, you will have to use prenek?s autoperiodic feature to generate periodic boundary conditions. Ketan -------------- next part -------------- A non-text attachment was scrubbed... Name: multi.box Type: application/octet-stream Size: 484 bytes Desc: multi.box URL: From nek5000-users at lists.mcs.anl.gov Thu Mar 16 23:53:52 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 17 Mar 2017 04:53:52 +0000 Subject: [Nek5000-users] How to use more than one box to generate one .rea file In-Reply-To: References: , Message-ID: Dear Hu, You can have more characters. Just keep wrapping lines... If you have 20 elements in the x direction, you can specify 10 coordinates on the first line and 11 on the next, or you can specify one coordinate per line for 21 lines. It will just keep reading until it finds 21 numbers. Then it will start reading the y values. 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, March 16, 2017 9:48 PM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] How to use more than one box to generate one .rea file Hi all, I learnt a lot from the turbulent channel flow case study. When I want to combine .box file and base.rea file to get a .rea file, I find the maximum length of the user-specified coordinate line can be read from the .box file is about 133. How can I read more than this length coordinate? I wonder whether the Nek5000 can use more than one box to generate element information in .rea file? Or how to overcome the limit length? Best wishes! Hu -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Fri Mar 17 08:35:45 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 17 Mar 2017 21:35:45 +0800 (GMT+08:00) Subject: [Nek5000-users] How to use more than one box to generate one .rea file In-Reply-To: References: , Message-ID: Thanks for your help, Paul. Hu -----Original Messages----- From: nek5000-users at lists.mcs.anl.gov Sent Time: Friday, March 17, 2017 To: "nek5000-users at lists.mcs.anl.gov" Cc: Subject: Re: [Nek5000-users] How to use more than one box to generate one .rea file Dear Hu, You can have more characters. Just keep wrapping lines... If you have 20 elements in the x direction, you can specify 10 coordinates on the first line and 11 on the next, or you can specify one coordinate per line for 21 lines. It will just keep reading until it finds 21 numbers. Then it will start reading the y values. 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, March 16, 2017 9:48 PM To:nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] How to use more than one box to generate one .rea file Hi all, I learnt a lot from the turbulent channel flow case study. When I want to combine .box file and base.rea file to get a .rea file, I find the maximum length of the user-specified coordinate line can be read from the .box file is about 133. How can I read more than this length coordinate? I wonder whether the Nek5000 can use more than one box to generate element information in .rea file? Or how to overcome the limit length? Best wishes! Hu -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Fri Mar 17 08:34:12 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 17 Mar 2017 21:34:12 +0800 (GMT+08:00) Subject: [Nek5000-users] How to use more than one box to generate one .rea file In-Reply-To: References: Message-ID: Thanks, Ketan. Your example box file is very helpful! Hu > -----Original Messages----- > From: nek5000-users at lists.mcs.anl.gov > Sent Time: Friday, March 17, 2017 > To: "nek5000-users at lists.mcs.anl.gov" > Cc: > Subject: Re: [Nek5000-users] How to use more than one box to generate one .rea file > > Hi Hu, > > Yes you can use multiple boxes to create a single mesh.. attached is an example of the box file that uses two boxes to mesh a 2D channel.. although, if you are breaking the box, you will not be able to use the periodic boundary conditions across two boxes i.e. if you break the box in the x-direction, both the boxes can have periodic faces in y-direction, but not in the x-direction because both the periodic faces are not attached to a single box. > In that case, you will have to use prenek?s autoperiodic feature to generate periodic boundary conditions. > > Ketan > From nek5000-users at lists.mcs.anl.gov Tue Mar 21 11:15:29 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 21 Mar 2017 16:15:29 +0000 Subject: [Nek5000-users] tubChannel - neknek script Message-ID: Hello, I am running the neknek script with the turbChannel example. My setup consists of two channels: the first one has periodic boundary conditions, and the second one has inlet/outlet boundary conditions. The numerical solution of first channel is used as an inlet condition for the second channel. The numerical solution seems to behave as expected. My next step is to simulate a short channel with periodic boundary conditions, and a longer one with inlet/outlet boundary conditions. The number of elements in the streamwise direction (x-axis) now differs. This is causing some problems since the number of elements in the x,y and z directions are set in the SIZE file that is unique to the sessions named inside and outside. Note that I need the number of elements in each direction to compute the y+ and u+ values. In the turbChannel example, the number of elements in the x, y and z directions are defined in the usr file (nelx, nely and nelz). This approach could work in my case, I think, assuming that I include a if statement on the session name (inside vs outside). However, I am after something more generic that can be applied to more complex geometries where the number of elements in each direction is not known or difficult to know. Is there a way with Nek5000 to get the number of elements in each direction in a automated way? I have another question that is a little bit off topic: when initializing an array in the subroutines defined in the usr file, should I use nelv or lelv as the number of elements per processors? In the turbChannel example, both are used and it confuses me. nelv is the maximum number of elements per processor, whereas lelv is the actual number of elements in a processor, which leads me to think lelv should be used. Is this correct? Thanks, Marco -------------- next part -------------- A non-text attachment was scrubbed... Name: smime.p7s Type: application/pkcs7-signature Size: 4215 bytes Desc: not available URL: From nek5000-users at lists.mcs.anl.gov Tue Mar 21 12:29:22 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 21 Mar 2017 10:29:22 -0700 Subject: [Nek5000-users] tubChannel - neknek script In-Reply-To: References: Message-ID: Hi Marco, The number of elements is set in .rea file. Only the maximum number of elements allowed is set in SIZE file. So, as long as your number of elements set in SIZE larger than a number of elements in each of your sub-domains, you are good to go. This is a generic set-up for neknek problems. TurbChannel example is slightly different in a sense that it hardwires the number of elements in .usr file to be used with post-processing. If you need to follow this approach, yes, putting if statements in the .usr file would perhaps help. Hope it helps. Yulia On Mar 21, 2017, at 9:15 AM, nek5000-users at lists.mcs.anl.gov wrote: > Hello, > > I am running the neknek script with the turbChannel example. My setup consists of two channels: the first one has periodic boundary conditions, and the second one has inlet/outlet boundary conditions. The numerical solution of first channel is used as an inlet condition for the second channel. The numerical solution seems to behave as expected. > > My next step is to simulate a short channel with periodic boundary conditions, and a longer one with inlet/outlet boundary conditions. The number of elements in the streamwise direction (x-axis) now differs. This is causing some problems since the number of elements in the x,y and z directions are set in the SIZE file that is unique to the sessions named inside and outside. Note that I need the number of elements in each direction to compute the y+ and u+ values. > > In the turbChannel example, the number of elements in the x, y and z directions are defined in the usr file (nelx, nely and nelz). This approach could work in my case, I think, assuming that I include a if statement on the session name (inside vs outside). However, I am after something more generic that can be applied to more complex geometries where the number of elements in each direction is not known or difficult to know. > > Is there a way with Nek5000 to get the number of elements in each direction in a automated way? > > I have another question that is a little bit off topic: when initializing an array in the subroutines defined in the usr file, should I use nelv or lelv as the number of elements per processors? In the turbChannel example, both are used and it confuses me. nelv is the maximum number of elements per processor, whereas lelv is the actual number of elements in a processor, which leads me to think lelv should be used. Is this correct? > > Thanks, > > Marco > > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Mar 21 13:03:34 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 21 Mar 2017 18:03:34 +0000 Subject: [Nek5000-users] tubChannel - neknek script In-Reply-To: References: Message-ID: Hi Marco, Just to follow up on Yulia's reply: You cannot declare space with nelv, as it is a run-time parameter not known at link time. You must use lelv. lelv = upper bound on number of elements per processor. nelv = number of elements on this processor (when the code is executing) nelv = number of elements in the mesh (for purposes of .rea file). If number of processors (mpi ranks) = 1, then nelv in the two preceding definitions are the same. nelgv = total number of elements in the (non-neknek) simulation -- i.e., nelgv is equal to the nelv value in the .rea file. lelx, lely, lelz are parameters, defined at compile time, that are _sometimes_ (but more and more rarely) used to aid in data post-processing when your domain is coming as a monolithic tensor-product-box from genbox. lelx,lely,lelz are never needed for simulations. Indeed, because these are compile-time parameters, you will have difficulty in the neknek case if your two coupled simulations do not have the same shape. A different post-processing strategy is in order. There is no good automated way that I know of to detect the domain size, particularly in parallel. It could be done, particularly on a case-by-case basis, but it would need some built in assumptions to work (e.g., that the domain is a monolithic tensor product mesh built by genbox). hth, Paul ________________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Tuesday, March 21, 2017 11:15 AM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] tubChannel - neknek script Hello, I am running the neknek script with the turbChannel example. My setup consists of two channels: the first one has periodic boundary conditions, and the second one has inlet/outlet boundary conditions. The numerical solution of first channel is used as an inlet condition for the second channel. The numerical solution seems to behave as expected. My next step is to simulate a short channel with periodic boundary conditions, and a longer one with inlet/outlet boundary conditions. The number of elements in the streamwise direction (x-axis) now differs. This is causing some problems since the number of elements in the x,y and z directions are set in the SIZE file that is unique to the sessions named inside and outside. Note that I need the number of elements in each direction to compute the y+ and u+ values. In the turbChannel example, the number of elements in the x, y and z directions are defined in the usr file (nelx, nely and nelz). This approach could work in my case, I think, assuming that I include a if statement on the session name (inside vs outside). However, I am after something more generic that can be applied to more complex geometries where the number of elements in each direction is not known or difficult to know. Is there a way with Nek5000 to get the number of elements in each direction in a automated way? I have another question that is a little bit off topic: when initializing an array in the subroutines defined in the usr file, should I use nelv or lelv as the number of elements per processors? In the turbChannel example, both are used and it confuses me. nelv is the maximum number of elements per processor, whereas lelv is the actual number of elements in a processor, which leads me to think lelv should be used. Is this correct? Thanks, Marco From nek5000-users at lists.mcs.anl.gov Tue Mar 21 14:24:08 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 21 Mar 2017 19:24:08 +0000 Subject: [Nek5000-users] tubChannel - neknek script In-Reply-To: References: Message-ID: Paul, Yulia, thank you for your help. Marco > On Mar 21, 2017, at 2:03 PM, nek5000-users at lists.mcs.anl.gov wrote: > > Hi Marco, > > Just to follow up on Yulia's reply: > > You cannot declare space with nelv, as it is a run-time parameter not known at link time. > You must use lelv. > > lelv = upper bound on number of elements per processor. > > nelv = number of elements on this processor (when the code is executing) > > nelv = number of elements in the mesh (for purposes of .rea file). > > If number of processors (mpi ranks) = 1, then nelv in the two preceding definitions are the same. > > nelgv = total number of elements in the (non-neknek) simulation -- i.e., nelgv is equal to the > nelv value in the .rea file. > > lelx, lely, lelz are parameters, defined at compile time, that are _sometimes_ (but more and > more rarely) used to aid in data post-processing when your domain is coming as a > monolithic tensor-product-box from genbox. > > lelx,lely,lelz are never needed for simulations. > > Indeed, because these are compile-time parameters, you will have difficulty in the neknek > case if your two coupled simulations do not have the same shape. A different post-processing > strategy is in order. > > There is no good automated way that I know of to detect the domain size, particularly in > parallel. It could be done, particularly on a case-by-case basis, but it would need some > built in assumptions to work (e.g., that the domain is a monolithic tensor product mesh > built by genbox). > > hth, > Paul > > ________________________________________ > From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > Sent: Tuesday, March 21, 2017 11:15 AM > To: nek5000-users at lists.mcs.anl.gov > Subject: [Nek5000-users] tubChannel - neknek script > > Hello, > > I am running the neknek script with the turbChannel example. My setup consists of two channels: the first one has periodic boundary conditions, and the second one has inlet/outlet boundary conditions. The numerical solution of first channel is used as an inlet condition for the second channel. The numerical solution seems to behave as expected. > > My next step is to simulate a short channel with periodic boundary conditions, and a longer one with inlet/outlet boundary conditions. The number of elements in the streamwise direction (x-axis) now differs. This is causing some problems since the number of elements in the x,y and z directions are set in the SIZE file that is unique to the sessions named inside and outside. Note that I need the number of elements in each direction to compute the y+ and u+ values. > > In the turbChannel example, the number of elements in the x, y and z directions are defined in the usr file (nelx, nely and nelz). This approach could work in my case, I think, assuming that I include a if statement on the session name (inside vs outside). However, I am after something more generic that can be applied to more complex geometries where the number of elements in each direction is not known or difficult to know. > > Is there a way with Nek5000 to get the number of elements in each direction in a automated way? > > I have another question that is a little bit off topic: when initializing an array in the subroutines defined in the usr file, should I use nelv or lelv as the number of elements per processors? In the turbChannel example, both are used and it confuses me. nelv is the maximum number of elements per processor, whereas lelv is the actual number of elements in a processor, which leads me to think lelv should be used. Is this correct? > > Thanks, > > Marco > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > -------------- next part -------------- A non-text attachment was scrubbed... Name: smime.p7s Type: application/pkcs7-signature Size: 4215 bytes Desc: not available URL: From nek5000-users at lists.mcs.anl.gov Tue Mar 21 14:25:55 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 21 Mar 2017 19:25:55 +0000 Subject: [Nek5000-users] turbChannel example Message-ID: Hello, I am trying to reproduce some of the turbChannel results that were published with Nek5000 in the paper that can be found in the following link: https://arxiv.org/pdf/math/0205264.pdf In this paper, two turbulent models are tested: the gradient model and the static Smagorinsky model. The paper also shows results from a coarse DNS for comparison. The implementation of the static Smagorinsky model is easily done when starting from the turbChannel example but I am not sure how to implement the gradient model since it involves a tensor product \grad u \dot \grad u. Can anyone point me to an example that has a similar implementation or explain how to implement the gradient model in Nek5000? Is it correct to assume that the current setup of the turbChannel example in Nek5000 should allow to reproduce the coarse DNS results presented in the paper? What is the relationship between Re_tau and the Reynolds number (param(2)) set in the rea file? Any help will be appreciated. Thanks, Marco -------------- next part -------------- A non-text attachment was scrubbed... Name: smime.p7s Type: application/pkcs7-signature Size: 4215 bytes Desc: not available URL: From nek5000-users at lists.mcs.anl.gov Tue Mar 21 20:07:26 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 21 Mar 2017 18:07:26 -0700 Subject: [Nek5000-users] turbChannel example In-Reply-To: References: Message-ID: Hi Marco, For the gradient model, you can use gradm1() subroutine to calculate the gradient of vx, vy, and vz individually and then the implementation is straightforward. For the turbChannel example check for the grid (genbox) and the Reynolds number used, such that it matches the paper., param(2) in negative is basically the inverse of dynamic viscosity. So, a properly defined scale, to generate the Reynolds number relationship for you. Eg, if your bulk flow streamwise velocity is 1, and the channel half width is 1, then Re_Delta = param(2), (Reynolds number based on half channel width). The relationship between Re_tau and Re_delta, can be found from Dean's correlation, that is provided in the seminal paper of Kim and Moin (1987) for DNS of Re_tau = 180. Best Regards, Tanmoy On Tue, Mar 21, 2017 at 12:25 PM, wrote: > Hello, > > I am trying to reproduce some of the turbChannel results that were > published with Nek5000 in the paper that can be found in the following link: > https://arxiv.org/pdf/math/0205264.pdf > > In this paper, two turbulent models are tested: the gradient model and the > static Smagorinsky model. The paper also shows results from a coarse DNS > for comparison. > > The implementation of the static Smagorinsky model is easily done when > starting from the turbChannel example but I am not sure how to implement > the gradient model since it involves a tensor product \grad u \dot \grad u. > Can anyone point me to an example that has a similar implementation or > explain how to implement the gradient model in Nek5000? > > Is it correct to assume that the current setup of the turbChannel example > in Nek5000 should allow to reproduce the coarse DNS results presented in > the paper? > > What is the relationship between Re_tau and the Reynolds number (param(2)) > set in the rea file? > > Any help will be appreciated. > > Thanks, > Marco > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Mar 21 11:15:30 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 21 Mar 2017 16:15:30 +0000 Subject: [Nek5000-users] turbChannel example Message-ID: Hello, I am trying to reproduce some of the turbChannel results that were published with Nek5000 in the attached paper. In this paper, two turbulent models are tested: the gradient model and the static Smagorinsky model. The paper also shows results from a coarse DNS for comparison. The implementation of the static Smagorinsky model is easily done when starting from the turbChannel example but I am not sure how to implement the gradient model since it involves a tensor product \grad u \dot \grad u. Can anyone point me to an example that has a similar implementation or explain how to implement the gradient model in Nek5000? Is it correct to assume that the current setup of the turbChannel example in Nek5000 should allow to reproduce the coarse DNS results presented in the attached paper? What is the relationship between Re_tau and the Reynolds number (param(2)) set in the rea file? Any help will be appreciated. Thanks, Marco -------------- next part -------------- A non-text attachment was scrubbed... Name: 0205264.pdf Type: application/pdf Size: 335353 bytes Desc: not available URL: -------------- next part -------------- A non-text attachment was scrubbed... Name: smime.p7s Type: application/pkcs7-signature Size: 4215 bytes Desc: not available URL: From nek5000-users at lists.mcs.anl.gov Tue Mar 21 21:08:03 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 22 Mar 2017 02:08:03 +0000 Subject: [Nek5000-users] Project a solution onto a polynomial space Message-ID: Hello, I need to compute some non-linear quantities as part of a post-processing procedure. Because they are non-linear, I will need to do some kind of dealiasing. So far, I know how to map the velocity field onto a finer grid (higher polynomial order) to compute the non-linear quantities. However, I don't know how to project the resulting field onto the original polynomial space. Note, I want to find the "projection" onto the original space, but not the "interpolation". Thanks, Juan Diego -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Mar 22 09:46:22 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 22 Mar 2017 14:46:22 +0000 Subject: [Nek5000-users] Project a solution onto a polynomial space In-Reply-To: References: Message-ID: Dear Juan, What kind of polynomial space are you projecting onto? Is it the standard Nek basis (which is piecewise polynomial), or something different? We have routines to do dealiasing, but it might be better to understand the problem a bit more. Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Tuesday, March 21, 2017 9:08 PM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] Project a solution onto a polynomial space Hello, I need to compute some non-linear quantities as part of a post-processing procedure. Because they are non-linear, I will need to do some kind of dealiasing. So far, I know how to map the velocity field onto a finer grid (higher polynomial order) to compute the non-linear quantities. However, I don't know how to project the resulting field onto the original polynomial space. Note, I want to find the "projection" onto the original space, but not the "interpolation". Thanks, Juan Diego -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Mar 22 12:21:37 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 22 Mar 2017 17:21:37 +0000 Subject: [Nek5000-users] Project a solution onto a polynomial space Message-ID: Dear Paul, Thank you for answering so quickly. Yes, the polynomial spaces I'm using are the standard Nek5000 basis functions. To understand the problem a little better: I am conducting DNS of a shear flow and I need to compute higher-order velocity moments. I've implemented some subroutines based on the "avg2" and "avg3" subroutines from Nek, but for higher order moments, i.e. , , etc. The problem is that I need to de-alias the non-linear quantities, i.e. U^3, before doing the averaging. Since the flow is planar, I also take the spanwise average using the "z_average" subroutine. I checked out the "convect.f" file to see how dealiasing is applied by mapping onto the finer grid (lxd), but I'm not quite sure how to project these results back onto the original grid. Thank you, Juan Diego -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Mar 22 16:10:15 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 22 Mar 2017 22:10:15 +0100 Subject: [Nek5000-users] Project a solution onto a polynomial space In-Reply-To: References: Message-ID: Hi, just out of interest, are you sure that you need dealiasing for statistics? Some long time ago, I tried it as well, and compared it to non-dealiased statistics, and I could not really see a difference. I guess my argument at the time was that you are interested in the low-frequency content of the statistics anyway, so that the aliasing errors would not show up. Are you then planning to increase the polynomial order such that you can completely eliminate the qudrature errors even for third order terms? Best regards, Philipp On 2017-03-22 18:21, nek5000-users at lists.mcs.anl.gov wrote: > Dear Paul, > > > Thank you for answering so quickly. Yes, the polynomial spaces I'm using > are the standard Nek5000 basis functions. > > > To understand the problem a little better: > > I am conducting DNS of a shear flow and I need to compute higher-order > velocity moments. I've implemented some subroutines based on the "avg2" > and "avg3" subroutines from Nek, but for higher order moments, i.e. > , , etc. The problem is that I need to de-alias the > non-linear quantities, i.e. U^3, before doing the averaging. Since the > flow is planar, I also take the spanwise average using the "z_average" > subroutine. > > > I checked out the "convect.f" file to see how dealiasing is applied by > mapping onto the finer grid (lxd), but I'm not quite sure how to project > these results back onto the original grid. > > > Thank you, > > > Juan Diego > > > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > From nek5000-users at lists.mcs.anl.gov Wed Mar 22 16:34:56 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 22 Mar 2017 21:34:56 +0000 Subject: [Nek5000-users] Project a solution onto a polynomial space In-Reply-To: References: Message-ID: Hi Juan, At first I would just try truncating the fully de-alised product for all the modes above lx1 since the first lx1 modes are accurately solved for. 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: Wednesday, March 22, 2017 12:21 PM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Project a solution onto a polynomial space Dear Paul, Thank you for answering so quickly. Yes, the polynomial spaces I'm using are the standard Nek5000 basis functions. To understand the problem a little better: I am conducting DNS of a shear flow and I need to compute higher-order velocity moments. I've implemented some subroutines based on the "avg2" and "avg3" subroutines from Nek, but for higher order moments, i.e. , , etc. The problem is that I need to de-alias the non-linear quantities, i.e. U^3, before doing the averaging. Since the flow is planar, I also take the spanwise average using the "z_average" subroutine. I checked out the "convect.f" file to see how dealiasing is applied by mapping onto the finer grid (lxd), but I'm not quite sure how to project these results back onto the original grid. Thank you, Juan Diego -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Mar 22 16:50:51 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 22 Mar 2017 14:50:51 -0700 Subject: [Nek5000-users] Project a solution onto a polynomial space In-Reply-To: References: Message-ID: Hi Philipp, I guess to answer your question: we are not sure if de-aliasing is needed, and my impression was that it is only needed for computation, since non-dealiased terms would contaminate the solution, but not so much for post-processing. But to be certain: we wanted to do both approaches and compare. It is very likely we will come to the same conclusions as you did long time ago. I do not believe we were planning to increase the polynomial order at this point, but we might consider it if it is necessary for accurate higher-order statistics. Best regards, Yulia On Mar 22, 2017, at 2:10 PM, nek5000-users at lists.mcs.anl.gov wrote: > Hi, > just out of interest, are you sure that you need dealiasing for statistics? Some long time ago, I tried it as well, and compared it to non-dealiased statistics, and I could not really see a difference. I guess my argument at the time was that you are interested in the low-frequency content of the statistics anyway, so that the aliasing errors would not show up. > > Are you then planning to increase the polynomial order such that you can completely eliminate the qudrature errors even for third order terms? > > Best regards, > Philipp > > On 2017-03-22 18:21, nek5000-users at lists.mcs.anl.gov wrote: >> Dear Paul, >> >> >> Thank you for answering so quickly. Yes, the polynomial spaces I'm using >> are the standard Nek5000 basis functions. >> >> >> To understand the problem a little better: >> >> I am conducting DNS of a shear flow and I need to compute higher-order >> velocity moments. I've implemented some subroutines based on the "avg2" >> and "avg3" subroutines from Nek, but for higher order moments, i.e. >> , , etc. The problem is that I need to de-alias the >> non-linear quantities, i.e. U^3, before doing the averaging. Since the >> flow is planar, I also take the spanwise average using the "z_average" >> subroutine. >> >> >> I checked out the "convect.f" file to see how dealiasing is applied by >> mapping onto the finer grid (lxd), but I'm not quite sure how to project >> these results back onto the original grid. >> >> >> Thank you, >> >> >> Juan Diego >> >> >> >> _______________________________________________ >> 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 Mar 23 07:39:42 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 23 Mar 2017 13:39:42 +0100 Subject: [Nek5000-users] Project a solution onto a polynomial space In-Reply-To: References: Message-ID: Hi Yulia and Juan Diego, thanks a lot for the answer. This is interesting, and let us know if it is really needed! With "increase the polynomial order" I essentially meant the overintegration, sorry if I was unclear. I wanted to ask whether you plan to use 3 times lx1 for third-order terms. Best, Philipp On 2017-03-22 22:50, nek5000-users at lists.mcs.anl.gov wrote: > Hi Philipp, > > I guess to answer your question: we are not sure if de-aliasing is > needed, and my impression was that it is only needed for computation, > since non-dealiased terms would contaminate the solution, but not so > much for post-processing. But to be certain: we wanted to do both > approaches and compare. It is very likely we will come to the same > conclusions as you did long time ago. > > I do not believe we were planning to increase the polynomial order at > this point, but we might consider it if it is necessary for accurate > higher-order statistics. > > Best regards, Yulia > > > On Mar 22, 2017, at 2:10 PM, nek5000-users at lists.mcs.anl.gov wrote: > >> Hi, just out of interest, are you sure that you need dealiasing for >> statistics? Some long time ago, I tried it as well, and compared it >> to non-dealiased statistics, and I could not really see a >> difference. I guess my argument at the time was that you are >> interested in the low-frequency content of the statistics anyway, >> so that the aliasing errors would not show up. >> >> Are you then planning to increase the polynomial order such that >> you can completely eliminate the qudrature errors even for third >> order terms? >> >> Best regards, Philipp >> >> On 2017-03-22 18:21, nek5000-users at lists.mcs.anl.gov wrote: >>> Dear Paul, >>> >>> >>> Thank you for answering so quickly. Yes, the polynomial spaces >>> I'm using are the standard Nek5000 basis functions. >>> >>> >>> To understand the problem a little better: >>> >>> I am conducting DNS of a shear flow and I need to compute >>> higher-order velocity moments. I've implemented some subroutines >>> based on the "avg2" and "avg3" subroutines from Nek, but for >>> higher order moments, i.e. , , etc. The problem is >>> that I need to de-alias the non-linear quantities, i.e. U^3, >>> before doing the averaging. Since the flow is planar, I also take >>> the spanwise average using the "z_average" subroutine. >>> >>> >>> I checked out the "convect.f" file to see how dealiasing is >>> applied by mapping onto the finer grid (lxd), but I'm not quite >>> sure how to project these results back onto the original grid. >>> >>> >>> Thank you, >>> >>> >>> Juan Diego >>> >>> >>> >>> _______________________________________________ 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 Thu Mar 23 08:32:29 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 23 Mar 2017 13:32:29 +0000 Subject: [Nek5000-users] Project a solution onto a polynomial space In-Reply-To: References: , Message-ID: Dear All, Thanks for the clarification. I think there are two (or three, maybe) issues here: 1) Presentation of a profile of w= (say) 2) Computation of w= Let's take a 2D case u=u(x,y), w=w(y), < f > := 1/L * \int_0^L f dx. , (x,y) \in [0,L]^2 For example 1, consider u(x,y)=y. Then, w(y) = u(x,y)^3 for all x, and w=y^3. Suppose we have only two points in x and y directions, so that u \in P_1. If w(y) is also only represented as a linear function (say, given by values at the GLL points of the mesh), then: a) The values at the 2 GLL points will be correct (i.e., w=y^3 at y=0 and y=L). b) For the case N=, there are not enough GLL points to represent w=y^3. You will need to interpolate u(x,y) onto a fine mesh prior to cubing the result, and you will need to retain w(y) on this mesh when you print it, if you want to see this. In a similar way, as noted before, if u(x,y)=x (say), then when you integrate u^3, then you'll need a higher-order quadrature, which means interpolating onto a finer mesh in the x direction. One cool thing, for quadrature, you need fewer points in the integration direction than you do in the "presentation" direction (i.e., fewer in x than in y in this example). That's because the Gauss rules allow you to accurately integrate a polynomial of degree 2M with ~M points. Regarding the possible third issue, the same rules apply in time, but might be less severe (or maybe not). The reason that they should be less of an issue in time is that we tend to not push the resolution so hard in time --- I think of it this way: Suppose I had a function that is growing in time. I want to compute it's integral (in time). I'm effectively using trapezoidal rule. I now cube that function, still using trapezoidal rule. If you look at the time history of any point in the domain, we generally have enough points that the trapezoidal rule will do a pretty good job. Otherwise, you will need to interpolate in time as well to accurately integrate u^3(y,t). Note also that of course all of the integration tends to smooth things out, which diminishes the number of modes that will not be accurately integrated (per Philipp's observation about low-frequency content). So, I think what you would want to do for your tests would be to interpolate into space to a higher polynomial, integrate in the planar directions using a higher-order Gauss rule (e.g., GL or GLL, with GL being most common), and present your wall normal profile on a finer set of GLL points. This is just a suggestion of course... Like the rest, I'm interested to know what you find! Thanks! Paul ________________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Thursday, March 23, 2017 7:39 AM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Project a solution onto a polynomial space Hi Yulia and Juan Diego, thanks a lot for the answer. This is interesting, and let us know if it is really needed! With "increase the polynomial order" I essentially meant the overintegration, sorry if I was unclear. I wanted to ask whether you plan to use 3 times lx1 for third-order terms. Best, Philipp On 2017-03-22 22:50, nek5000-users at lists.mcs.anl.gov wrote: > Hi Philipp, > > I guess to answer your question: we are not sure if de-aliasing is > needed, and my impression was that it is only needed for computation, > since non-dealiased terms would contaminate the solution, but not so > much for post-processing. But to be certain: we wanted to do both > approaches and compare. It is very likely we will come to the same > conclusions as you did long time ago. > > I do not believe we were planning to increase the polynomial order at > this point, but we might consider it if it is necessary for accurate > higher-order statistics. > > Best regards, Yulia > > > On Mar 22, 2017, at 2:10 PM, nek5000-users at lists.mcs.anl.gov wrote: > >> Hi, just out of interest, are you sure that you need dealiasing for >> statistics? Some long time ago, I tried it as well, and compared it >> to non-dealiased statistics, and I could not really see a >> difference. I guess my argument at the time was that you are >> interested in the low-frequency content of the statistics anyway, >> so that the aliasing errors would not show up. >> >> Are you then planning to increase the polynomial order such that >> you can completely eliminate the qudrature errors even for third >> order terms? >> >> Best regards, Philipp >> >> On 2017-03-22 18:21, nek5000-users at lists.mcs.anl.gov wrote: >>> Dear Paul, >>> >>> >>> Thank you for answering so quickly. Yes, the polynomial spaces >>> I'm using are the standard Nek5000 basis functions. >>> >>> >>> To understand the problem a little better: >>> >>> I am conducting DNS of a shear flow and I need to compute >>> higher-order velocity moments. I've implemented some subroutines >>> based on the "avg2" and "avg3" subroutines from Nek, but for >>> higher order moments, i.e. , , etc. The problem is >>> that I need to de-alias the non-linear quantities, i.e. U^3, >>> before doing the averaging. Since the flow is planar, I also take >>> the spanwise average using the "z_average" subroutine. >>> >>> >>> I checked out the "convect.f" file to see how dealiasing is >>> applied by mapping onto the finer grid (lxd), but I'm not quite >>> sure how to project these results back onto the original grid. >>> >>> >>> Thank you, >>> >>> >>> Juan Diego >>> >>> >>> >>> _______________________________________________ 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 Thu Mar 23 12:32:30 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 23 Mar 2017 18:32:30 +0100 Subject: [Nek5000-users] =?utf-8?q?What=27s_change_have_been_made_between_?= =?utf-8?q?version_1=2E0rc1_/_SVN__r1053_and_the_current_version?= Message-ID: Hello, I continue the work of another one, he use an old version of Nek (version 1.0rc1 / SVN r1053), and everything work fine. My problem is when I change the version to the newest one from the official website, the solution diverge after 60 time step. I can't figure out why? So if I want to work with the new version, what should be changed? Thank you for your attention, From nek5000-users at lists.mcs.anl.gov Thu Mar 23 14:09:00 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 23 Mar 2017 12:09:00 -0700 Subject: [Nek5000-users] Compile optimization flags and GDB Message-ID: Dear all, I found two problems in Nek500 while i try to make some changes to the source codes. 1. When using GDB, I cannot break on some specific lines, it prompts message like missing line number information. I?ve enabled the debuging Flag ?G=-g? in bin/makenek 2. I want to use optimization level O0 instead of the default O2 to make gdb debugging easier. So i changed line number 122 in core/makefile.template from "L2=$(G) -O2? to "L2=$(G) -O0?. While compiling with -O2 the result is correct , there is segment fault with -O0. Developing Environment: CENTOS 6.5 GCC-4.9.2 Nek example: eddy_uv Thanks Steven -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Mar 23 14:32:35 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 23 Mar 2017 20:32:35 +0100 Subject: [Nek5000-users] =?utf-8?q?Run_nek5000_in_BlueGene_supercalculator?= =?utf-8?q?_=28IBM_compiler=29?= Message-ID: Hi, I have trouble running Nek in BlueGene in IDRIS, French national supercalculator: the compilation show no error, but the output give NaN before the time loop start. I looked in the internet and I found 1 person ask almost the same question 4 years ago (In my case the compilation was fine), but I can't find the answear. Are there anyone ran Nek5000 in IDRIS can share their experience? Thank you guy, From nek5000-users at lists.mcs.anl.gov Thu Mar 23 14:57:32 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 23 Mar 2017 20:57:32 +0100 Subject: [Nek5000-users] comp_vort3, nelt, conj_ht Message-ID: Hello Neks, I modified conj_ht example and defined three scalars. NEL>NELV. The domain of scalars is bigger than the fluid. I create a vector by taking the curl of three scalars, using common /myvort/ b1(lx1,ly1,lz1,lelt,3), call comp_vort3(b1,work1,work2,t(1,1,1,1,1), $ t(1,1,1,1,2),t(1,1,1,1,3)) b1 is computed correctly in the fluid domain, but is solid domain it showing zero. Can someone tell me how to modify the comp_vort3 subroutine, to correctly compute b1 over the entire domain. I tried to modify call dudxyz(work1,w,rym1,sym1,tym1,jacm1,2,2), changing the imsh=2 (the last second parameter in the above call), but the the result remains the same. I use the three components of computed b1 in userq Thank you in advance. Sincerely, Sandeep -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Fri Mar 24 02:25:55 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 24 Mar 2017 08:25:55 +0100 Subject: [Nek5000-users] Run nek5000 in BlueGene supercalculator (IBM compiler) In-Reply-To: References: Message-ID: Hello, I recently moved my computations to the blue-gene server of IDRIS. I had to make the following modifications to make the code run on this server: 1. Change the compiler settings. A page containing the details of the various compilers are given on IDRIS website. 2. There were some issues with the sub-block submission. Sometimes the the computations hung displaying "permission denied". So I was advised to use compute blocks in multiple of 64. 3. Can you check which step of your code gives NaN? Is it because of an error in reading any file? In my simulations, apparently, "load_fld' subroutine was causing a problem so I used an alternate method to read the files. Hope these help. N. On Thursday 23 March 2017 08:32 PM, nek5000-users at lists.mcs.anl.gov wrote: > Hi, > > I have trouble running Nek in BlueGene in IDRIS, French national supercalculator: the compilation show no error, but the output give NaN before the time loop start. I looked in the internet and I found 1 person ask almost the same question 4 years ago (In my case the compilation was fine), but I can't find the answear. > > Are there anyone ran Nek5000 in IDRIS can share their experience? > > Thank you guy, > > > > _______________________________________________ > 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 Mar 24 03:00:21 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 24 Mar 2017 09:00:21 +0100 Subject: [Nek5000-users] =?utf-8?b?Pz09P3V0Zi04P3E/ICBSdW4gbmVrNTAwMCBp?= =?utf-8?q?n_BlueGene_supercalculator_=28IBM=3F=3D=3D=3Futf-8=3Fq=3F_compi?= =?utf-8?q?ler=29?= In-Reply-To: Message-ID: Hello, Thank you very much for your answear, could you please share more detail about your changes? 1: What compilers did you chose? 2: I will do that 3: I read only standard file, I don't have to read fld (yet), the fileds is initialized with an analytical form, and it fail just after the setup phrase, it show NaN in one columm of Hemholtz step. But I will have to read on fld file, what alternative methode did you use? Thank you again, Best, Le Vendredi 24 Mars 2017 08:25 CET, nek5000-users at lists.mcs.anl.gov a ?crit: > Hello, > > I recently moved my computations to the blue-gene server of > IDRIS. I had to make the following modifications to make the code > run on this server: > > 1. Change the compiler settings. A page containing the details > of the various compilers are given on IDRIS website. > > 2. There were some issues with the sub-block submission. Sometimes the > the computations hung displaying "permission denied". So I was advised > to use compute blocks in multiple of 64. > > 3. Can you check which step of your code gives NaN? Is it because of > an error in reading any file? In my simulations, apparently, "load_fld' > subroutine was causing a problem so I used an alternate method to read > the files. > > Hope these help. > > N. > > On Thursday 23 March 2017 08:32 PM, nek5000-users at lists.mcs.anl.gov wrote: > > Hi, > > > > I have trouble running Nek in BlueGene in IDRIS, French national supercalculator: the compilation show no error, but the output give NaN before the time loop start. I looked in the internet and I found 1 person ask almost the same question 4 years ago (In my case the compilation was fine), but I can't find the answear. > > > > Are there anyone ran Nek5000 in IDRIS can share their experience? > > > > Thank you guy, > > > > > > > > _______________________________________________ > > 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 Fri Mar 24 03:15:40 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 24 Mar 2017 09:15:40 +0100 Subject: [Nek5000-users] ?= Run nek5000 in BlueGene supercalculator (IBM=?utf-8?q? compiler) In-Reply-To: References: Message-ID: Hello again, 1. I use "mpixlf77" and "mpixlc_r" for fortran and C compilers, respectively. 2. Is it possible for you to run the case that you are attempting on IDRIS, on a different server? Perhaps, by comparing the output files for the two you might get an idea of resolving the problem. Can you check if you are able to run examples from NeK repository on IDRIS? 3. I would suggest that you try load_fld subroutine first. It might work for you as we used "load_fld" to read base flow as well perturbation variables. To circumvent this problem on IDRIS, we use "mfi" subroutine of nek with slight modifications. Cheers. N. On Friday 24 March 2017 09:00 AM, nek5000-users at lists.mcs.anl.gov wrote: > Hello, > > Thank you very much for your answear, could you please share more detail about your changes? > > 1: What compilers did you chose? > 2: I will do that > 3: I read only standard file, I don't have to read fld (yet), the fileds is initialized with an analytical form, and it fail just after the setup phrase, it show NaN in one columm of Hemholtz step. > But I will have to read on fld file, what alternative methode did you use? > > Thank you again, > > Best, > > Le Vendredi 24 Mars 2017 08:25 CET, nek5000-users at lists.mcs.anl.gov a ?crit: > >> Hello, >> >> I recently moved my computations to the blue-gene server of >> IDRIS. I had to make the following modifications to make the code >> run on this server: >> >> 1. Change the compiler settings. A page containing the details >> of the various compilers are given on IDRIS website. >> >> 2. There were some issues with the sub-block submission. Sometimes the >> the computations hung displaying "permission denied". So I was advised >> to use compute blocks in multiple of 64. >> >> 3. Can you check which step of your code gives NaN? Is it because of >> an error in reading any file? In my simulations, apparently, "load_fld' >> subroutine was causing a problem so I used an alternate method to read >> the files. >> >> Hope these help. >> >> N. >> >> On Thursday 23 March 2017 08:32 PM, nek5000-users at lists.mcs.anl.gov wrote: >>> Hi, >>> >>> I have trouble running Nek in BlueGene in IDRIS, French national supercalculator: the compilation show no error, but the output give NaN before the time loop start. I looked in the internet and I found 1 person ask almost the same question 4 years ago (In my case the compilation was fine), but I can't find the answear. >>> >>> Are there anyone ran Nek5000 in IDRIS can share their experience? >>> >>> Thank you guy, >>> >>> >>> >>> _______________________________________________ >>> 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 Fri Mar 24 03:16:44 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 24 Mar 2017 15:16:44 +0700 Subject: [Nek5000-users] Copy velocity slice from one boundary to another Message-ID: Hi, Neks! I have two pipes in my simulation. They are placed near each other on one axis with empty space between. One of them with periodic boundary conditions on z direction, another one - inflow -> outflow. How can I copy velocity slice from one of boundary on first pipe with periodic bc to the inflow boundary on second pipe? Regards, Vatslav. -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Fri Mar 24 03:17:59 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 24 Mar 2017 09:17:59 +0100 Subject: [Nek5000-users] ?= Run nek5000 in BlueGene supercalculator (IBM=?utf-8?q? compiler) In-Reply-To: References: Message-ID: I am not aware of a bug like this. On BG you want to use the IBM compilers. Did you try the latest version on GitHub? You can also try to run one of our examples or short tests to check your installation. Can you please trap NaNs to see where they occur the first time. Stefan On 24 Mar 2017, at 09:01, "nek5000-users at lists.mcs.anl.gov " > wrote: Hello, Thank you very much for your answear, could you please share more detail about your changes? 1: What compilers did you chose? 2: I will do that 3: I read only standard file, I don't have to read fld (yet), the fileds is initialized with an analytical form, and it fail just after the setup phrase, it show NaN in one columm of Hemholtz step. But I will have to read on fld file, what alternative methode did you use? Thank you again, Best, Le Vendredi 24 Mars 2017 08:25 CET, nek5000-users at lists.mcs.anl.gov a ?crit: > Hello, > >?? I recently moved my computations to the blue-gene server of > IDRIS. I had to make the following modifications to make the code > run on this server: > > 1. Change the compiler settings. A page containing the details > of the various compilers are given on IDRIS website. > > 2. There were some issues with the sub-block submission. Sometimes the > the computations hung displaying "permission denied". So I was advised > to use compute blocks in multiple of 64. > > 3. Can you check which step of your code gives NaN? Is it because of > an error in reading any file? In my simulations, apparently, "load_fld' > subroutine was causing a problem so I used an alternate method to read > the files. > > Hope these help. > > N. > > On Thursday 23 March 2017 08:32 PM, nek5000-users at lists.mcs.anl.gov wrote: > > Hi, > > > > I have trouble running Nek in BlueGene in IDRIS, French national supercalculator: the compilation show no error, but the output give NaN before the time loop start. I looked in the internet and I found 1 person ask almost the same question 4 years ago (In my case the compilation was fine), but I can't find the answear. > > > > Are there anyone ran Nek5000 in IDRIS can share their experience? > > > > Thank you guy, > > > > > > > > _______________________________________________ > > 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 Mar 24 03:20:34 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 24 Mar 2017 09:20:34 +0100 Subject: [Nek5000-users] ?= Run nek5000 in BlueGene supercalculator (IBM=?utf-8?q? compiler) In-Reply-To: References: Message-ID: If there is indeed a bug with load_fld please report an issue on Github an provide the necessary details. This way we can fix it. Stefan? On 24 Mar 2017, at 09:16, "nek5000-users at lists.mcs.anl.gov " > wrote: Hello again, ? 1. I use "mpixlf77" and "mpixlc_r" for fortran and C compilers, respectively. ? 2. Is it possible for you to run the case that you are attempting on IDRIS, on a different server? Perhaps, by comparing the output files for the two you might get an idea of resolving the problem. Can you check if you are able to run examples from NeK repository on IDRIS? ? 3. I would suggest that you try load_fld subroutine first. It might work for you as we used "load_fld" to read base flow as well perturbation variables. To circumvent this problem on IDRIS, we use "mfi" subroutine of nek with slight modifications. Cheers. N. On Friday 24 March 2017 09:00 AM, nek5000-users at lists.mcs.anl.gov wrote: >?? Hello, > > Thank you very much for your answear, could you please share more detail about your changes? > > 1: What compilers did you chose? > 2: I will do that > 3: I read only standard file, I don't have to read fld (yet), the fileds is initialized with an analytical form, and it fail just after the setup phrase, it show NaN in one columm of Hemholtz step. > But I will have to read on fld file, what alternative methode did you use? > > Thank you again, > > Best, > > Le Vendredi 24 Mars 2017 08:25 CET, nek5000-users at lists.mcs.anl.gov a ?crit: >?? >> Hello, >> >>??? I recently moved my computations to the blue-gene server of >> IDRIS. I had to make the following modifications to make the code >> run on this server: >> >> 1. Change the compiler settings. A page containing the details >> of the various compilers are given on IDRIS website. >> >> 2. There were some issues with the sub-block submission. Sometimes the >> the computations hung displaying "permission denied". So I was advised >> to use compute blocks in multiple of 64. >> >> 3. Can you check which step of your code gives NaN? Is it because of >> an error in reading any file? In my simulations, apparently, "load_fld' >> subroutine was causing a problem so I used an alternate method to read >> the files. >> >> Hope these help. >> >> N. >> >> On Thursday 23 March 2017 08:32 PM, nek5000-users at lists.mcs.anl.gov wrote: >>> Hi, >>> >>> I have trouble running Nek in BlueGene in IDRIS, French national supercalculator: the compilation show no error, but the output give NaN before the time loop start. I looked in the internet and I found 1 person ask almost the same question 4 years ago (In my case the compilation was fine), but I can't find the answear. >>> >>> Are there anyone ran Nek5000 in IDRIS can share their experience? >>> >>> Thank you guy, >>> >>> >>> >>> _______________________________________________ >>> 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 Mar 24 03:47:01 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 24 Mar 2017 08:47:01 +0000 Subject: [Nek5000-users] Dimensionfull passive scalar Message-ID: Hi! I am simulating a flow where thermodynamic processes takes place. Since these thermodynamic processes are rather complicated I decided that developing the set up is best done in dimensionfull variables. Here I ran into unexpected problems since it seems as if the parameters in the .rea file do not work as I thought they would. The temperature solution works well. Putting in the "rhocp" and "conduct" of my fluid into "p007" and "p008" gives the results that I expect. However, I also have two passive scalars. For them I am not sure what the meaning of "rhocp" actually is. >From eqn (1.4) of Ref. [*] I would assume that setting up a passive scalar \phi with diffusivity a = 2.14E-5 m^2/s evolving as D \phi /D t = a Laplacian(\phi) [D/Dt = total derivative] means using "rhocp = 1" and "a = 2.14E-5". However, this seems to not be the case, since under these assumptions the corresponding dimensionless set-up gives totally different results. If my understanding was correct it would only be the ratio of "rhocp" and "conduct" that matters fo a scalar, but I have found that the individual values matter. This leads me to the questions: * What is the meaning of "rhocp" and "conduct" for a scalar? * In which dimensions "rhocp" and "conduct" for a scalar? * Why does the individual values of "rhocp" and "conduct" matter, when they should no according to eqn (1.4) of Ref. [*]? Best, Johan [*]: User Documentation: http://nek5000.github.io/NekDoc/Nek_users.pdf -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Fri Mar 24 12:40:59 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 24 Mar 2017 17:40:59 +0000 Subject: [Nek5000-users] turbChannel example In-Reply-To: References: Message-ID: Hi Tanmoy, thank you for your reply. I did find the correlation in the reference you provided. I have one more question regarding the implementation of the gradient model: the gradient model consists of computing \tau defined as proportional to the tensor product \grad u \dot \grad u. Then, once \tau is computed, \grad \tau is added to the momentum equation as a source term. Should I add \grad \tau to the momentum equation using userf function in the user file? Thanks, Marco On Mar 21, 2017, at 9:07 PM, nek5000-users at lists.mcs.anl.gov wrote: Hi Marco, For the gradient model, you can use gradm1() subroutine to calculate the gradient of vx, vy, and vz individually and then the implementation is straightforward. For the turbChannel example check for the grid (genbox) and the Reynolds number used, such that it matches the paper., param(2) in negative is basically the inverse of dynamic viscosity. So, a properly defined scale, to generate the Reynolds number relationship for you. Eg, if your bulk flow streamwise velocity is 1, and the channel half width is 1, then Re_Delta = param(2), (Reynolds number based on half channel width). The relationship between Re_tau and Re_delta, can be found from Dean's correlation, that is provided in the seminal paper of Kim and Moin (1987) for DNS of Re_tau = 180. Best Regards, Tanmoy On Tue, Mar 21, 2017 at 12:25 PM, > wrote: Hello, I am trying to reproduce some of the turbChannel results that were published with Nek5000 in the paper that can be found in the following link: https://arxiv.org/pdf/math/0205264.pdf In this paper, two turbulent models are tested: the gradient model and the static Smagorinsky model. The paper also shows results from a coarse DNS for comparison. The implementation of the static Smagorinsky model is easily done when starting from the turbChannel example but I am not sure how to implement the gradient model since it involves a tensor product \grad u \dot \grad u. Can anyone point me to an example that has a similar implementation or explain how to implement the gradient model in Nek5000? Is it correct to assume that the current setup of the turbChannel example in Nek5000 should allow to reproduce the coarse DNS results presented in the paper? What is the relationship between Re_tau and the Reynolds number (param(2)) set in the rea file? Any help will be appreciated. Thanks, Marco _______________________________________________ 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 Mar 24 12:52:28 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 24 Mar 2017 17:52:28 +0000 Subject: [Nek5000-users] Copy velocity slice from one boundary to another In-Reply-To: References: Message-ID: Vatslav, you will have to use the neknek script that allows you to exchange data between two Nek5000 sessions that are run simultaneously. You should have a look at the neknek examples to understand how to set up your usr file. Some of the subroutines that will be useful to you are located in the following link: http://www.mcs.anl.gov/research/projects/nek5/docs/html/multimesh_8f_source.html You will have to modify some of them to fit your needs since for example the subroutine ?set_inflag? is written to look for ?in? boundary conditions and replace them with ?v ?. You will need a subroutine that looks for ?in? and substitute it with either ?v ? or ?P ? depending on the which pipe you are at. Marco On Mar 24, 2017, at 4:16 AM, nek5000-users at lists.mcs.anl.gov wrote: Hi, Neks! I have two pipes in my simulation. They are placed near each other on one axis with empty space between. One of them with periodic boundary conditions on z direction, another one - inflow -> outflow. How can I copy velocity slice from one of boundary on first pipe with periodic bc to the inflow boundary on second pipe? Regards, Vatslav. _______________________________________________ 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 Mar 24 13:20:09 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 24 Mar 2017 11:20:09 -0700 Subject: [Nek5000-users] turbChannel example In-Reply-To: References: Message-ID: Hi Marco, Yes, the gradient model should be added as a forcing term in userf() subroutine. Best Regards, Tanmoy On Fri, Mar 24, 2017 at 10:40 AM, wrote: > Hi Tanmoy, > > thank you for your reply. I did find the correlation in the reference you > provided. > > I have one more question regarding the implementation of the gradient > model: > the gradient model consists of computing \tau defined as proportional to > the tensor product \grad u \dot \grad u. Then, once \tau is computed, \grad > \tau is added to the momentum equation as a source term. Should I add \grad > \tau to the momentum equation using userf function in the user file? > > Thanks, > Marco > > > On Mar 21, 2017, at 9:07 PM, nek5000-users at lists.mcs.anl.gov wrote: > > Hi Marco, > > For the gradient model, you can use gradm1() subroutine to calculate the > gradient of vx, vy, and vz individually and then the implementation is > straightforward. > For the turbChannel example check for the grid (genbox) and the Reynolds > number used, such that it matches the paper., param(2) in negative is > basically the inverse of dynamic viscosity. So, a properly defined scale, > to generate the Reynolds number relationship for you. Eg, if your bulk flow > streamwise velocity is 1, and the channel half width is 1, then Re_Delta = > param(2), (Reynolds number based on half channel width). The relationship > between Re_tau and Re_delta, can be found from Dean's correlation, that is > provided in the seminal paper of Kim and Moin (1987) for DNS of Re_tau = > 180. > > Best Regards, > Tanmoy > > On Tue, Mar 21, 2017 at 12:25 PM, wrote: > >> Hello, >> >> I am trying to reproduce some of the turbChannel results that were >> published with Nek5000 in the paper that can be found in the following link: >> https://arxiv.org/pdf/math/0205264.pdf >> >> In this paper, two turbulent models are tested: the gradient model and >> the static Smagorinsky model. The paper also shows results from a coarse >> DNS for comparison. >> >> The implementation of the static Smagorinsky model is easily done when >> starting from the turbChannel example but I am not sure how to implement >> the gradient model since it involves a tensor product \grad u \dot \grad u. >> Can anyone point me to an example that has a similar implementation or >> explain how to implement the gradient model in Nek5000? >> >> Is it correct to assume that the current setup of the turbChannel example >> in Nek5000 should allow to reproduce the coarse DNS results presented in >> the paper? >> >> What is the relationship between Re_tau and the Reynolds number >> (param(2)) set in the rea file? >> >> Any help will be appreciated. >> >> Thanks, >> Marco >> _______________________________________________ >> 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 Sat Mar 25 12:07:59 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sat, 25 Mar 2017 17:07:59 +0000 Subject: [Nek5000-users] comp_vort3, nelt, conj_ht In-Reply-To: References: Message-ID: Hi Sandeep, This issue should now be resolved. comp_vort3() will now compute the curl of the supplied vector field over all elements, e=1,...,nelt. Moreover, prepost() has been modified to not put zeros in the velocity field when e > nelv. So, you should be able to do something like: call comp_vort3(curlv,w1,w2,u,v,w) call outpost(curlv(1,1),curlv(1,2),culrv(1,3),pr,t,' ') and have the right thing happen. 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, March 23, 2017 2:57 PM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] comp_vort3, nelt, conj_ht Hello Neks, I modified conj_ht example and defined three scalars. NEL>NELV. The domain of scalars is bigger than the fluid. I create a vector by taking the curl of three scalars, using common /myvort/ b1(lx1,ly1,lz1,lelt,3), call comp_vort3(b1,work1,work2,t(1,1,1,1,1), $ t(1,1,1,1,2),t(1,1,1,1,3)) b1 is computed correctly in the fluid domain, but is solid domain it showing zero. Can someone tell me how to modify the comp_vort3 subroutine, to correctly compute b1 over the entire domain. I tried to modify call dudxyz(work1,w,rym1,sym1,tym1,jacm1,2,2), changing the imsh=2 (the last second parameter in the above call), but the the result remains the same. I use the three components of computed b1 in userq Thank you in advance. Sincerely, Sandeep -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Sun Mar 26 23:37:46 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 27 Mar 2017 04:37:46 +0000 Subject: [Nek5000-users] Interpolation between two meshes Message-ID: Dear Neks, I have been using 'g2gi' to do interpolation between different meshes. Recently, I have noticed that when I interpolate between two big meshes (say 300000 elements in each mesh), the interpolation hangs at 'call findpts' and never moves on. I tried increasing number of processors and changing 'lpart', but none of these worked. I'm wondering what could cause the interpolation to hang at 'findpts'. Has anyone encountered similar issue? Hope anyone could give me some advice. Thank you very much in advance. Best regards, Tony -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Mar 27 02:47:37 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 27 Mar 2017 09:47:37 +0200 Subject: [Nek5000-users] Interpolation between two meshes In-Reply-To: References: Message-ID: Please update to the latest master. Note, g2gi was replaced by gfldr. Stefan -----Original message----- > From:nek5000-users at lists.mcs.anl.gov > Sent: Monday 27th March 2017 6:38 > To: Nek5000 > Subject: [Nek5000-users] Interpolation between two meshes > > Dear Neks, > > I have been using 'g2gi' to do interpolation between different meshes. Recently, I have?noticed that when I interpolate between two big meshes (say 300000 elements in each mesh), the interpolation hangs at 'call findpts' and never moves on. I tried increasing > number of processors and changing 'lpart', but none of these worked. > > I'm wondering what could cause the interpolation to hang at 'findpts'. Has anyone encountered similar issue? > > Hope anyone could give me some advice. Thank you very much in advance. > > Best regards, > Tony > _______________________________________________ > 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 Mar 27 04:47:00 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 27 Mar 2017 16:47:00 +0700 Subject: [Nek5000-users] Copy velocity slice from one boundary to another Message-ID: Thanks a lot for replying, your answer was very useful. I look on multimesh.f file. As i understood, i need set subroutine 'set_inflag' to look for 'P ' bc. After this i need to call 'get_values(field)' subroutine, which interpolate and put the value in valint(ix,iy,iz,ie,ifld) array. And then this array will be available in userbc in .usr file, to set it on inflow boundary. c----------------------------------------------------------------------------------------------- Vatslav, you will have to use the neknek script that allows you to exchange data between two Nek5000 sessions that are run simultaneously. You should have a look at the neknek examples to understand how to set up your usr file. Some of the subroutines that will be useful to you are located in the following link: http://www.mcs.anl.gov/research/projects/nek5/docs/ html/multimesh_8f_source.html You will have to modify some of them to fit your needs since for example the subroutine ?set_inflag? is written to look for ?in? boundary conditions and replace them with ?v ?. You will need a subroutine that looks for ?in? and substitute it with either ?v ? or ?P ? depending on the which pipe you are at. Marco Hi, Neks! I have two pipes in my simulation. They are placed near each other on one axis with empty space between. One of them with periodic boundary conditions on z direction, another one - inflow -> outflow. How can I copy velocity slice from one of boundary on first pipe with periodic bc to the inflow boundary on second pipe? Regards, Vatslav c----------------------------------------------------------------------------------------------- Regards, Vatslav -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Mar 27 04:31:53 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 27 Mar 2017 11:31:53 +0200 Subject: [Nek5000-users] Robin Boundary Condition -- Navier's Slip Length Message-ID: Hi Neks, I wish to simulate a transitional channel flow whose wall respect a "slip-length" boundary condition, such as: $ [u + \delta \frac{\partial u}{\partial n}]_{wall}=0$ Where \delta is the slip length ^n | u u | |-->/ |----->/ | | / | / | | / | / | | / | / |___|/_______| /_____ | / ^ |/ v \delta No-slip Slip-length (a better sketch can be found here: http://www.nature.com/nmat/journal/v2/n4/fig_tab/nmat857_F1.html ) I would like to know if this Robin boundary condition for velocity field is already implemented in the current code. Thank you Ciccio -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Mar 27 06:56:02 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 27 Mar 2017 13:56:02 +0200 Subject: [Nek5000-users] Interpolation between two meshes In-Reply-To: References: Message-ID: Hi Tony, I have encountered the same issue with g2gi when interpolating very large meshes. I don't know what is causing the issue but a workaround is to reduce the polynomial order. You obviously loose accuracy by doing this, but I still find it better than starting from scratch with the new mesh. Hope this helps. Best, Mattias On 03/27/2017 06:37 AM, nek5000-users at lists.mcs.anl.gov wrote: > Dear Neks, > > I have been using 'g2gi' to do interpolation between different meshes. > Recently, I have noticed that when I interpolate between two big > meshes (say 300000 elements in each mesh), the interpolation hangs at > 'call findpts' and never moves on. I tried increasing number of > processors and changing 'lpart', but none of these worked. > > I'm wondering what could cause the interpolation to hang at 'findpts'. > Has anyone encountered similar issue? > > Hope anyone could give me some advice. Thank you very much in advance. > > Best regards, > Tony > > > _______________________________________________ > 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 Mar 27 11:16:27 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 27 Mar 2017 18:16:27 +0200 Subject: [Nek5000-users] comp_vort3, nelt, conj_ht Message-ID: Thank you Paul. Now comp_vort3 doesnt give zeros in the solid domain. What is the difference between comp_vort3 and the calculation of curl using call gradm1(dAxdx,dAxdy,dAxdz,t(1,1,1,1,1)) call gradm1(dAydx,dAydy,dAydz,t(1,1,1,1,2)) call gradm1(dAzdx,dAzdy,dAzdz,t(1,1,1,1,3)) call sub3(bfx1,dAzdy,dAydz,m) call sub3(bfy1,dAxdz,dAzdx,m) call sub3(bfz1,dAydx,dAxdy,m) ?When I compare the glsc3 of a curls computed by comp_vort3 and gradm1, there is a difference of 0.5% to 1%. Which procedure suits well, if I want to use u x curl in the userq Sincerely, Sandeep > > > Hi Sandeep, > > This issue should now be resolved. > > comp_vort3() will now compute the curl of the supplied vector field over > all elements, e=1,...,nelt. > > Moreover, prepost() has been modified to not put zeros in the velocity > field when e > nelv. > > So, you should be able to do something like: > > call comp_vort3(curlv,w1,w2,u,v,w) > > call outpost(curlv(1,1),curlv(1,2),culrv(1,3),pr,t,' ') > > and have the right thing happen. > > 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, March 23, 2017 2:57 PM > To: nek5000-users at lists.mcs.anl.gov > Subject: [Nek5000-users] comp_vort3, nelt, conj_ht > > Hello Neks, > I modified conj_ht example and defined three scalars. NEL>NELV. The domain > of scalars is bigger than the fluid. > I create a vector by taking the curl of three scalars, using > common /myvort/ b1(lx1,ly1,lz1,lelt,3), > call comp_vort3(b1,work1,work2,t(1,1,1,1,1), > $ t(1,1,1,1,2),t(1,1,1,1,3)) > > b1 is computed correctly in the fluid domain, but is solid domain it > showing zero. > Can someone tell me how to modify the comp_vort3 subroutine, to correctly > compute b1 over the entire domain. > I tried to modify call dudxyz(work1,w,rym1,sym1,tym1,jacm1,2,2), changing > the imsh=2 (the last second parameter in the above call), but the the > result remains the same. > I use the three components of computed b1 in userq > Thank you in advance. > > Sincerely, > Sandeep > > > -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Mar 27 11:18:14 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 27 Mar 2017 16:18:14 +0000 Subject: [Nek5000-users] Interpolation between two meshes In-Reply-To: References: Message-ID: Hi Stefan and Mattias, Thank you both for your kind advice. Stefan, I had a look at the new 'gfldr' subroutine. It seems that the spectral interpolation procedure is the same as before, however, the latest subroutine breaks down the number of fields to interpolate in one go. I still don't see why the old g2gi hangs at 'findpts'. Is it mainly because of memory size? (I have been using my own copy of the legacy nek, so I'm quite keen on making it work with g2gi.) Mattias, I will give it a go with your suggestion. By reducing the polynomial order, did you mean the order of the old field or the order of the new geometry field, or both? Thank you again for both your help. Best regards, Tony ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov on behalf of nek5000-users-request at lists.mcs.anl.gov Sent: 27 March 2017 12:57 To: nek5000-users at lists.mcs.anl.gov Subject: Nek5000-users Digest, Vol 97, Issue 27 Send Nek5000-users mailing list submissions to nek5000-users at lists.mcs.anl.gov To subscribe or unsubscribe via the World Wide Web, visit https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users or, via email, send a message with subject or body 'help' to nek5000-users-request at lists.mcs.anl.gov You can reach the person managing the list at nek5000-users-owner at lists.mcs.anl.gov When replying, please edit your Subject line so it is more specific than "Re: Contents of Nek5000-users digest..." Today's Topics: 1. Interpolation between two meshes (nek5000-users at lists.mcs.anl.gov) 2. Re: Interpolation between two meshes (nek5000-users at lists.mcs.anl.gov) 3. Re: Copy velocity slice from one boundary to another (nek5000-users at lists.mcs.anl.gov) 4. Robin Boundary Condition -- Navier's Slip Length (nek5000-users at lists.mcs.anl.gov) 5. Re: Interpolation between two meshes (nek5000-users at lists.mcs.anl.gov) ---------------------------------------------------------------------- Message: 1 Date: Mon, 27 Mar 2017 04:37:46 +0000 From: nek5000-users at lists.mcs.anl.gov To: Nek5000 Subject: [Nek5000-users] Interpolation between two meshes Message-ID: Content-Type: text/plain; charset="iso-8859-1" Dear Neks, I have been using 'g2gi' to do interpolation between different meshes. Recently, I have noticed that when I interpolate between two big meshes (say 300000 elements in each mesh), the interpolation hangs at 'call findpts' and never moves on. I tried increasing number of processors and changing 'lpart', but none of these worked. I'm wondering what could cause the interpolation to hang at 'findpts'. Has anyone encountered similar issue? Hope anyone could give me some advice. Thank you very much in advance. Best regards, Tony -------------- next part -------------- An HTML attachment was scrubbed... URL: ------------------------------ Message: 2 Date: Mon, 27 Mar 2017 09:47:37 +0200 From: nek5000-users at lists.mcs.anl.gov To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Interpolation between two meshes Message-ID: Content-Type: text/plain; charset=utf-8 Please update to the latest master. Note, g2gi was replaced by gfldr. Stefan -----Original message----- > From:nek5000-users at lists.mcs.anl.gov > Sent: Monday 27th March 2017 6:38 > To: Nek5000 > Subject: [Nek5000-users] Interpolation between two meshes > > Dear Neks, > > I have been using 'g2gi' to do interpolation between different meshes. Recently, I have?noticed that when I interpolate between two big meshes (say 300000 elements in each mesh), the interpolation hangs at 'call findpts' and never moves on. I tried increasing > number of processors and changing 'lpart', but none of these worked. > > I'm wondering what could cause the interpolation to hang at 'findpts'. Has anyone encountered similar issue? > > Hope anyone could give me some advice. Thank you very much in advance. > > Best regards, > Tony > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users ------------------------------ Message: 3 Date: Mon, 27 Mar 2017 16:47:00 +0700 From: nek5000-users at lists.mcs.anl.gov To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Copy velocity slice from one boundary to another Message-ID: Content-Type: text/plain; charset="utf-8" Thanks a lot for replying, your answer was very useful. I look on multimesh.f file. As i understood, i need set subroutine 'set_inflag' to look for 'P ' bc. After this i need to call 'get_values(field)' subroutine, which interpolate and put the value in valint(ix,iy,iz,ie,ifld) array. And then this array will be available in userbc in .usr file, to set it on inflow boundary. c----------------------------------------------------------------------------------------------- Vatslav, you will have to use the neknek script that allows you to exchange data between two Nek5000 sessions that are run simultaneously. You should have a look at the neknek examples to understand how to set up your usr file. Some of the subroutines that will be useful to you are located in the following link: http://www.mcs.anl.gov/research/projects/nek5/docs/ html/multimesh_8f_source.html You will have to modify some of them to fit your needs since for example the subroutine ?set_inflag? is written to look for ?in? boundary conditions and replace them with ?v ?. You will need a subroutine that looks for ?in? and substitute it with either ?v ? or ?P ? depending on the which pipe you are at. Marco Hi, Neks! I have two pipes in my simulation. They are placed near each other on one axis with empty space between. One of them with periodic boundary conditions on z direction, another one - inflow -> outflow. How can I copy velocity slice from one of boundary on first pipe with periodic bc to the inflow boundary on second pipe? Regards, Vatslav c----------------------------------------------------------------------------------------------- Regards, Vatslav -------------- next part -------------- An HTML attachment was scrubbed... URL: ------------------------------ Message: 4 Date: Mon, 27 Mar 2017 11:31:53 +0200 From: nek5000-users at lists.mcs.anl.gov To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] Robin Boundary Condition -- Navier's Slip Length Message-ID: Content-Type: text/plain; charset="utf-8" Hi Neks, I wish to simulate a transitional channel flow whose wall respect a "slip-length" boundary condition, such as: $ [u + \delta \frac{\partial u}{\partial n}]_{wall}=0$ Where \delta is the slip length ^n | u u | |-->/ |----->/ | | / | / | | / | / | | / | / |___|/_______| /_____ | / ^ |/ v \delta No-slip Slip-length (a better sketch can be found here: http://www.nature.com/nmat/journal/v2/n4/fig_tab/nmat857_F1.html ) [http://www.nature.com/nmat/journal/v2/n4/images/nmat857-f1.gif] Figure 1 : Low-friction flows of liquid at nanopatterned ... www.nature.com Nature Materials journal covers a range of topics within materials science, from materials engineering and structural materials (metals, alloys, ceramics, composites ... I would like to know if this Robin boundary condition for velocity field is already implemented in the current code. Thank you Ciccio -------------- next part -------------- An HTML attachment was scrubbed... URL: ------------------------------ Message: 5 Date: Mon, 27 Mar 2017 13:56:02 +0200 From: nek5000-users at lists.mcs.anl.gov To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Interpolation between two meshes Message-ID: Content-Type: text/plain; charset="windows-1252"; Format="flowed" Hi Tony, I have encountered the same issue with g2gi when interpolating very large meshes. I don't know what is causing the issue but a workaround is to reduce the polynomial order. You obviously loose accuracy by doing this, but I still find it better than starting from scratch with the new mesh. Hope this helps. Best, Mattias On 03/27/2017 06:37 AM, nek5000-users at lists.mcs.anl.gov wrote: > Dear Neks, > > I have been using 'g2gi' to do interpolation between different meshes. > Recently, I have noticed that when I interpolate between two big > meshes (say 300000 elements in each mesh), the interpolation hangs at > 'call findpts' and never moves on. I tried increasing number of > processors and changing 'lpart', but none of these worked. > > I'm wondering what could cause the interpolation to hang at 'findpts'. > Has anyone encountered similar issue? > > Hope anyone could give me some advice. Thank you very much in advance. > > Best regards, > Tony > > > _______________________________________________ > 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: ------------------------------ _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users End of Nek5000-users Digest, Vol 97, Issue 27 ********************************************* -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Mar 27 11:21:52 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 27 Mar 2017 18:21:52 +0200 Subject: [Nek5000-users] Interpolation between two meshes In-Reply-To: References: Message-ID: Just give it a whirl. It's important for us to see if the latest version fixes your problem. I have some confidence that it will ;) -----Original message----- > From:nek5000-users at lists.mcs.anl.gov > Sent: Monday 27th March 2017 18:19 > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] Interpolation between two meshes > > Hi Stefan and Mattias, > > Thank you both for your kind advice. > > Stefan, I had a look at the new 'gfldr' subroutine. It seems that the spectral interpolation procedure is the same as before, however, the latest subroutine breaks down the number of fields to interpolate in one go. I still don't see why the old g2gi hangs > at 'findpts'. Is it mainly because of memory size? (I have been using my own copy of the legacy nek, so I'm quite keen on making it work with g2gi.) > > Mattias, I will give it a go with your suggestion. By reducing the polynomial order, did you mean the order of the old field or the order of the new geometry field, or both? > > Thank you again for both your help. > > Best regards, > Tony > > > ----------- > From: nek5000-users-bounces at lists.mcs.anl.gov on behalf of nek5000-users-request at lists.mcs.anl.gov > Sent: 27 March 2017 12:57 > To: nek5000-users at lists.mcs.anl.gov > Subject: Nek5000-users Digest, Vol 97, Issue 27 > Send Nek5000-users mailing list submissions to > ??????? nek5000-users at lists.mcs.anl.gov > > To subscribe or unsubscribe via the World Wide Web, visit > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > or, via email, send a message with subject or body 'help' to > ??????? nek5000-users-request at lists.mcs.anl.gov > > You can reach the person managing the list at > ??????? nek5000-users-owner at lists.mcs.anl.gov > > When replying, please edit your Subject line so it is more specific > than "Re: Contents of Nek5000-users digest..." > > > Today's Topics: > > ?? 1. Interpolation between two meshes (nek5000-users at lists.mcs.anl.gov) > ?? 2. Re: Interpolation between two meshes > ????? (nek5000-users at lists.mcs.anl.gov) > ?? 3. Re: Copy velocity slice from one boundary to another > ????? (nek5000-users at lists.mcs.anl.gov) > ?? 4. Robin Boundary Condition -- Navier's Slip Length > ????? (nek5000-users at lists.mcs.anl.gov) > ?? 5. Re: Interpolation between two meshes > ????? (nek5000-users at lists.mcs.anl.gov) > > > ---------------------------------------------------------------------- > > Message: 1 > Date: Mon, 27 Mar 2017 04:37:46 0000 > From: nek5000-users at lists.mcs.anl.gov > To: Nek5000 > Subject: [Nek5000-users] Interpolation between two meshes > Message-ID: > ??????? > Content-Type: text/plain; charset="iso-8859-1" > > Dear Neks, > > I have been using 'g2gi' to do interpolation between different meshes. Recently, I have noticed that when I interpolate between two big meshes (say 300000 elements in each mesh), the interpolation hangs at 'call findpts' and never moves on. I tried increasing > number of processors and changing 'lpart', but none of these worked. > > I'm wondering what could cause the interpolation to hang at 'findpts'. Has anyone encountered similar issue? > > Hope anyone could give me some advice. Thank you very much in advance. > > Best regards, > Tony > -------------- next part -------------- > An HTML attachment was scrubbed... > URL: > > > ------------------------------ > > Message: 2 > Date: Mon, 27 Mar 2017 09:47:37 0200 > From: nek5000-users at lists.mcs.anl.gov > To: nek5000-users at lists.mcs.anl.gov????? > Subject: Re: [Nek5000-users] Interpolation between two meshes > Message-ID: > ??????? > Content-Type: text/plain; charset=utf-8 > > Please update to the latest master. Note, g2gi was replaced by gfldr. > > Stefan > > -----Original message----- > > From:nek5000-users at lists.mcs.anl.gov > > Sent: Monday 27th March 2017 6:38 > > To: Nek5000 > > Subject: [Nek5000-users] Interpolation between two meshes > > > > Dear Neks, > > > > I have been using 'g2gi' to do interpolation between different meshes. Recently, I have?noticed that when I interpolate between two big meshes (say 300000 elements in each mesh), the interpolation hangs at 'call findpts' and never moves on. I tried increasing > >? number of processors and changing 'lpart', but none of these worked. > > > > I'm wondering what could cause the interpolation to hang at 'findpts'. Has anyone encountered similar issue? > > > > Hope anyone could give me some advice. Thank you very much in advance. > > > > Best regards, > > Tony > > _______________________________________________ > > Nek5000-users mailing list > > Nek5000-users at lists.mcs.anl.gov > > > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > ------------------------------ > > Message: 3 > Date: Mon, 27 Mar 2017 16:47:00 0700 > From: nek5000-users at lists.mcs.anl.gov > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] Copy velocity slice from one boundary to > ??????? another > Message-ID: > ??????? > Content-Type: text/plain; charset="utf-8" > > Thanks a lot for replying, your answer was very useful. > > I look on multimesh.f file. > As i understood, i need set subroutine 'set_inflag' to look for 'P? ' bc. > After this i need to call 'get_values(field)' subroutine, which interpolate > and put the value in valint(ix,iy,iz,ie,ifld) array. > And then this array will be available in userbc in .usr file, to set it on > inflow boundary. > > c----------------------------------------------------------------------------------------------- > > Vatslav, > you will have to use the neknek script that allows you to exchange data > between two Nek5000 sessions that are run simultaneously. You should have a > look at the neknek examples to understand how to set up your usr file. > Some of the subroutines that will be useful to you are located in the > following link: > http://www.mcs.anl.gov/research/projects/nek5/docs/ > html/multimesh_8f_source.html > You will have to modify some of them to fit your needs since for example > the subroutine ?set_inflag? is written to look for ?in? boundary conditions > and replace them with ?v? ?. You will need a subroutine that looks for ?in? > and substitute it with either ?v? ? or ?P? ? depending on the which pipe > you are at. > Marco > > Hi, Neks! > I have two pipes in my simulation. They are placed near each other on one > axis with empty space between. > One of them with periodic boundary conditions on z direction, another one - > inflow -> outflow. > How can I copy velocity slice from one of boundary on first pipe with > periodic bc to the inflow boundary on second pipe? > Regards, Vatslav > > c----------------------------------------------------------------------------------------------- > > Regards, Vatslav > -------------- next part -------------- > An HTML attachment was scrubbed... > URL: > > > ------------------------------ > > Message: 4 > Date: Mon, 27 Mar 2017 11:31:53 0200 > From: nek5000-users at lists.mcs.anl.gov > To: nek5000-users at lists.mcs.anl.gov > Subject: [Nek5000-users] Robin Boundary Condition -- Navier's Slip > ??????? Length > Message-ID: > ??????? > Content-Type: text/plain; charset="utf-8" > > Hi Neks, > I wish to simulate a transitional channel flow whose wall respect a > "slip-length" boundary condition, such as: > > $ [u \delta \frac{\partial u}{\partial n}]_{wall}=0$ > > Where \delta is the slip length > > ^n > |??????? u?????????????? u > |????? |-->/???????? |----->/ > |????? |?? /?????????? |????? / > |????? |? /??????????? |???? / > |????? | /???????????? |??? / > |___|/_______|?? /_____ > ?????????????????????? | /? ^ > ?????????????????????? |/?? v \delta > > No-slip?????? Slip-length > > (a better sketch can be found here: > http://www.nature.com/nmat/journal/v2/n4/fig_tab/nmat857_F1.html ) > > > Figure 1 : Low-friction flows of liquid at nanopatterned ... www.nature.com > Nature Materials journal covers a range of topics within materials science, from materials engineering and structural materials (metals, alloys, ceramics, composites ... > > > > I would like to know if this Robin boundary condition for velocity field is > already implemented in the current code. > > Thank you > > Ciccio > -------------- next part -------------- > An HTML attachment was scrubbed... > URL: > > > ------------------------------ > > Message: 5 > Date: Mon, 27 Mar 2017 13:56:02 0200 > From: nek5000-users at lists.mcs.anl.gov > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] Interpolation between two meshes > Message-ID: > ??????? > Content-Type: text/plain; charset="windows-1252"; Format="flowed" > > Hi Tony, > I have encountered the same issue with g2gi when interpolating very > large meshes. I don't know what is causing the issue but a workaround is > to reduce the polynomial order. You obviously loose accuracy by doing > this, but I still find it better than starting from scratch with the new > mesh. Hope this helps. > > Best, > Mattias > > > On 03/27/2017 06:37 AM, nek5000-users at lists.mcs.anl.gov wrote: > > Dear Neks, > > > > I have been using 'g2gi' to do interpolation between different meshes. > > Recently, I have noticed that when I interpolate between two big > > meshes (say 300000 elements in each mesh), the interpolation hangs at > > 'call findpts' and never moves on. I tried increasing number of > > processors and changing 'lpart', but none of these worked. > > > > I'm wondering what could cause the interpolation to hang at 'findpts'. > > Has anyone encountered similar issue? > > > > Hope anyone could give me some advice. Thank you very much in advance. > > > > Best regards, > > Tony > > > > > > _______________________________________________ > > 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: > > > ------------------------------ > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > End of Nek5000-users Digest, Vol 97, Issue 27 > ********************************************* > _______________________________________________ > 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 Mar 27 12:39:31 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 27 Mar 2017 17:39:31 +0000 Subject: [Nek5000-users] comp_vort3, nelt, conj_ht In-Reply-To: References: Message-ID: Thanks Sandeep. Your approach should work too. Can you elaborate more on the difference ? It may be because there is a dsavg() in comp_vort3... but I think I turned that off. Comp_vort3 might be a bit faster, but we normally don't care about performance for this routine, so I think your way is cleaner and thus better. I'm concerned however that they are different (which likely points to a problem in the new comp_vort3 routine). 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 27, 2017 11:16 AM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] comp_vort3, nelt, conj_ht Thank you Paul. Now comp_vort3 doesnt give zeros in the solid domain. What is the difference between comp_vort3 and the calculation of curl using call gradm1(dAxdx,dAxdy,dAxdz,t(1,1,1,1,1)) call gradm1(dAydx,dAydy,dAydz,t(1,1,1,1,2)) call gradm1(dAzdx,dAzdy,dAzdz,t(1,1,1,1,3)) call sub3(bfx1,dAzdy,dAydz,m) call sub3(bfy1,dAxdz,dAzdx,m) call sub3(bfz1,dAydx,dAxdy,m) ?When I compare the glsc3 of a curls computed by comp_vort3 and gradm1, there is a difference of 0.5% to 1%. Which procedure suits well, if I want to use u x curl in the userq Sincerely, Sandeep Hi Sandeep, This issue should now be resolved. comp_vort3() will now compute the curl of the supplied vector field over all elements, e=1,...,nelt. Moreover, prepost() has been modified to not put zeros in the velocity field when e > nelv. So, you should be able to do something like: call comp_vort3(curlv,w1,w2,u,v,w) call outpost(curlv(1,1),curlv(1,2),culrv(1,3),pr,t,' ') and have the right thing happen. 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, March 23, 2017 2:57 PM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] comp_vort3, nelt, conj_ht Hello Neks, I modified conj_ht example and defined three scalars. NEL>NELV. The domain of scalars is bigger than the fluid. I create a vector by taking the curl of three scalars, using common /myvort/ b1(lx1,ly1,lz1,lelt,3), call comp_vort3(b1,work1,work2,t(1,1,1,1,1), $ t(1,1,1,1,2),t(1,1,1,1,3)) b1 is computed correctly in the fluid domain, but is solid domain it showing zero. Can someone tell me how to modify the comp_vort3 subroutine, to correctly compute b1 over the entire domain. I tried to modify call dudxyz(work1,w,rym1,sym1,tym1,jacm1,2,2), changing the imsh=2 (the last second parameter in the above call), but the the result remains the same. I use the three components of computed b1 in userq Thank you in advance. Sincerely, Sandeep -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Mar 27 13:43:39 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 27 Mar 2017 20:43:39 +0200 Subject: [Nek5000-users] comp_vort3, nelt, conj_ht Message-ID: ?Hello Paul, Thank you for your advice. I compared visually, but difficult to locate what is the difference. Overall they seem to look the same. I compared the values of glsc3 obtained by vector comp_vort3 and the curl computed using gradm1 and the averaged values are off by 0.5% to 0.9% Sandeep ? -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Mar 27 21:02:49 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 28 Mar 2017 02:02:49 +0000 Subject: [Nek5000-users] Interpolation between two meshes In-Reply-To: References: Message-ID: Hi Stefan, Many thanks for your reply. I have tried the new 'gfldr' subroutine in two ways. First, I copied the whole 'gfldr.f' into my usr file and ran the interpolation with my legacy nek master code (tuned few lines to match the old byte_mpi.f format). The source field was read in successfully and I also confirmed the coordinates from the source field. However, the interpolation halted again at 'findpts' in 'gfldr_intp' subroutine. Second, I ran the interpolation directly with the latest master nek code. The same thing happened and the interpolation halted at 'findpts' and never moved on. In addition, I also tried reducing polynomial order (lx1) as Mattias suggested, but with no success. I really don't know what causes the problem when interpolating between two large meshes. Do you have any workaround? Please help me out. Thank you very much. Best regards, Tony ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov on behalf of nek5000-users-request at lists.mcs.anl.gov Sent: 27 March 2017 18:00 To: nek5000-users at lists.mcs.anl.gov Subject: Nek5000-users Digest, Vol 97, Issue 29 Send Nek5000-users mailing list submissions to nek5000-users at lists.mcs.anl.gov To subscribe or unsubscribe via the World Wide Web, visit https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users or, via email, send a message with subject or body 'help' to nek5000-users-request at lists.mcs.anl.gov You can reach the person managing the list at nek5000-users-owner at lists.mcs.anl.gov When replying, please edit your Subject line so it is more specific than "Re: Contents of Nek5000-users digest..." Today's Topics: 1. Re: Interpolation between two meshes (nek5000-users at lists.mcs.anl.gov) ---------------------------------------------------------------------- Message: 1 Date: Mon, 27 Mar 2017 18:21:52 +0200 From: nek5000-users at lists.mcs.anl.gov To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Interpolation between two meshes Message-ID: Content-Type: text/plain; charset=utf-8 Just give it a whirl. It's important for us to see if the latest version fixes your problem. I have some confidence that it will ;) -----Original message----- > From:nek5000-users at lists.mcs.anl.gov > Sent: Monday 27th March 2017 18:19 > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] Interpolation between two meshes > > Hi Stefan and Mattias, > > Thank you both for your kind advice. > > Stefan, I had a look at the new 'gfldr' subroutine. It seems that the spectral interpolation procedure is the same as before, however, the latest subroutine breaks down the number of fields to interpolate in one go. I still don't see why the old g2gi hangs > at 'findpts'. Is it mainly because of memory size? (I have been using my own copy of the legacy nek, so I'm quite keen on making it work with g2gi.) > > Mattias, I will give it a go with your suggestion. By reducing the polynomial order, did you mean the order of the old field or the order of the new geometry field, or both? > > Thank you again for both your help. > > Best regards, > Tony > > > ----------- > From: nek5000-users-bounces at lists.mcs.anl.gov on behalf of nek5000-users-request at lists.mcs.anl.gov > Sent: 27 March 2017 12:57 > To: nek5000-users at lists.mcs.anl.gov > Subject: Nek5000-users Digest, Vol 97, Issue 27 > Send Nek5000-users mailing list submissions to > ??????? nek5000-users at lists.mcs.anl.gov > > To subscribe or unsubscribe via the World Wide Web, visit > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > or, via email, send a message with subject or body 'help' to > ??????? nek5000-users-request at lists.mcs.anl.gov > > You can reach the person managing the list at > ??????? nek5000-users-owner at lists.mcs.anl.gov > > When replying, please edit your Subject line so it is more specific > than "Re: Contents of Nek5000-users digest..." > > > Today's Topics: > > ?? 1. Interpolation between two meshes (nek5000-users at lists.mcs.anl.gov) > ?? 2. Re: Interpolation between two meshes > ????? (nek5000-users at lists.mcs.anl.gov) > ?? 3. Re: Copy velocity slice from one boundary to another > ????? (nek5000-users at lists.mcs.anl.gov) > ?? 4. Robin Boundary Condition -- Navier's Slip Length > ????? (nek5000-users at lists.mcs.anl.gov) > ?? 5. Re: Interpolation between two meshes > ????? (nek5000-users at lists.mcs.anl.gov) > > > ---------------------------------------------------------------------- > > Message: 1 > Date: Mon, 27 Mar 2017 04:37:46 0000 > From: nek5000-users at lists.mcs.anl.gov > To: Nek5000 > Subject: [Nek5000-users] Interpolation between two meshes > Message-ID: > ??????? > Content-Type: text/plain; charset="iso-8859-1" > > Dear Neks, > > I have been using 'g2gi' to do interpolation between different meshes. Recently, I have noticed that when I interpolate between two big meshes (say 300000 elements in each mesh), the interpolation hangs at 'call findpts' and never moves on. I tried increasing > number of processors and changing 'lpart', but none of these worked. > > I'm wondering what could cause the interpolation to hang at 'findpts'. Has anyone encountered similar issue? > > Hope anyone could give me some advice. Thank you very much in advance. > > Best regards, > Tony > -------------- next part -------------- > An HTML attachment was scrubbed... > URL: > > > ------------------------------ > > Message: 2 > Date: Mon, 27 Mar 2017 09:47:37 0200 > From: nek5000-users at lists.mcs.anl.gov > To: nek5000-users at lists.mcs.anl.gov????? > Subject: Re: [Nek5000-users] Interpolation between two meshes > Message-ID: > ??????? > Content-Type: text/plain; charset=utf-8 > > Please update to the latest master. Note, g2gi was replaced by gfldr. > > Stefan > > -----Original message----- > > From:nek5000-users at lists.mcs.anl.gov > > Sent: Monday 27th March 2017 6:38 > > To: Nek5000 > > Subject: [Nek5000-users] Interpolation between two meshes > > > > Dear Neks, > > > > I have been using 'g2gi' to do interpolation between different meshes. Recently, I have?noticed that when I interpolate between two big meshes (say 300000 elements in each mesh), the interpolation hangs at 'call findpts' and never moves on. I tried increasing > >? number of processors and changing 'lpart', but none of these worked. > > > > I'm wondering what could cause the interpolation to hang at 'findpts'. Has anyone encountered similar issue? > > > > Hope anyone could give me some advice. Thank you very much in advance. > > > > Best regards, > > Tony > > _______________________________________________ > > Nek5000-users mailing list > > Nek5000-users at lists.mcs.anl.gov > > > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > ------------------------------ > > Message: 3 > Date: Mon, 27 Mar 2017 16:47:00 0700 > From: nek5000-users at lists.mcs.anl.gov > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] Copy velocity slice from one boundary to > ??????? another > Message-ID: > ??????? > Content-Type: text/plain; charset="utf-8" > > Thanks a lot for replying, your answer was very useful. > > I look on multimesh.f file. > As i understood, i need set subroutine 'set_inflag' to look for 'P? ' bc. > After this i need to call 'get_values(field)' subroutine, which interpolate > and put the value in valint(ix,iy,iz,ie,ifld) array. > And then this array will be available in userbc in .usr file, to set it on > inflow boundary. > > c----------------------------------------------------------------------------------------------- > > Vatslav, > you will have to use the neknek script that allows you to exchange data > between two Nek5000 sessions that are run simultaneously. You should have a > look at the neknek examples to understand how to set up your usr file. > Some of the subroutines that will be useful to you are located in the > following link: > http://www.mcs.anl.gov/research/projects/nek5/docs/ > html/multimesh_8f_source.html > You will have to modify some of them to fit your needs since for example > the subroutine ?set_inflag? is written to look for ?in? boundary conditions > and replace them with ?v? ?. You will need a subroutine that looks for ?in? > and substitute it with either ?v? ? or ?P? ? depending on the which pipe > you are at. > Marco > > Hi, Neks! > I have two pipes in my simulation. They are placed near each other on one > axis with empty space between. > One of them with periodic boundary conditions on z direction, another one - > inflow -> outflow. > How can I copy velocity slice from one of boundary on first pipe with > periodic bc to the inflow boundary on second pipe? > Regards, Vatslav > > c----------------------------------------------------------------------------------------------- > > Regards, Vatslav > -------------- next part -------------- > An HTML attachment was scrubbed... > URL: > > > ------------------------------ > > Message: 4 > Date: Mon, 27 Mar 2017 11:31:53 0200 > From: nek5000-users at lists.mcs.anl.gov > To: nek5000-users at lists.mcs.anl.gov > Subject: [Nek5000-users] Robin Boundary Condition -- Navier's Slip > ??????? Length > Message-ID: > ??????? > Content-Type: text/plain; charset="utf-8" > > Hi Neks, > I wish to simulate a transitional channel flow whose wall respect a > "slip-length" boundary condition, such as: > > $ [u \delta \frac{\partial u}{\partial n}]_{wall}=0$ > > Where \delta is the slip length > > ^n > |??????? u?????????????? u > |????? |-->/???????? |----->/ > |????? |?? /?????????? |????? / > |????? |? /??????????? |???? / > |????? | /???????????? |??? / > |___|/_______|?? /_____ > ?????????????????????? | /? ^ > ?????????????????????? |/?? v \delta > > No-slip?????? Slip-length > > (a better sketch can be found here: > http://www.nature.com/nmat/journal/v2/n4/fig_tab/nmat857_F1.html ) > > > Figure 1 : Low-friction flows of liquid at nanopatterned ... www.nature.com > Nature Materials journal covers a range of topics within materials science, from materials engineering and structural materials (metals, alloys, ceramics, composites ... > > > > I would like to know if this Robin boundary condition for velocity field is > already implemented in the current code. > > Thank you > > Ciccio > -------------- next part -------------- > An HTML attachment was scrubbed... > URL: > > > ------------------------------ > > Message: 5 > Date: Mon, 27 Mar 2017 13:56:02 0200 > From: nek5000-users at lists.mcs.anl.gov > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] Interpolation between two meshes > Message-ID: > ??????? > Content-Type: text/plain; charset="windows-1252"; Format="flowed" > > Hi Tony, > I have encountered the same issue with g2gi when interpolating very > large meshes. I don't know what is causing the issue but a workaround is > to reduce the polynomial order. You obviously loose accuracy by doing > this, but I still find it better than starting from scratch with the new > mesh. Hope this helps. > > Best, > Mattias > > > On 03/27/2017 06:37 AM, nek5000-users at lists.mcs.anl.gov wrote: > > Dear Neks, > > > > I have been using 'g2gi' to do interpolation between different meshes. > > Recently, I have noticed that when I interpolate between two big > > meshes (say 300000 elements in each mesh), the interpolation hangs at > > 'call findpts' and never moves on. I tried increasing number of > > processors and changing 'lpart', but none of these worked. > > > > I'm wondering what could cause the interpolation to hang at 'findpts'. > > Has anyone encountered similar issue? > > > > Hope anyone could give me some advice. Thank you very much in advance. > > > > Best regards, > > Tony > > > > > > _______________________________________________ > > 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: > > > ------------------------------ > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > End of Nek5000-users Digest, Vol 97, Issue 27 > ********************************************* > _______________________________________________ > 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 End of Nek5000-users Digest, Vol 97, Issue 29 ********************************************* -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Mar 28 02:57:33 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 28 Mar 2017 09:57:33 +0200 Subject: [Nek5000-users] Interpolation between two meshes In-Reply-To: References: Message-ID: Can you please provide more information about your case (machine, compiler) and include the .usr and log file. If the case is reasonably small, I can try to run it myself. -----Original message----- > From:nek5000-users at lists.mcs.anl.gov > Sent: Tuesday 28th March 2017 4:03 > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] Interpolation between two meshes > > Hi Stefan, > > Many thanks for your reply. I have tried the new 'gfldr' subroutine in two ways. > > First, I copied the whole 'gfldr.f' into my usr file and ran the interpolation with my legacy nek master code > (tuned few lines to match the old byte_mpi.f format). The source field was read in successfully and I also confirmed the coordinates from the source field. However, the interpolation halted again at 'findpts' in 'gfldr_intp' subroutine. > > Second, I ran the interpolation directly with the latest master nek code. The same thing happened and the interpolation halted at 'findpts' and never moved on. > > In addition, I also tried reducing polynomial order (lx1) as Mattias suggested, but with no success. > > I really don't know what causes the problem when interpolating between two large meshes. Do you have any workaround? > > Please help me out. Thank you very much. > > Best regards, > Tony > > > ----------- > From: nek5000-users-bounces at lists.mcs.anl.gov on behalf of nek5000-users-request at lists.mcs.anl.gov > Sent: 27 March 2017 18:00 > To: nek5000-users at lists.mcs.anl.gov > Subject: Nek5000-users Digest, Vol 97, Issue 29 > Send Nek5000-users mailing list submissions to > ??????? nek5000-users at lists.mcs.anl.gov > > To subscribe or unsubscribe via the World Wide Web, visit > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > or, via email, send a message with subject or body 'help' to > ??????? nek5000-users-request at lists.mcs.anl.gov > > You can reach the person managing the list at > ??????? nek5000-users-owner at lists.mcs.anl.gov > > When replying, please edit your Subject line so it is more specific > than "Re: Contents of Nek5000-users digest..." > > > Today's Topics: > > ?? 1. Re: Interpolation between two meshes > ????? (nek5000-users at lists.mcs.anl.gov) > > > ---------------------------------------------------------------------- > > Message: 1 > Date: Mon, 27 Mar 2017 18:21:52 0200 > From: nek5000-users at lists.mcs.anl.gov > To: nek5000-users at lists.mcs.anl.gov????? > Subject: Re: [Nek5000-users] Interpolation between two meshes > Message-ID: > ??????? > Content-Type: text/plain; charset=utf-8 > > Just give it a whirl. > It's important for us to see if the latest version fixes your problem. I have some confidence that it will ;) > ? > -----Original message----- > > From:nek5000-users at lists.mcs.anl.gov > > Sent: Monday 27th March 2017 18:19 > > To: nek5000-users at lists.mcs.anl.gov > > Subject: Re: [Nek5000-users] Interpolation between two meshes > > > > Hi Stefan and Mattias, > > > > Thank you both for your kind advice. > > > > Stefan, I had a look at the new 'gfldr' subroutine. It seems that the spectral interpolation procedure is the same as before, however, the latest subroutine breaks down the number of fields to interpolate in one go. I still don't see why the old g2gi hangs > >? at 'findpts'. Is it mainly because of memory size? (I have been using my own copy of the legacy nek, so I'm quite keen on making it work with g2gi.) > > > > Mattias, I will give it a go with your suggestion. By reducing the polynomial order, did you mean the order of the old field or the order of the new geometry field, or both? > > > > Thank you again for both your help. > > > > Best regards, > > Tony > > > > > > ----------- > > From: nek5000-users-bounces at lists.mcs.anl.gov on behalf of nek5000-users-request at lists.mcs.anl.gov > > Sent: 27 March 2017 12:57 > > To: nek5000-users at lists.mcs.anl.gov > > Subject: Nek5000-users Digest, Vol 97, Issue 27 > > Send Nek5000-users mailing list submissions to > > ??????? nek5000-users at lists.mcs.anl.gov > > > > To subscribe or unsubscribe via the World Wide Web, visit > > > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > or, via email, send a message with subject or body 'help' to > > ??????? nek5000-users-request at lists.mcs.anl.gov > > > > You can reach the person managing the list at > > ??????? nek5000-users-owner at lists.mcs.anl.gov > > > > When replying, please edit your Subject line so it is more specific > > than "Re: Contents of Nek5000-users digest..." > > > > > > Today's Topics: > > > > ?? 1. Interpolation between two meshes (nek5000-users at lists.mcs.anl.gov) > > ?? 2. Re: Interpolation between two meshes > > ????? (nek5000-users at lists.mcs.anl.gov) > > ?? 3. Re: Copy velocity slice from one boundary to another > > ????? (nek5000-users at lists.mcs.anl.gov) > > ?? 4. Robin Boundary Condition -- Navier's Slip Length > > ????? (nek5000-users at lists.mcs.anl.gov) > > ?? 5. Re: Interpolation between two meshes > > ????? (nek5000-users at lists.mcs.anl.gov) > > > > > > ---------------------------------------------------------------------- > > > > Message: 1 > > Date: Mon, 27 Mar 2017 04:37:46 0000 > > From: nek5000-users at lists.mcs.anl.gov > > To: Nek5000 > > Subject: [Nek5000-users] Interpolation between two meshes > > Message-ID: > > ??????? > > Content-Type: text/plain; charset="iso-8859-1" > > > > Dear Neks, > > > > I have been using 'g2gi' to do interpolation between different meshes. Recently, I have noticed that when I interpolate between two big meshes (say 300000 elements in each mesh), the interpolation hangs at 'call findpts' and never moves on. I tried increasing > >? number of processors and changing 'lpart', but none of these worked. > > > > I'm wondering what could cause the interpolation to hang at 'findpts'. Has anyone encountered similar issue? > > > > Hope anyone could give me some advice. Thank you very much in advance. > > > > Best regards, > > Tony > > -------------- next part -------------- > > An HTML attachment was scrubbed... > > URL: < <>http://lists.mcs.anl.gov/pipermail/nek5000-users/attachments/20170327/b238e605/attachment-0001.html >> > > > > ------------------------------ > > > > Message: 2 > > Date: Mon, 27 Mar 2017 09:47:37 0200 > > From: nek5000-users at lists.mcs.anl.gov > > To: nek5000-users at lists.mcs.anl.gov????? > > Subject: Re: [Nek5000-users] Interpolation between two meshes > > Message-ID: > > ??????? > > Content-Type: text/plain; charset=utf-8 > > > > Please update to the latest master. Note, g2gi was replaced by gfldr. > > > > Stefan > > > > -----Original message----- > > > From:nek5000-users at lists.mcs.anl.gov > > > Sent: Monday 27th March 2017 6:38 > > > To: Nek5000 > > > Subject: [Nek5000-users] Interpolation between two meshes > > > > > > Dear Neks, > > > > > > I have been using 'g2gi' to do interpolation between different meshes. Recently, I have?noticed that when I interpolate between two big meshes (say 300000 elements in each mesh), the interpolation hangs at 'call findpts' and never moves on. I tried increasing > > >? number of processors and changing 'lpart', but none of these worked. > > > > > > I'm wondering what could cause the interpolation to hang at 'findpts'. Has anyone encountered similar issue? > > > > > > Hope anyone could give me some advice. Thank you very much in advance. > > > > > > Best regards, > > > Tony > > > _______________________________________________ > > > Nek5000-users mailing list > > > Nek5000-users at lists.mcs.anl.gov > > > > > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > > > > > ------------------------------ > > > > Message: 3 > > Date: Mon, 27 Mar 2017 16:47:00 0700 > > From: nek5000-users at lists.mcs.anl.gov > > To: nek5000-users at lists.mcs.anl.gov > > Subject: Re: [Nek5000-users] Copy velocity slice from one boundary to > > ??????? another > > Message-ID: > > ??????? > > Content-Type: text/plain; charset="utf-8" > > > > Thanks a lot for replying, your answer was very useful. > > > > I look on multimesh.f file. > > As i understood, i need set subroutine 'set_inflag' to look for 'P? ' bc. > > After this i need to call 'get_values(field)' subroutine, which interpolate > > and put the value in valint(ix,iy,iz,ie,ifld) array. > > And then this array will be available in userbc in .usr file, to set it on > > inflow boundary. > > > > c----------------------------------------------------------------------------------------------- > > > > Vatslav, > > you will have to use the neknek script that allows you to exchange data > > between two Nek5000 sessions that are run simultaneously. You should have a > > look at the neknek examples to understand how to set up your usr file. > > Some of the subroutines that will be useful to you are located in the > > following link: > > http://www.mcs.anl.gov/research/projects/nek5/docs/ > > > html/multimesh_8f_source.html > > You will have to modify some of them to fit your needs since for example > > the subroutine ?set_inflag? is written to look for ?in? boundary conditions > > and replace them with ?v? ?. You will need a subroutine that looks for ?in? > > and substitute it with either ?v? ? or ?P? ? depending on the which pipe > > you are at. > > Marco > > > > Hi, Neks! > > I have two pipes in my simulation. They are placed near each other on one > > axis with empty space between. > > One of them with periodic boundary conditions on z direction, another one - > > inflow -> outflow. > > How can I copy velocity slice from one of boundary on first pipe with > > periodic bc to the inflow boundary on second pipe? > > Regards, Vatslav > > > > c----------------------------------------------------------------------------------------------- > > > > Regards, Vatslav > > -------------- next part -------------- > > An HTML attachment was scrubbed... > > URL: < <>http://lists.mcs.anl.gov/pipermail/nek5000-users/attachments/20170327/92c78de8/attachment-0001.html >> > > > > ------------------------------ > > > > Message: 4 > > Date: Mon, 27 Mar 2017 11:31:53 0200 > > From: nek5000-users at lists.mcs.anl.gov > > To: nek5000-users at lists.mcs.anl.gov > > Subject: [Nek5000-users] Robin Boundary Condition -- Navier's Slip > > ??????? Length > > Message-ID: > > ??????? > > Content-Type: text/plain; charset="utf-8" > > > > Hi Neks, > > I wish to simulate a transitional channel flow whose wall respect a > > "slip-length" boundary condition, such as: > > > > $ [u? \delta \frac{\partial u}{\partial n}]_{wall}=0$ > > > > Where \delta is the slip length > > > > ^n > > |??????? u?????????????? u > > |????? |-->/???????? |----->/ > > |????? |?? /?????????? |????? / > > |????? |? /??????????? |???? / > > |????? | /???????????? |??? / > > |___|/_______|?? /_____ > > ?????????????????????? | /? ^ > > ?????????????????????? |/?? v \delta > > > > No-slip?????? Slip-length > > > > (a better sketch can be found here: > > http://www.nature.com/nmat/journal/v2/n4/fig_tab/nmat857_F1.html > > ) > > > >? > > > Figure 1 : Low-friction flows of liquid at nanopatterned ... >www.nature.com > > Nature Materials journal covers a range of topics within materials science, from materials engineering and structural materials (metals, alloys, ceramics, composites ... > > > > > > > > I would like to know if this Robin boundary condition for velocity field is > > already implemented in the current code. > > > > Thank you > > > > Ciccio > > -------------- next part -------------- > > An HTML attachment was scrubbed... > > URL: < <>http://lists.mcs.anl.gov/pipermail/nek5000-users/attachments/20170327/9922e2e7/attachment-0001.html >> > > > > ------------------------------ > > > > Message: 5 > > Date: Mon, 27 Mar 2017 13:56:02 0200 > > From: nek5000-users at lists.mcs.anl.gov > > To: nek5000-users at lists.mcs.anl.gov > > Subject: Re: [Nek5000-users] Interpolation between two meshes > > Message-ID: > > ??????? > > Content-Type: text/plain; charset="windows-1252"; Format="flowed" > > > > Hi Tony, > > I have encountered the same issue with g2gi when interpolating very > > large meshes. I don't know what is causing the issue but a workaround is > > to reduce the polynomial order. You obviously loose accuracy by doing > > this, but I still find it better than starting from scratch with the new > > mesh. Hope this helps. > > > > Best, > > Mattias > > > > > > On 03/27/2017 06:37 AM, nek5000-users at lists.mcs.anl.gov wrote: > > > Dear Neks, > > > > > > I have been using 'g2gi' to do interpolation between different meshes. > > > Recently, I have noticed that when I interpolate between two big > > > meshes (say 300000 elements in each mesh), the interpolation hangs at > > > 'call findpts' and never moves on. I tried increasing number of > > > processors and changing 'lpart', but none of these worked. > > > > > > I'm wondering what could cause the interpolation to hang at 'findpts'. > > > Has anyone encountered similar issue? > > > > > > Hope anyone could give me some advice. Thank you very much in advance. > > > > > > Best regards, > > > Tony > > > > > > > > > _______________________________________________ > > > 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: < <>http://lists.mcs.anl.gov/pipermail/nek5000-users/attachments/20170327/031d792f/attachment.html >> > > > > ------------------------------ > > > > _______________________________________________ > > Nek5000-users mailing list > > Nek5000-users at lists.mcs.anl.gov > > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > > > > > End of Nek5000-users Digest, Vol 97, Issue 27 > > ********************************************* > > _______________________________________________ > > 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 > > > End of Nek5000-users Digest, Vol 97, Issue 29 > ********************************************* > _______________________________________________ > 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 Mar 28 07:18:56 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 28 Mar 2017 12:18:56 +0000 Subject: [Nek5000-users] Copy velocity slice from one boundary to another In-Reply-To: References: Message-ID: Vatslav, what I do and it seems to work for my case is the following. Let assume you have two pipes (pipe 1 with periodic bc and pipe 2 with inlet/outlet), and that the flow is moving from pipe 1 to pipe 2. The solution from pipe 1 is interpolated to pipe 2 and used as inlet condition. In a separate subroutine, do the following: * in pipe 1, look for the boundary faces with P boundary condition that will be used for the interpolation and substitute P with inP. * in pipe 2, look for the boundary faces with v boundary condition and substitute v with inV. In a subroutine analogous to set_inflag: * in pipe 1, collect boundary faces with flag inP, set intflag to 1 for this boundary face, and substitute back boundary condition to P. * in pip2, do the same: inV - > v After, this step, you have marked all boundary faces that will be involved in the interpolation process in Nek5000. From this point, the steps are similar to what is done in the examples. All of this is done in my usr file. Hope this help, Marco On Mar 27, 2017, at 5:47 AM, nek5000-users at lists.mcs.anl.gov wrote: Thanks a lot for replying, your answer was very useful. I look on multimesh.f file. As i understood, i need set subroutine 'set_inflag' to look for 'P ' bc. After this i need to call 'get_values(field)' subroutine, which interpolate and put the value in valint(ix,iy,iz,ie,ifld) array. And then this array will be available in userbc in .usr file, to set it on inflow boundary. c----------------------------------------------------------------------------------------------- Vatslav, you will have to use the neknek script that allows you to exchange data between two Nek5000 sessions that are run simultaneously. You should have a look at the neknek examples to understand how to set up your usr file. Some of the subroutines that will be useful to you are located in the following link: http://www.mcs.anl.gov/research/projects/nek5/docs/html/multimesh_8f_source.html You will have to modify some of them to fit your needs since for example the subroutine ?set_inflag? is written to look for ?in? boundary conditions and replace them with ?v ?. You will need a subroutine that looks for ?in? and substitute it with either ?v ? or ?P ? depending on the which pipe you are at. Marco Hi, Neks! I have two pipes in my simulation. They are placed near each other on one axis with empty space between. One of them with periodic boundary conditions on z direction, another one - inflow -> outflow. How can I copy velocity slice from one of boundary on first pipe with periodic bc to the inflow boundary on second pipe? Regards, Vatslav c----------------------------------------------------------------------------------------------- Regards, Vatslav _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Mar 28 10:48:58 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 28 Mar 2017 15:48:58 +0000 Subject: [Nek5000-users] Undefined reference to 'intp_do' Message-ID: Dear Neks, I am using the latest Nek5000, which replaced the old interpolation intpts() by the optional intp.h module. When I call the subroutines of ?intp_setup? and ?intp_do? in the ?intp.f?, there is always the compilation error of undefined reference to ?intp_setup? and ?intp_do?. How should I fix the error? Could anyone help me out? Thanks, Peng From nek5000-users at lists.mcs.anl.gov Tue Mar 28 11:23:57 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 28 Mar 2017 18:23:57 +0200 Subject: [Nek5000-users] Undefined reference to 'intp_do' In-Reply-To: References: Message-ID: There is intp.f (designed for .usr) which does not get compiled by default. Make sure define INTP_MAXPTS (e.g. in your SIZE) otherwise you the error you are referring to. On 28 Mar 2017, at 17:50, "nek5000-users at lists.mcs.anl.gov " > wrote: Dear Neks, I am using the latest Nek5000, which replaced the old interpolation intpts() by the optional intp.h module. When I call the subroutines of ?intp_setup? and ?intp_do? in the ?intp.f?, there is always the? compilation error of undefined reference to ?intp_setup? and ?intp_do?. How should I fix the error? Could anyone help me out? Thanks, Peng _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Mar 28 12:17:05 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 28 Mar 2017 17:17:05 +0000 Subject: [Nek5000-users] Undefined reference to 'intp_do' In-Reply-To: References: Message-ID: OK, thank you for your help. It works now. > On Mar 28, 2017, at 1:00 PM, nek5000-users-request at lists.mcs.anl.gov wrote: > > Send Nek5000-users mailing list submissions to > nek5000-users at lists.mcs.anl.gov > > To subscribe or unsubscribe via the World Wide Web, visit > https://urldefense.proofpoint.com/v2/url?u=https-3A__lists.mcs.anl.gov_mailman_listinfo_nek5000-2Dusers&d=DwICAg&c=y2w-uYmhgFWijp_IQN0DhA&r=QEl5evD27KmYmPJRHh_RJPXwtG0VKYwu68jKU6Xd1hw&m=pgFhQyncOlIywpCNAntdrPtvEgnA_jlh8gX6L84LjEQ&s=MFXAhrrmYh8voZLzYQ0hpe7aaeAElF6EOM5I6NqvoWo&e= > or, via email, send a message with subject or body 'help' to > nek5000-users-request at lists.mcs.anl.gov > > You can reach the person managing the list at > nek5000-users-owner at lists.mcs.anl.gov > > When replying, please edit your Subject line so it is more specific > than "Re: Contents of Nek5000-users digest..." > > > Today's Topics: > > 1. Undefined reference to 'intp_do' (nek5000-users at lists.mcs.anl.gov) > 2. Re: Undefined reference to 'intp_do' > (nek5000-users at lists.mcs.anl.gov) > > > ---------------------------------------------------------------------- > > Message: 1 > Date: Tue, 28 Mar 2017 15:48:58 +0000 > From: nek5000-users at lists.mcs.anl.gov > To: "nek5000-users at lists.mcs.anl.gov" > > Subject: [Nek5000-users] Undefined reference to 'intp_do' > Message-ID: > > Content-Type: text/plain; charset="utf-8" > > Dear Neks, > > I am using the latest Nek5000, which replaced the old interpolation intpts() > by the optional intp.h module. > When I call the subroutines of ?intp_setup? and ?intp_do? in the ?intp.f?, > there is always the compilation error of undefined reference to ?intp_setup? and ?intp_do?. > > How should I fix the error? > Could anyone help me out? > > Thanks, > Peng > > > ------------------------------ > > Message: 2 > Date: Tue, 28 Mar 2017 18:23:57 +0200 > From: nek5000-users at lists.mcs.anl.gov > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] Undefined reference to 'intp_do' > Message-ID: > > Content-Type: text/plain; charset="utf-8" > > There is intp.f (designed for .usr) which does not get compiled by default. Make sure define INTP_MAXPTS (e.g. in your SIZE) otherwise you the error you are referring to. > > On 28 Mar 2017, at 17:50, "nek5000-users at lists.mcs.anl.gov " > wrote: > > Dear Neks, > > I am using the latest Nek5000, which replaced the old interpolation intpts() > by the optional intp.h module. > When I call the subroutines of ?intp_setup? and ?intp_do? in the ?intp.f?, > there is always the? compilation error of undefined reference to ?intp_setup? and ?intp_do?. > > How should I fix the error? > Could anyone help me out? > > Thanks, > Peng > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://urldefense.proofpoint.com/v2/url?u=https-3A__lists.mcs.anl.gov_mailman_listinfo_nek5000-2Dusers&d=DwICAg&c=y2w-uYmhgFWijp_IQN0DhA&r=QEl5evD27KmYmPJRHh_RJPXwtG0VKYwu68jKU6Xd1hw&m=pgFhQyncOlIywpCNAntdrPtvEgnA_jlh8gX6L84LjEQ&s=MFXAhrrmYh8voZLzYQ0hpe7aaeAElF6EOM5I6NqvoWo&e= > > -------------- next part -------------- > An HTML attachment was scrubbed... > URL: > > ------------------------------ > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://urldefense.proofpoint.com/v2/url?u=https-3A__lists.mcs.anl.gov_mailman_listinfo_nek5000-2Dusers&d=DwICAg&c=y2w-uYmhgFWijp_IQN0DhA&r=QEl5evD27KmYmPJRHh_RJPXwtG0VKYwu68jKU6Xd1hw&m=pgFhQyncOlIywpCNAntdrPtvEgnA_jlh8gX6L84LjEQ&s=MFXAhrrmYh8voZLzYQ0hpe7aaeAElF6EOM5I6NqvoWo&e= > > > End of Nek5000-users Digest, Vol 97, Issue 32 > ********************************************* From nek5000-users at lists.mcs.anl.gov Tue Mar 28 13:27:11 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 28 Mar 2017 18:27:11 +0000 Subject: [Nek5000-users] Project a solution onto a polynomial space Message-ID: Dear all, Thank you for your responses. I've taken some time to think about your comments and I have some more questions: Paul: Are you suggesting to represent the moments on the 2*M grid and not project it back onto the original space? I am assuming this means that the moments would be in the space of polynomials of order 2*N. Am I understanding correctly? Aleks: You talk about truncating to polyn. order < lx1. Would this have the same effect as projecting onto the original space? Also, is the "cut_off_filter" subroutine the correct way to implement this? Thanks, Juan Diego -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Mar 28 14:51:04 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 28 Mar 2017 19:51:04 +0000 Subject: [Nek5000-users] Interpolation between two meshes In-Reply-To: References: Message-ID: Hi Stefan, Many thanks for your reply. I'm running my simulations on ARCHER (Cray XC30 supercomputer) and I'm using the Intel compiler. The current simulation has 469500 elements with polynomial order of 7. The source field I used for interpolation has 383700 elements with the same polynomial order. The size of the source field is about 10GB. I'm not sure if it can be easily transferred. But I have attached my .usr and log files herewith (also the gfldr.f with few added checking lines). I ran the interpolation using 720 processors. Please have a look and let me know if you need further information about the case. Thank you very much for you help. Best regards, Tony ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov on behalf of nek5000-users-request at lists.mcs.anl.gov Sent: 28 March 2017 13:19 To: nek5000-users at lists.mcs.anl.gov Subject: Nek5000-users Digest, Vol 97, Issue 31 Send Nek5000-users mailing list submissions to nek5000-users at lists.mcs.anl.gov To subscribe or unsubscribe via the World Wide Web, visit https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users or, via email, send a message with subject or body 'help' to nek5000-users-request at lists.mcs.anl.gov You can reach the person managing the list at nek5000-users-owner at lists.mcs.anl.gov When replying, please edit your Subject line so it is more specific than "Re: Contents of Nek5000-users digest..." Today's Topics: 1. Re: Interpolation between two meshes (nek5000-users at lists.mcs.anl.gov) 2. Re: Copy velocity slice from one boundary to another (nek5000-users at lists.mcs.anl.gov) ---------------------------------------------------------------------- Message: 1 Date: Tue, 28 Mar 2017 09:57:33 +0200 From: nek5000-users at lists.mcs.anl.gov To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Interpolation between two meshes Message-ID: Content-Type: text/plain; charset=utf-8 Can you please provide more information about your case (machine, compiler) and include the .usr and log file. If the case is reasonably small, I can try to run it myself. -----Original message----- > From:nek5000-users at lists.mcs.anl.gov > Sent: Tuesday 28th March 2017 4:03 > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] Interpolation between two meshes > > Hi Stefan, > > Many thanks for your reply. I have tried the new 'gfldr' subroutine in two ways. > > First, I copied the whole 'gfldr.f' into my usr file and ran the interpolation with my legacy nek master code > (tuned few lines to match the old byte_mpi.f format). The source field was read in successfully and I also confirmed the coordinates from the source field. However, the interpolation halted again at 'findpts' in 'gfldr_intp' subroutine. > > Second, I ran the interpolation directly with the latest master nek code. The same thing happened and the interpolation halted at 'findpts' and never moved on. > > In addition, I also tried reducing polynomial order (lx1) as Mattias suggested, but with no success. > > I really don't know what causes the problem when interpolating between two large meshes. Do you have any workaround? > > Please help me out. Thank you very much. > > Best regards, > Tony > > > ----------- > From: nek5000-users-bounces at lists.mcs.anl.gov on behalf of nek5000-users-request at lists.mcs.anl.gov > Sent: 27 March 2017 18:00 > To: nek5000-users at lists.mcs.anl.gov > Subject: Nek5000-users Digest, Vol 97, Issue 29 > Send Nek5000-users mailing list submissions to > ??????? nek5000-users at lists.mcs.anl.gov > > To subscribe or unsubscribe via the World Wide Web, visit > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > or, via email, send a message with subject or body 'help' to > ??????? nek5000-users-request at lists.mcs.anl.gov > > You can reach the person managing the list at > ??????? nek5000-users-owner at lists.mcs.anl.gov > > When replying, please edit your Subject line so it is more specific > than "Re: Contents of Nek5000-users digest..." > > > Today's Topics: > > ?? 1. Re: Interpolation between two meshes > ????? (nek5000-users at lists.mcs.anl.gov) > > > ---------------------------------------------------------------------- > > Message: 1 > Date: Mon, 27 Mar 2017 18:21:52 0200 > From: nek5000-users at lists.mcs.anl.gov > To: nek5000-users at lists.mcs.anl.gov????? > Subject: Re: [Nek5000-users] Interpolation between two meshes > Message-ID: > ??????? > Content-Type: text/plain; charset=utf-8 > > Just give it a whirl. > It's important for us to see if the latest version fixes your problem. I have some confidence that it will ;) > ? > -----Original message----- > > From:nek5000-users at lists.mcs.anl.gov > > Sent: Monday 27th March 2017 18:19 > > To: nek5000-users at lists.mcs.anl.gov > > Subject: Re: [Nek5000-users] Interpolation between two meshes > > > > Hi Stefan and Mattias, > > > > Thank you both for your kind advice. > > > > Stefan, I had a look at the new 'gfldr' subroutine. It seems that the spectral interpolation procedure is the same as before, however, the latest subroutine breaks down the number of fields to interpolate in one go. I still don't see why the old g2gi hangs > >? at 'findpts'. Is it mainly because of memory size? (I have been using my own copy of the legacy nek, so I'm quite keen on making it work with g2gi.) > > > > Mattias, I will give it a go with your suggestion. By reducing the polynomial order, did you mean the order of the old field or the order of the new geometry field, or both? > > > > Thank you again for both your help. > > > > Best regards, > > Tony > > > > > > ----------- > > From: nek5000-users-bounces at lists.mcs.anl.gov on behalf of nek5000-users-request at lists.mcs.anl.gov > > Sent: 27 March 2017 12:57 > > To: nek5000-users at lists.mcs.anl.gov > > Subject: Nek5000-users Digest, Vol 97, Issue 27 > > Send Nek5000-users mailing list submissions to > > ??????? nek5000-users at lists.mcs.anl.gov > > > > To subscribe or unsubscribe via the World Wide Web, visit > > > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > or, via email, send a message with subject or body 'help' to > > ??????? nek5000-users-request at lists.mcs.anl.gov > > > > You can reach the person managing the list at > > ??????? nek5000-users-owner at lists.mcs.anl.gov > > > > When replying, please edit your Subject line so it is more specific > > than "Re: Contents of Nek5000-users digest..." > > > > > > Today's Topics: > > > > ?? 1. Interpolation between two meshes (nek5000-users at lists.mcs.anl.gov) > > ?? 2. Re: Interpolation between two meshes > > ????? (nek5000-users at lists.mcs.anl.gov) > > ?? 3. Re: Copy velocity slice from one boundary to another > > ????? (nek5000-users at lists.mcs.anl.gov) > > ?? 4. Robin Boundary Condition -- Navier's Slip Length > > ????? (nek5000-users at lists.mcs.anl.gov) > > ?? 5. Re: Interpolation between two meshes > > ????? (nek5000-users at lists.mcs.anl.gov) > > > > > > ---------------------------------------------------------------------- > > > > Message: 1 > > Date: Mon, 27 Mar 2017 04:37:46 0000 > > From: nek5000-users at lists.mcs.anl.gov > > To: Nek5000 > > Subject: [Nek5000-users] Interpolation between two meshes > > Message-ID: > > ??????? > > Content-Type: text/plain; charset="iso-8859-1" > > > > Dear Neks, > > > > I have been using 'g2gi' to do interpolation between different meshes. Recently, I have noticed that when I interpolate between two big meshes (say 300000 elements in each mesh), the interpolation hangs at 'call findpts' and never moves on. I tried increasing > >? number of processors and changing 'lpart', but none of these worked. > > > > I'm wondering what could cause the interpolation to hang at 'findpts'. Has anyone encountered similar issue? > > > > Hope anyone could give me some advice. Thank you very much in advance. > > > > Best regards, > > Tony > > -------------- next part -------------- > > An HTML attachment was scrubbed... > > URL: < <>http://lists.mcs.anl.gov/pipermail/nek5000-users/attachments/20170327/b238e605/attachment-0001.html >> > > > > ------------------------------ > > > > Message: 2 > > Date: Mon, 27 Mar 2017 09:47:37 0200 > > From: nek5000-users at lists.mcs.anl.gov > > To: nek5000-users at lists.mcs.anl.gov????? > > Subject: Re: [Nek5000-users] Interpolation between two meshes > > Message-ID: > > ??????? > > Content-Type: text/plain; charset=utf-8 > > > > Please update to the latest master. Note, g2gi was replaced by gfldr. > > > > Stefan > > > > -----Original message----- > > > From:nek5000-users at lists.mcs.anl.gov > > > Sent: Monday 27th March 2017 6:38 > > > To: Nek5000 > > > Subject: [Nek5000-users] Interpolation between two meshes > > > > > > Dear Neks, > > > > > > I have been using 'g2gi' to do interpolation between different meshes. Recently, I have?noticed that when I interpolate between two big meshes (say 300000 elements in each mesh), the interpolation hangs at 'call findpts' and never moves on. I tried increasing > > >? number of processors and changing 'lpart', but none of these worked. > > > > > > I'm wondering what could cause the interpolation to hang at 'findpts'. Has anyone encountered similar issue? > > > > > > Hope anyone could give me some advice. Thank you very much in advance. > > > > > > Best regards, > > > Tony > > > _______________________________________________ > > > Nek5000-users mailing list > > > Nek5000-users at lists.mcs.anl.gov > > > > > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > > > > > ------------------------------ > > > > Message: 3 > > Date: Mon, 27 Mar 2017 16:47:00 0700 > > From: nek5000-users at lists.mcs.anl.gov > > To: nek5000-users at lists.mcs.anl.gov > > Subject: Re: [Nek5000-users] Copy velocity slice from one boundary to > > ??????? another > > Message-ID: > > ??????? > > Content-Type: text/plain; charset="utf-8" > > > > Thanks a lot for replying, your answer was very useful. > > > > I look on multimesh.f file. > > As i understood, i need set subroutine 'set_inflag' to look for 'P? ' bc. > > After this i need to call 'get_values(field)' subroutine, which interpolate > > and put the value in valint(ix,iy,iz,ie,ifld) array. > > And then this array will be available in userbc in .usr file, to set it on > > inflow boundary. > > > > c----------------------------------------------------------------------------------------------- > > > > Vatslav, > > you will have to use the neknek script that allows you to exchange data > > between two Nek5000 sessions that are run simultaneously. You should have a > > look at the neknek examples to understand how to set up your usr file. > > Some of the subroutines that will be useful to you are located in the > > following link: > > http://www.mcs.anl.gov/research/projects/nek5/docs/ > > > html/multimesh_8f_source.html > > You will have to modify some of them to fit your needs since for example > > the subroutine ?set_inflag? is written to look for ?in? boundary conditions > > and replace them with ?v? ?. You will need a subroutine that looks for ?in? > > and substitute it with either ?v? ? or ?P? ? depending on the which pipe > > you are at. > > Marco > > > > Hi, Neks! > > I have two pipes in my simulation. They are placed near each other on one > > axis with empty space between. > > One of them with periodic boundary conditions on z direction, another one - > > inflow -> outflow. > > How can I copy velocity slice from one of boundary on first pipe with > > periodic bc to the inflow boundary on second pipe? > > Regards, Vatslav > > > > c----------------------------------------------------------------------------------------------- > > > > Regards, Vatslav > > -------------- next part -------------- > > An HTML attachment was scrubbed... > > URL: < <>http://lists.mcs.anl.gov/pipermail/nek5000-users/attachments/20170327/92c78de8/attachment-0001.html >> > > > > ------------------------------ > > > > Message: 4 > > Date: Mon, 27 Mar 2017 11:31:53 0200 > > From: nek5000-users at lists.mcs.anl.gov > > To: nek5000-users at lists.mcs.anl.gov > > Subject: [Nek5000-users] Robin Boundary Condition -- Navier's Slip > > ??????? Length > > Message-ID: > > ??????? > > Content-Type: text/plain; charset="utf-8" > > > > Hi Neks, > > I wish to simulate a transitional channel flow whose wall respect a > > "slip-length" boundary condition, such as: > > > > $ [u? \delta \frac{\partial u}{\partial n}]_{wall}=0$ > > > > Where \delta is the slip length > > > > ^n > > |??????? u?????????????? u > > |????? |-->/???????? |----->/ > > |????? |?? /?????????? |????? / > > |????? |? /??????????? |???? / > > |????? | /???????????? |??? / > > |___|/_______|?? /_____ > > ?????????????????????? | /? ^ > > ?????????????????????? |/?? v \delta > > > > No-slip?????? Slip-length > > > > (a better sketch can be found here: > > http://www.nature.com/nmat/journal/v2/n4/fig_tab/nmat857_F1.html > > ) > > > >? > > > Figure 1 : Low-friction flows of liquid at nanopatterned ... >www.nature.com > > Nature Materials journal covers a range of topics within materials science, from materials engineering and structural materials (metals, alloys, ceramics, composites ... > > > > > > > > I would like to know if this Robin boundary condition for velocity field is > > already implemented in the current code. > > > > Thank you > > > > Ciccio > > -------------- next part -------------- > > An HTML attachment was scrubbed... > > URL: < <>http://lists.mcs.anl.gov/pipermail/nek5000-users/attachments/20170327/9922e2e7/attachment-0001.html >> > > > > ------------------------------ > > > > Message: 5 > > Date: Mon, 27 Mar 2017 13:56:02 0200 > > From: nek5000-users at lists.mcs.anl.gov > > To: nek5000-users at lists.mcs.anl.gov > > Subject: Re: [Nek5000-users] Interpolation between two meshes > > Message-ID: > > ??????? > > Content-Type: text/plain; charset="windows-1252"; Format="flowed" > > > > Hi Tony, > > I have encountered the same issue with g2gi when interpolating very > > large meshes. I don't know what is causing the issue but a workaround is > > to reduce the polynomial order. You obviously loose accuracy by doing > > this, but I still find it better than starting from scratch with the new > > mesh. Hope this helps. > > > > Best, > > Mattias > > > > > > On 03/27/2017 06:37 AM, nek5000-users at lists.mcs.anl.gov wrote: > > > Dear Neks, > > > > > > I have been using 'g2gi' to do interpolation between different meshes. > > > Recently, I have noticed that when I interpolate between two big > > > meshes (say 300000 elements in each mesh), the interpolation hangs at > > > 'call findpts' and never moves on. I tried increasing number of > > > processors and changing 'lpart', but none of these worked. > > > > > > I'm wondering what could cause the interpolation to hang at 'findpts'. > > > Has anyone encountered similar issue? > > > > > > Hope anyone could give me some advice. Thank you very much in advance. > > > > > > Best regards, > > > Tony > > > > > > > > > _______________________________________________ > > > 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: < <>http://lists.mcs.anl.gov/pipermail/nek5000-users/attachments/20170327/031d792f/attachment.html >> > > > > ------------------------------ > > > > _______________________________________________ > > Nek5000-users mailing list > > Nek5000-users at lists.mcs.anl.gov > > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > > > > > End of Nek5000-users Digest, Vol 97, Issue 27 > > ********************************************* > > _______________________________________________ > > 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 > > > End of Nek5000-users Digest, Vol 97, Issue 29 > ********************************************* > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users ------------------------------ Message: 2 Date: Tue, 28 Mar 2017 12:18:56 +0000 From: nek5000-users at lists.mcs.anl.gov To: "nek5000-users at lists.mcs.anl.gov" Subject: Re: [Nek5000-users] Copy velocity slice from one boundary to another Message-ID: Content-Type: text/plain; charset="us-ascii" Vatslav, what I do and it seems to work for my case is the following. Let assume you have two pipes (pipe 1 with periodic bc and pipe 2 with inlet/outlet), and that the flow is moving from pipe 1 to pipe 2. The solution from pipe 1 is interpolated to pipe 2 and used as inlet condition. In a separate subroutine, do the following: * in pipe 1, look for the boundary faces with P boundary condition that will be used for the interpolation and substitute P with inP. * in pipe 2, look for the boundary faces with v boundary condition and substitute v with inV. In a subroutine analogous to set_inflag: * in pipe 1, collect boundary faces with flag inP, set intflag to 1 for this boundary face, and substitute back boundary condition to P. * in pip2, do the same: inV - > v After, this step, you have marked all boundary faces that will be involved in the interpolation process in Nek5000. From this point, the steps are similar to what is done in the examples. All of this is done in my usr file. Hope this help, Marco On Mar 27, 2017, at 5:47 AM, nek5000-users at lists.mcs.anl.gov wrote: Thanks a lot for replying, your answer was very useful. I look on multimesh.f file. As i understood, i need set subroutine 'set_inflag' to look for 'P ' bc. After this i need to call 'get_values(field)' subroutine, which interpolate and put the value in valint(ix,iy,iz,ie,ifld) array. And then this array will be available in userbc in .usr file, to set it on inflow boundary. c----------------------------------------------------------------------------------------------- Vatslav, you will have to use the neknek script that allows you to exchange data between two Nek5000 sessions that are run simultaneously. You should have a look at the neknek examples to understand how to set up your usr file. Some of the subroutines that will be useful to you are located in the following link: http://www.mcs.anl.gov/research/projects/nek5/docs/html/multimesh_8f_source.html You will have to modify some of them to fit your needs since for example the subroutine ?set_inflag? is written to look for ?in? boundary conditions and replace them with ?v ?. You will need a subroutine that looks for ?in? and substitute it with either ?v ? or ?P ? depending on the which pipe you are at. Marco Hi, Neks! I have two pipes in my simulation. They are placed near each other on one axis with empty space between. One of them with periodic boundary conditions on z direction, another one - inflow -> outflow. How can I copy velocity slice from one of boundary on first pipe with periodic bc to the inflow boundary on second pipe? Regards, Vatslav c----------------------------------------------------------------------------------------------- Regards, Vatslav _______________________________________________ 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: ------------------------------ _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users End of Nek5000-users Digest, Vol 97, Issue 31 ********************************************* -------------- next part -------------- An HTML attachment was scrubbed... URL: -------------- next part -------------- A non-text attachment was scrubbed... Name: gfldr.f Type: text/x-fortran Size: 8871 bytes Desc: gfldr.f URL: -------------- next part -------------- A non-text attachment was scrubbed... Name: interp.usr Type: application/octet-stream Size: 4894 bytes Desc: interp.usr URL: -------------- next part -------------- A non-text attachment was scrubbed... Name: log.old Type: application/x-trash Size: 5822 bytes Desc: log.old URL: From nek5000-users at lists.mcs.anl.gov Tue Mar 28 15:46:36 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 28 Mar 2017 20:46:36 +0000 Subject: [Nek5000-users] Interpolation between two meshes In-Reply-To: References: Message-ID: Hi Stefan, In case the attachments didn't go through, please see below for the .usr file and log file. I only used 'userchk' and 'usrdat' in the .usr file for interpolation. The other subroutines are empty. (I added several print lines in 'gfldr.f' to see where the interpolation halted.) Best regards, Tony .USR FILE: c----------------------------------------------------------------------- subroutine userchk() include 'SIZE' include 'TOTAL' include 'ZPER' include 'CTIMER' include 'RESTART' character*132 sourcefld sourcefld='source.f00001' call gfldr(sourcefld) call outpost(vx,vy,vz,pr,t,'rst') call exitt() return end c----------------------------------------------------------------------- subroutine usrdat() ! This routine to modify element vertices include 'SIZE' include 'TOTAL' parameter (ielx=150) parameter (iely=22) parameter (ielz=142) integer i,e,eg,ex,ey,ez real cony cony = 2.36d0 do e=1,nelv eg = lglel(e) if(eg<=ielx*iely*ielz) then call get_exyz(ex,ey,ez,eg,ielx,iely,ielz) do i=1,8 if(i<=2 .or. i==5 .or. i==6) then if((yc(i,e)>0.0e0.and.yc(i,e)<1.0e0).OR. & (yc(i,e)>1.0e0.and.yc(i,e)<2.0e0)) then yc(i,e) = 2.0e0*Real(ey-1)/Real(iely) end if else if(i==3 .or. i==4 .or. i>=7) then if((yc(i,e)>0.0e0.and.yc(i,e)<1.0e0).OR. & (yc(i,e)>1.0e0.and.yc(i,e)<2.0e0)) then yc(i,e) = 2.0e0*Real(ey)/Real(iely) end if end if end do end if end do do e=1,nelv eg = lglel(e) if(eg==1) print*,yc(1,e),yc(2,e),yc(5,e),yc(6,e) if(eg==1) print*,yc(3,e),yc(4,e),yc(7,e),yc(8,e) do i=1,8 if(yc(i,e)>0.0e0 .AND. yc(i,e)<1.0e0) then yc(i,e) = yc(i,e)-1.0e0 yc(i,e) = tanh(cony*yc(i,e))/tanh(cony) yc(i,e) = yc(i,e)+1.0e0 else if(yc(i,e)>1.0e0 .AND. yc(i,e)<2.0e0) then yc(i,e) = yc(i,e)-1.0e0 yc(i,e) = tanh(cony*yc(i,e))/tanh(cony) yc(i,e) = yc(i,e)+1.0e0 end if end do end do return end c----------------------------------------------------------------------- LOG FILE: /----------------------------------------------------------\\ | _ __ ______ __ __ ______ ____ ____ ____ | | / | / // ____// //_/ / ____/ / __ \\/ __ \\/ __ \\ | | / |/ // __/ / ,< /___ \\ / / / // / / // / / / | | / /| // /___ / /| | ____/ / / /_/ // /_/ // /_/ / | | /_/ |_//_____//_/ |_|/_____/ \\___/ \\___/ \\___/ | | | |----------------------------------------------------------| | | | NEK5000: Open Source Spectral Element Solver | | COPYRIGHT (c) 2008-2017 UCHICAGO ARGONNE, LLC | | Version: 17.0.0 | | Web: http://nek5000.mcs.anl.gov | | | \\----------------------------------------------------------/ Number of processors: 720 REAL wdsize : 8 INTEGER wdsize : 4 Timer accuracy : 9.54E-08 Reading /work/e01/e01/tony/geometry_nonosci_cavity/interp.rea mapping elements to processors Reading /work/e01/e01/tony/geometry_nonosci_cavity/interp.map element load imbalance: 1 652 653 done :: mapping elements to processors 0 objects found 118 Parameters from file: 1 1.00000 p001 DENSITY 2 -3150.00 p002 VISCOS 12 -0.11750E-01 p012 DT 15 500.000 p015 IOSTEP 21 0.100000E-07 p021 DIVERGENCE 22 0.100000E-07 p022 HELMHOLTZ 26 2.00000 p026 COURANT/NTAU 27 3.00000 p027 TORDER 59 0.00000 p059 !=0 --> full Jac. eval. for each el. 63 8.00000 p063 =8 --> force 8-byte output 65 1.00000 p065 #iofiles (eg, 0 or 64); <0 --> sep. dirs 66 6.00000 p066 output : <0=ascii, else binary 67 6.00000 p067 restart: <0=ascii, else binary 93 20.0000 p093 Number of previous pressure solns saved 94 5.00000 p094 start projecting velocity after p94 step 95 5.00000 p095 start projecting pressure after p95 step 99 3.00000 p099 dealiasing: <0--> off/3--> old/4--> new 103 0.10000E-01 p103 weight of stabilizing filter (.01) nelgt/nelgv/lelt: 469500 469500 653 lx1 /lx2 /lx3 : 8 8 8 done :: read .rea file 45.222 sec setup mesh topology Right-handed check complete for 469500 elements. OK. setvert3d: 8 60855000 162267000 60855000 60855000 call usrsetvert done :: usrsetvert gs_setup: 10325502 unique labels shared pairwise times (avg, min, max): 0.00044986 0.00033021 0.000500798 crystal router : 0.00145524 0.00143301 0.0014781 used all_to_all method: pairwise handle bytes (avg, min, max): 2.64212e+06 2463020 2796252 buffer bytes (avg, min, max): 491593 352288 632640 setupds time 5.3504E-01 seconds 0 8 60855000 469500 8 max multiplicity done :: setup mesh topology 0.000000000000000E+000 0.000000000000000E+000 0.000000000000000E+000 0.000000000000000E+000 9.090909090909091E-002 9.090909090909091E-002 9.090909090909091E-002 9.090909090909091E-002 call usrdat done :: usrdat generate geometry data NOTE: All elements deformed , param(59) ^=0 done :: generate geometry data call usrdat2 done :: usrdat2 regenerate geometry data 1 NOTE: All elements deformed , param(59) ^=0 done :: regenerate geometry data 1 verify mesh topology 0.000000000000000E+000 6.00000000000000 Xrange -0.120000000000000 2.00000000000000 Yrange 0.000000000000000E+000 49.7000000000000 Zrange done :: verify mesh topology IFTRAN = T IFFLOW = T IFHEAT = F IFSPLIT = T IFLOMACH = F IFUSERVP = F IFUSERMV = F IFSTRS = F IFCHAR = T IFCYCLIC = F IFAXIS = F IFMVBD = F IFMELT = F IFMODEL = F IFKEPS = F IFMOAB = F IFNEKNEK = F IFSYNC = T IFVCOR = F IFINTQ = F IFCWUZ = F IFSWALL = F IFGEOM = F IFSURT = F IFWCNO = F IFTMSH for field 1 = F IFADVC for field 1 = T IFNONL for field 1 = F Dealiasing enabled, lxd= 12 verify mesh topology 0.000000000000000E+000 6.00000000000000 Xrange -0.120000000000000 2.00000000000000 Yrange 0.000000000000000E+000 49.7000000000000 Zrange done :: verify mesh topology call usrdat3 done :: usrdat3 set initial conditions nekuic (1) for ifld 1 call nekuic for vel xyz min 0.0000 -0.12000 0.0000 uvwpt min 0.0000 0.0000 0.0000 0.0000 0.0000 xyz max 6.0000 2.0000 49.700 uvwpt max 0.0000 0.0000 0.0000 0.0000 0.0000 done :: set initial conditions gridpoints unique/tot: 162267000 240384000 dofs: 159972750 162104250 Initialization successfully completed 46.588 sec nsteps=0 -> skip time loop running solver in post processing mode call userchk call gfldr byte swap: F 6.543210 -2.9312772E+35 sourcefld X 0.000000000000000E+000 6.00000000000000 sourcefld Y -0.120000000000000 2.00000000000000 sourcefld Z 0.000000000000000E+000 49.7000000000000 CHECK interp prepare CHECK interp read ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov on behalf of nek5000-users-request at lists.mcs.anl.gov Sent: 28 March 2017 20:51 To: nek5000-users at lists.mcs.anl.gov Subject: Nek5000-users Digest, Vol 97, Issue 33 Message: 3 Date: Tue, 28 Mar 2017 19:51:04 +0000 From: nek5000-users at lists.mcs.anl.gov To: "nek5000-users at lists.mcs.anl.gov" Subject: Re: [Nek5000-users] Interpolation between two meshes Message-ID: Content-Type: text/plain; charset="iso-8859-1" Hi Stefan, Many thanks for your reply. I'm running my simulations on ARCHER (Cray XC30 supercomputer) and I'm using the Intel compiler. The current simulation has 469500 elements with polynomial order of 7. The source field I used for interpolation has 383700 elements with the same polynomial order. The size of the source field is about 10GB. I'm not sure if it can be easily transferred. But I have attached my .usr and log files herewith (also the gfldr.f with few added checking lines). I ran the interpolation using 720 processors. Please have a look and let me know if you need further information about the case. Thank you very much for you help. Best regards, Tony -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Mar 28 15:59:18 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 28 Mar 2017 22:59:18 +0200 Subject: [Nek5000-users] Interpolation between two meshes Message-ID: We have tested glfdr() using different cases/machines and it worked fine. With the information below I cannot say what's going wrong. - Is your source fld in double precision? - Do have any additional information where it hangs or crashes? - Can you please test gfldr() say with turbChannel (NekExamples). Stefan -----Original message----- > From:nek5000-users at lists.mcs.anl.gov > Sent: Tuesday 28th March 2017 22:46 > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] Interpolation between two meshes > > Hi Stefan, > > In case the attachments didn't go through, please see below for the .usr file and log file. > I only used 'userchk' and 'usrdat' in the .usr file for interpolation. The other subroutines are empty. > (I added several print lines in 'gfldr.f' to see where the interpolation halted.) > > Best regards, > Tony > > .USR FILE: > c----------------------------------------------------------------------- > ????? subroutine userchk() > ????? include 'SIZE' > ????? include 'TOTAL' > ????? include 'ZPER' > ????? include 'CTIMER' > ????? include 'RESTART' > > ????? character*132 sourcefld > > ????? sourcefld='source.f00001' > ????? call gfldr(sourcefld) > ????? call outpost(vx,vy,vz,pr,t,'rst') > ????? call exitt() > > ????? return > ????? end > c----------------------------------------------------------------------- > ????? subroutine usrdat()?? ! This routine to modify element vertices > ????? include 'SIZE' > ????? include 'TOTAL' > > ????? parameter (ielx=150) > ????? parameter (iely=22) > ????? parameter (ielz=142) > ????? integer i,e,eg,ex,ey,ez > ????? real cony > > ????? cony = 2.36d0 > > ????? do e=1,nelv > ??????? eg = lglel(e) > ?????? if(eg<=ielx*iely*ielz) then > ??????? call get_exyz(ex,ey,ez,eg,ielx,iely,ielz) > > ??????? do i=1,8 > ???????? if(i<=2 .or. i==5 .or. i==6) then > ????????? if((yc(i,e)>0.0e0.and.yc(i,e)<1.0e0).OR. > ???? &????? (yc(i,e)>1.0e0.and.yc(i,e)<2.0e0)) then > ?????????? yc(i,e) = 2.0e0*Real(ey-1)/Real(iely) > ????????? end if > ???????? else if(i==3 .or. i==4 .or. i>=7) then > ????????? if((yc(i,e)>0.0e0.and.yc(i,e)<1.0e0).OR. > ???? &????? (yc(i,e)>1.0e0.and.yc(i,e)<2.0e0)) then > ?????????? yc(i,e) = 2.0e0*Real(ey)/Real(iely) > ????????? end if > ???????? end if > ??????? end do > > ?????? end if > ????? end do > > ????? do e=1,nelv > ??????? eg = lglel(e) > ??????? if(eg==1) print*,yc(1,e),yc(2,e),yc(5,e),yc(6,e) > ??????? if(eg==1) print*,yc(3,e),yc(4,e),yc(7,e),yc(8,e) > ??????? do i=1,8 > ???????? if(yc(i,e)>0.0e0 .AND. yc(i,e)<1.0e0) then > ?????????? yc(i,e) = yc(i,e)-1.0e0 > ?????????? yc(i,e) = tanh(cony*yc(i,e))/tanh(cony) > ?????????? yc(i,e) = yc(i,e)1.0e0 > ???????? else if(yc(i,e)>1.0e0 .AND. yc(i,e)<2.0e0) then > ?????????? yc(i,e) = yc(i,e)-1.0e0 > ?????????? yc(i,e) = tanh(cony*yc(i,e))/tanh(cony) > ?????????? yc(i,e) = yc(i,e)1.0e0 > ???????? end if > ??????? end do > ????? end do > > ????? return > ????? end > c----------------------------------------------------------------------- > > > LOG FILE: > > /----------------------------------------------------------\\ > |????? _?? __ ______ __ __? ______? ____?? ____?? ____???? | > |???? / | / // ____// //_/ / ____/ / __ \\/ __ \\/ __ \\?? | > |??? /? |/ // __/? / , |?? / /|? // /___ / /| | ____/ / / /_/ // /_/ // /_/ /???? | > |? /_/ |_//_____//_/ |_|/_____/? \\___/ \\___/ \\___/????? | > |????????????????????????????????????????????????????????? | > |----------------------------------------------------------| > |????????????????????????????????????????????????????????? | > | NEK5000:? Open Source Spectral Element Solver??????????? | > | COPYRIGHT (c) 2008-2017 UCHICAGO ARGONNE, LLC??????????? | > | Version:? 17.0.0???????????????????????????????????????? | > | Web:????? http://nek5000.mcs.anl.gov???????????????????? | > |????????????????????????????????????????????????????????? | > \\----------------------------------------------------------/ > > > ?Number of processors:???????? 720 > ?REAL??? wdsize????? :?????????? 8 > ?INTEGER wdsize????? :?????????? 4 > ?Timer accuracy????? : 9.54E-08 > ?Reading /work/e01/e01/tony/geometry_nonosci_cavity/interp.rea > > ?mapping elements to processors > ?Reading /work/e01/e01/tony/geometry_nonosci_cavity/interp.map > ?element load imbalance:??????????? 1???????? 652???????? 653 > ?done :: mapping elements to processors > > ?????????? 0? objects found > ?118?? Parameters from file: > ?? 1????? 1.00000???? p001 DENSITY > ?? 2???? -3150.00???? p002 VISCOS > ? 12???? -0.11750E-01 p012 DT > ? 15????? 500.000???? p015 IOSTEP > ? 21???? 0.100000E-07 p021 DIVERGENCE > ? 22???? 0.100000E-07 p022 HELMHOLTZ > ? 26????? 2.00000???? p026 COURANT/NTAU > ? 27????? 3.00000???? p027 TORDER > ? 59????? 0.00000???? p059 !=0 --> full Jac. eval. for each el. > ? 63????? 8.00000???? p063 =8 --> force 8-byte output > ? 65????? 1.00000???? p065 #iofiles (eg, 0 or 64); <0 --> sep. dirs > ? 66????? 6.00000???? p066 output : <0=ascii, else binary > ? 67????? 6.00000???? p067 restart: <0=ascii, else binary > ? 93????? 20.0000???? p093 Number of previous pressure solns saved > ? 94????? 5.00000???? p094 start projecting velocity after p94 step > ? 95????? 5.00000???? p095 start projecting pressure after p95 step > ? 99????? 3.00000???? p099 dealiasing: <0--> off/3--> old/4--> new > ?103????? 0.10000E-01 p103 weight of stabilizing filter (.01) > > ?nelgt/nelgv/lelt:????? 469500????? 469500???????? 653 > ?lx1? /lx2? /lx3 :?????????? 8?????????? 8?????????? 8 > ?done :: read .rea file??? 45.222???? sec > > ?setup mesh topology > ?? Right-handed check complete for? 469500 elements. OK. > ?? setvert3d:?? 8??? 60855000?? 162267000??? 60855000??? 60855000 > ?call usrsetvert > ?done :: usrsetvert > > gs_setup: 10325502 unique labels shared > ?? pairwise times (avg, min, max): 0.00044986 0.00033021 0.000500798 > ?? crystal router??????????????? : 0.00145524 0.00143301 0.0014781 > ?? used all_to_all method: pairwise > ?? handle bytes (avg, min, max): 2.64212e06 2463020 2796252 > ?? buffer bytes (avg, min, max): 491593 352288 632640 > ?? setupds time 5.3504E-01 seconds?? 0? 8??? 60855000????? 469500 > ?????????? 8? max multiplicity > ?done :: setup mesh topology > > ? 0.000000000000000E000? 0.000000000000000E000? 0.000000000000000E000 > ? 0.000000000000000E000 > ? 9.090909090909091E-002? 9.090909090909091E-002? 9.090909090909091E-002 > ? 9.090909090909091E-002 > ?call usrdat > ?done :: usrdat > > ?generate geometry data > ?NOTE: All elements deformed , param(59) ^=0 > ?done :: generate geometry data > > ?call usrdat2 > ?done :: usrdat2 > > ?regenerate geometry data?????????? 1 > ?NOTE: All elements deformed , param(59) ^=0 > ?done :: regenerate geometry data?????????? 1 > > ?verify mesh topology > ? 0.000000000000000E000?? 6.00000000000000?????? Xrange > ?-0.120000000000000??????? 2.00000000000000?????? Yrange > ? 0.000000000000000E000?? 49.7000000000000?????? Zrange > ?done :: verify mesh topology > > ?IFTRAN?? = T > ?IFFLOW?? = T > ?IFHEAT?? = F > ?IFSPLIT? = T > ?IFLOMACH = F > ?IFUSERVP = F > ?IFUSERMV = F > ?IFSTRS?? = F > ?IFCHAR?? = T > ?IFCYCLIC = F > ?IFAXIS?? = F > ?IFMVBD?? = F > ?IFMELT?? = F > ?IFMODEL? = F > ?IFKEPS?? = F > ?IFMOAB?? = F > ?IFNEKNEK = F > ?IFSYNC?? = T > > ?IFVCOR?? = F > ?IFINTQ?? = F > ?IFCWUZ?? = F > ?IFSWALL? = F > ?IFGEOM?? = F > ?IFSURT?? = F > ?IFWCNO?? = F > > ?IFTMSH for field?????????? 1??? =? F > ?IFADVC for field?????????? 1??? =? T > ?IFNONL for field?????????? 1??? =? F > > ?Dealiasing enabled, lxd=????????? 12 > ?verify mesh topology > ? 0.000000000000000E000?? 6.00000000000000?????? Xrange > ?-0.120000000000000??????? 2.00000000000000?????? Yrange > ? 0.000000000000000E000?? 49.7000000000000?????? Zrange > ?done :: verify mesh topology > > ?call usrdat3 > ?done :: usrdat3 > > ?set initial conditions > ?nekuic (1) for ifld??????????? 1 > ?call nekuic for vel > ?xyz min???? 0.0000???? -0.12000?????? 0.0000 > ?uvwpt min?? 0.0000?????? 0.0000?????? 0.0000?????? 0.0000?????? 0.0000 > ?xyz max???? 6.0000?????? 2.0000?????? 49.700 > ?uvwpt max?? 0.0000?????? 0.0000?????? 0.0000?????? 0.0000?????? 0.0000 > ?done :: set initial conditions > > gridpoints unique/tot:???? 162267000??? 240384000 > ? dofs:???????????? 159972750???????????? 162104250 > > ?Initialization successfully completed??? 46.588???? sec > > ?nsteps=0 -> skip time loop > ?running solver in post processing mode > > ?call userchk > ?call gfldr > ?byte swap: F?? 6.543210???? -2.9312772E35 > ?sourcefld X? 0.000000000000000E000?? 6.00000000000000 > ?sourcefld Y -0.120000000000000??????? 2.00000000000000 > ?sourcefld Z? 0.000000000000000E000?? 49.7000000000000 > ?CHECK interp prepare > ?CHECK interp read > > ----------- > From: nek5000-users-bounces at lists.mcs.anl.gov on behalf of nek5000-users-request at lists.mcs.anl.gov > Sent: 28 March 2017 20:51 > To: nek5000-users at lists.mcs.anl.gov > Subject: Nek5000-users Digest, Vol 97, Issue 33 > > Message: 3 > Date: Tue, 28 Mar 2017 19:51:04 0000 > From: nek5000-users at lists.mcs.anl.gov > To: "nek5000-users at lists.mcs.anl.gov" > ??????? > Subject: Re: [Nek5000-users] Interpolation between two meshes > Message-ID: > ??????? > Content-Type: text/plain; charset="iso-8859-1" > > Hi Stefan, > > > Many thanks for your reply. I'm running my simulations on ARCHER (Cray XC30 supercomputer) and I'm using the Intel compiler. > > > The current simulation has 469500 elements with polynomial order of 7. The source field I used for interpolation has 383700 elements with the same polynomial order. The size of the source field is about 10GB. I'm not sure if it can be easily transferred. But > I have attached my .usr and log files herewith (also the gfldr.f with few added checking lines). I ran the interpolation using 720 processors. > > > Please have a look and let me know if you need further information about the case. Thank you very much for you help. > > > Best regards, > > Tony > _______________________________________________ > 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 Mar 28 16:14:56 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 28 Mar 2017 23:14:56 +0200 Subject: [Nek5000-users] Interpolation between two meshes Message-ID: Can you also call nekgsync() before and after findpts. Just trying to understand if it really hangs there. -----Original message----- > From:nek5000-users at lists.mcs.anl.gov > Sent: Tuesday 28th March 2017 22:59 > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] Interpolation between two meshes > > We have tested glfdr() using different cases/machines and it worked fine. With the information below I cannot say what's going wrong. > > - Is your source fld in double precision? > - Do have any additional information where it hangs or crashes? > - Can you please test gfldr() say with turbChannel (NekExamples). > > Stefan > > -----Original message----- > > From:nek5000-users at lists.mcs.anl.gov > > Sent: Tuesday 28th March 2017 22:46 > > To: nek5000-users at lists.mcs.anl.gov > > Subject: Re: [Nek5000-users] Interpolation between two meshes > > > > Hi Stefan, > > > > In case the attachments didn't go through, please see below for the .usr file and log file. > > I only used 'userchk' and 'usrdat' in the .usr file for interpolation. The other subroutines are empty. > > (I added several print lines in 'gfldr.f' to see where the interpolation halted.) > > > > Best regards, > > Tony > > > > .USR FILE: > > c----------------------------------------------------------------------- > > ????? subroutine userchk() > > ????? include 'SIZE' > > ????? include 'TOTAL' > > ????? include 'ZPER' > > ????? include 'CTIMER' > > ????? include 'RESTART' > > > > ????? character*132 sourcefld > > > > ????? sourcefld='source.f00001' > > ????? call gfldr(sourcefld) > > ????? call outpost(vx,vy,vz,pr,t,'rst') > > ????? call exitt() > > > > ????? return > > ????? end > > c----------------------------------------------------------------------- > > ????? subroutine usrdat()?? ! This routine to modify element vertices > > ????? include 'SIZE' > > ????? include 'TOTAL' > > > > ????? parameter (ielx=150) > > ????? parameter (iely=22) > > ????? parameter (ielz=142) > > ????? integer i,e,eg,ex,ey,ez > > ????? real cony > > > > ????? cony = 2.36d0 > > > > ????? do e=1,nelv > > ??????? eg = lglel(e) > > ?????? if(eg<=ielx*iely*ielz) then > > ??????? call get_exyz(ex,ey,ez,eg,ielx,iely,ielz) > > > > ??????? do i=1,8 > > ???????? if(i<=2 .or. i==5 .or. i==6) then > > ????????? if((yc(i,e)>0.0e0.and.yc(i,e)<1.0e0).OR. > > ???? &????? (yc(i,e)>1.0e0.and.yc(i,e)<2.0e0)) then > > ?????????? yc(i,e) = 2.0e0*Real(ey-1)/Real(iely) > > ????????? end if > > ???????? else if(i==3 .or. i==4 .or. i>=7) then > > ????????? if((yc(i,e)>0.0e0.and.yc(i,e)<1.0e0).OR. > > ???? &????? (yc(i,e)>1.0e0.and.yc(i,e)<2.0e0)) then > > ?????????? yc(i,e) = 2.0e0*Real(ey)/Real(iely) > > ????????? end if > > ???????? end if > > ??????? end do > > > > ?????? end if > > ????? end do > > > > ????? do e=1,nelv > > ??????? eg = lglel(e) > > ??????? if(eg==1) print*,yc(1,e),yc(2,e),yc(5,e),yc(6,e) > > ??????? if(eg==1) print*,yc(3,e),yc(4,e),yc(7,e),yc(8,e) > > ??????? do i=1,8 > > ???????? if(yc(i,e)>0.0e0 .AND. yc(i,e)<1.0e0) then > > ?????????? yc(i,e) = yc(i,e)-1.0e0 > > ?????????? yc(i,e) = tanh(cony*yc(i,e))/tanh(cony) > > ?????????? yc(i,e) = yc(i,e)1.0e0 > > ???????? else if(yc(i,e)>1.0e0 .AND. yc(i,e)<2.0e0) then > > ?????????? yc(i,e) = yc(i,e)-1.0e0 > > ?????????? yc(i,e) = tanh(cony*yc(i,e))/tanh(cony) > > ?????????? yc(i,e) = yc(i,e)1.0e0 > > ???????? end if > > ??????? end do > > ????? end do > > > > ????? return > > ????? end > > c----------------------------------------------------------------------- > > > > > > LOG FILE: > > > > /----------------------------------------------------------\\ > > |????? _?? __ ______ __ __? ______? ____?? ____?? ____???? | > > |???? / | / // ____// //_/ / ____/ / __ \\/ __ \\/ __ \\?? | > > |??? /? |/ // __/? / , > |?? / /|? // /___ / /| | ____/ / / /_/ // /_/ // /_/ /???? | > > |? /_/ |_//_____//_/ |_|/_____/? \\___/ \\___/ \\___/????? | > > |????????????????????????????????????????????????????????? | > > |----------------------------------------------------------| > > |????????????????????????????????????????????????????????? | > > | NEK5000:? Open Source Spectral Element Solver??????????? | > > | COPYRIGHT (c) 2008-2017 UCHICAGO ARGONNE, LLC??????????? | > > | Version:? 17.0.0???????????????????????????????????????? | > > | Web:????? http://nek5000.mcs.anl.gov???????????????????? | > > |????????????????????????????????????????????????????????? | > > \\----------------------------------------------------------/ > > > > > > ?Number of processors:???????? 720 > > ?REAL??? wdsize????? :?????????? 8 > > ?INTEGER wdsize????? :?????????? 4 > > ?Timer accuracy????? : 9.54E-08 > > ?Reading /work/e01/e01/tony/geometry_nonosci_cavity/interp.rea > > > > ?mapping elements to processors > > ?Reading /work/e01/e01/tony/geometry_nonosci_cavity/interp.map > > ?element load imbalance:??????????? 1???????? 652???????? 653 > > ?done :: mapping elements to processors > > > > ?????????? 0? objects found > > ?118?? Parameters from file: > > ?? 1????? 1.00000???? p001 DENSITY > > ?? 2???? -3150.00???? p002 VISCOS > > ? 12???? -0.11750E-01 p012 DT > > ? 15????? 500.000???? p015 IOSTEP > > ? 21???? 0.100000E-07 p021 DIVERGENCE > > ? 22???? 0.100000E-07 p022 HELMHOLTZ > > ? 26????? 2.00000???? p026 COURANT/NTAU > > ? 27????? 3.00000???? p027 TORDER > > ? 59????? 0.00000???? p059 !=0 --> full Jac. eval. for each el. > > ? 63????? 8.00000???? p063 =8 --> force 8-byte output > > ? 65????? 1.00000???? p065 #iofiles (eg, 0 or 64); <0 --> sep. dirs > > ? 66????? 6.00000???? p066 output : <0=ascii, else binary > > ? 67????? 6.00000???? p067 restart: <0=ascii, else binary > > ? 93????? 20.0000???? p093 Number of previous pressure solns saved > > ? 94????? 5.00000???? p094 start projecting velocity after p94 step > > ? 95????? 5.00000???? p095 start projecting pressure after p95 step > > ? 99????? 3.00000???? p099 dealiasing: <0--> off/3--> old/4--> new > > ?103????? 0.10000E-01 p103 weight of stabilizing filter (.01) > > > > ?nelgt/nelgv/lelt:????? 469500????? 469500???????? 653 > > ?lx1? /lx2? /lx3 :?????????? 8?????????? 8?????????? 8 > > ?done :: read .rea file??? 45.222???? sec > > > > ?setup mesh topology > > ?? Right-handed check complete for? 469500 elements. OK. > > ?? setvert3d:?? 8??? 60855000?? 162267000??? 60855000??? 60855000 > > ?call usrsetvert > > ?done :: usrsetvert > > > > gs_setup: 10325502 unique labels shared > > ?? pairwise times (avg, min, max): 0.00044986 0.00033021 0.000500798 > > ?? crystal router??????????????? : 0.00145524 0.00143301 0.0014781 > > ?? used all_to_all method: pairwise > > ?? handle bytes (avg, min, max): 2.64212e06 2463020 2796252 > > ?? buffer bytes (avg, min, max): 491593 352288 632640 > > ?? setupds time 5.3504E-01 seconds?? 0? 8??? 60855000????? 469500 > > ?????????? 8? max multiplicity > > ?done :: setup mesh topology > > > > ? 0.000000000000000E000? 0.000000000000000E000? 0.000000000000000E000 > > ? 0.000000000000000E000 > > ? 9.090909090909091E-002? 9.090909090909091E-002? 9.090909090909091E-002 > > ? 9.090909090909091E-002 > > ?call usrdat > > ?done :: usrdat > > > > ?generate geometry data > > ?NOTE: All elements deformed , param(59) ^=0 > > ?done :: generate geometry data > > > > ?call usrdat2 > > ?done :: usrdat2 > > > > ?regenerate geometry data?????????? 1 > > ?NOTE: All elements deformed , param(59) ^=0 > > ?done :: regenerate geometry data?????????? 1 > > > > ?verify mesh topology > > ? 0.000000000000000E000?? 6.00000000000000?????? Xrange > > ?-0.120000000000000??????? 2.00000000000000?????? Yrange > > ? 0.000000000000000E000?? 49.7000000000000?????? Zrange > > ?done :: verify mesh topology > > > > ?IFTRAN?? = T > > ?IFFLOW?? = T > > ?IFHEAT?? = F > > ?IFSPLIT? = T > > ?IFLOMACH = F > > ?IFUSERVP = F > > ?IFUSERMV = F > > ?IFSTRS?? = F > > ?IFCHAR?? = T > > ?IFCYCLIC = F > > ?IFAXIS?? = F > > ?IFMVBD?? = F > > ?IFMELT?? = F > > ?IFMODEL? = F > > ?IFKEPS?? = F > > ?IFMOAB?? = F > > ?IFNEKNEK = F > > ?IFSYNC?? = T > > > > ?IFVCOR?? = F > > ?IFINTQ?? = F > > ?IFCWUZ?? = F > > ?IFSWALL? = F > > ?IFGEOM?? = F > > ?IFSURT?? = F > > ?IFWCNO?? = F > > > > ?IFTMSH for field?????????? 1??? =? F > > ?IFADVC for field?????????? 1??? =? T > > ?IFNONL for field?????????? 1??? =? F > > > > ?Dealiasing enabled, lxd=????????? 12 > > ?verify mesh topology > > ? 0.000000000000000E000?? 6.00000000000000?????? Xrange > > ?-0.120000000000000??????? 2.00000000000000?????? Yrange > > ? 0.000000000000000E000?? 49.7000000000000?????? Zrange > > ?done :: verify mesh topology > > > > ?call usrdat3 > > ?done :: usrdat3 > > > > ?set initial conditions > > ?nekuic (1) for ifld??????????? 1 > > ?call nekuic for vel > > ?xyz min???? 0.0000???? -0.12000?????? 0.0000 > > ?uvwpt min?? 0.0000?????? 0.0000?????? 0.0000?????? 0.0000?????? 0.0000 > > ?xyz max???? 6.0000?????? 2.0000?????? 49.700 > > ?uvwpt max?? 0.0000?????? 0.0000?????? 0.0000?????? 0.0000?????? 0.0000 > > ?done :: set initial conditions > > > > gridpoints unique/tot:???? 162267000??? 240384000 > > ? dofs:???????????? 159972750???????????? 162104250 > > > > ?Initialization successfully completed??? 46.588???? sec > > > > ?nsteps=0 -> skip time loop > > ?running solver in post processing mode > > > > ?call userchk > > ?call gfldr > > ?byte swap: F?? 6.543210???? -2.9312772E35 > > ?sourcefld X? 0.000000000000000E000?? 6.00000000000000 > > ?sourcefld Y -0.120000000000000??????? 2.00000000000000 > > ?sourcefld Z? 0.000000000000000E000?? 49.7000000000000 > > ?CHECK interp prepare > > ?CHECK interp read > > > > ----------- > > From: nek5000-users-bounces at lists.mcs.anl.gov on behalf of nek5000-users-request at lists.mcs.anl.gov > > Sent: 28 March 2017 20:51 > > To: nek5000-users at lists.mcs.anl.gov > > Subject: Nek5000-users Digest, Vol 97, Issue 33 > > > > Message: 3 > > Date: Tue, 28 Mar 2017 19:51:04 0000 > > From: nek5000-users at lists.mcs.anl.gov > > To: "nek5000-users at lists.mcs.anl.gov" > > ??????? > > Subject: Re: [Nek5000-users] Interpolation between two meshes > > Message-ID: > > ??????? > > Content-Type: text/plain; charset="iso-8859-1" > > > > Hi Stefan, > > > > > > Many thanks for your reply. I'm running my simulations on ARCHER (Cray XC30 supercomputer) and I'm using the Intel compiler. > > > > > > The current simulation has 469500 elements with polynomial order of 7. The source field I used for interpolation has 383700 elements with the same polynomial order. The size of the source field is about 10GB. I'm not sure if it can be easily transferred. But > > I have attached my .usr and log files herewith (also the gfldr.f with few added checking lines). I ran the interpolation using 720 processors. > > > > > > Please have a look and let me know if you need further information about the case. Thank you very much for you help. > > > > > > Best regards, > > > > Tony > > _______________________________________________ > > Nek5000-users mailing list > > Nek5000-users at lists.mcs.anl.gov > > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > From nek5000-users at lists.mcs.anl.gov Wed Mar 29 06:10:34 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 29 Mar 2017 13:10:34 +0200 Subject: [Nek5000-users] NekNek with PN-PN Message-ID: Dear Nek users, I am coupling Navier-Stokes and Darcy equations using NekNek. I need to pass pressure from Navier-Stokes as the boundary condition for Darcy equation. Pn/Pn-2 formulations extrapolate pressure to GLL nodes and apply dsavg to compute C-0 continuous pressure field. Though the resulting pressure field is continuous it is not very smooth and exhibits oscillations near each element boundaries. Using this as the boundary condition for Darcy equation gives raise to convergence issues after some time steps. I tried to use neknek with Pn/Pn formulation which will avoid this problem. However, I endup with "ERROR: .... crs_solve: invalid handle" and the simulation breaks away after the first time step in "happy_check" subroutine. Is Neknek not implemented for Pn/Pn formulations? Thank you very much for your response, Best regards, Sudhakar Linne FLOW centre. From nek5000-users at lists.mcs.anl.gov Wed Mar 29 07:58:25 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 29 Mar 2017 12:58:25 +0000 Subject: [Nek5000-users] Interpolation between two meshes In-Reply-To: References: Message-ID: Hi Stefan, Thank you very much for your quick reply. 1. Yes, my source field is in double precision since I need to keep the accuracy. 2. I added several print lines in gfldr.f to check where the interpolation hangs (see below). I also put 'call nekgsync()' before and after findpts as you suggested. I can confirm that findpts is exactly where the interpolation hangs. The last output in the logfile is 'CHECK interp findpts before' and it never gets updated again. 3. I've just tested gfldr() with turbChannel example. Everything worked fine and the source field was interpolated onto the turbChannel mesh (512 elements). So I moved on increasing the number of elements of turbChannel case. First, I used 234300 elements in the turbChannel example (half of my current simulation size) and the interpolation was done successfully. Then, I used 468600 elements for the turbChannel example (similar to my current simulation size), the interpolation hangs again at findpts. I guess it might be something to do with the memory. What do you think? Is there any solution to this? Best regards, Tony if(nid==0) print*,'CHECK interp findpts before' call nekgsync() call findpts(inth_gfldr, & rcode,1, & proc,1, & elid,1, & rst,ndim, & dist,1, & xm1,1, & ym1,1, & zm1,1,ntot) call nekgsync() if(nid==0) print*,'CHECK interp findpts after' ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov on behalf of nek5000-users-request at lists.mcs.anl.gov Sent: 28 March 2017 22:15 To: nek5000-users at lists.mcs.anl.gov Subject: Nek5000-users Digest, Vol 97, Issue 35 Today's Topics: 1. Re: Interpolation between two meshes (nek5000-users at lists.mcs.anl.gov) 2. Re: Interpolation between two meshes (nek5000-users at lists.mcs.anl.gov) Message: 2 Date: Tue, 28 Mar 2017 23:14:56 +0200 From: nek5000-users at lists.mcs.anl.gov To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Interpolation between two meshes Message-ID: Content-Type: text/plain; charset=utf-8 Can you also call nekgsync() before and after findpts. Just trying to understand if it really hangs there. -----Original message----- > From:nek5000-users at lists.mcs.anl.gov > Sent: Tuesday 28th March 2017 22:59 > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] Interpolation between two meshes > > We have tested glfdr() using different cases/machines and it worked fine. With the information below I cannot say what's going wrong. > > - Is your source fld in double precision? > - Do have any additional information where it hangs or crashes? > - Can you please test gfldr() say with turbChannel (NekExamples). > > Stefan -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Mar 29 12:32:52 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 29 Mar 2017 19:32:52 +0200 Subject: [Nek5000-users] Outflow BC with negative velocity Message-ID: Dear all, I've been having some trouble with the outflow BCs in an axisymmetric case with periodic velocity inflow conditions. Inflow velocity takes these values: ux=(sqrt(2.)/5.)*sin(2.*pi*0.03*time) It runs fine at Re=1000, but when set to Re=13329, which is the value I'm interested in testing, it crashes due to backflow near the boundary (with outflow BC). Is there any setting that allows the outflow to handle flow in both ways? I have already tried turb_outflow (trying to eliminate the negative flow), but it's not working properly with the axisymmetric condition. Thanks in advance for the help, MViturro From nek5000-users at lists.mcs.anl.gov Wed Mar 29 18:37:59 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 29 Mar 2017 16:37:59 -0700 Subject: [Nek5000-users] NekNek with PN-PN In-Reply-To: References: Message-ID: That?s correct. Neknek is not currently implemented with Pn/Pn formulation. However, there are some ways around it if you use outflow boundary conditions instead of interpolation at the outflow boundaries. I am not sure if this example is in repo, but it should be doable, if this is what you need. Yulia On Mar 29, 2017, at 4:10 AM, nek5000-users at lists.mcs.anl.gov wrote: > Dear Nek users, > > I am coupling Navier-Stokes and Darcy equations using NekNek. I need to pass pressure from Navier-Stokes as the boundary condition for Darcy equation. Pn/Pn-2 formulations extrapolate pressure to GLL nodes and apply dsavg to compute C-0 continuous pressure field. Though the resulting pressure field is continuous it is not very smooth and exhibits oscillations near each element boundaries. Using this as the boundary condition for Darcy equation gives raise to convergence issues after some time steps. I tried to use neknek with Pn/Pn formulation which will avoid this problem. However, I endup with "ERROR: .... crs_solve: invalid handle" and the simulation breaks away after the first time step in "happy_check" subroutine. > > Is Neknek not implemented for Pn/Pn formulations? > > Thank you very much for your response, > > Best regards, > Sudhakar > Linne FLOW centre. > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Wed Mar 29 17:35:16 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 29 Mar 2017 22:35:16 +0000 Subject: [Nek5000-users] NekNek with PN-PN In-Reply-To: References: , Message-ID: We have used neknek + pn/pn in the past. Also, coupling the pressure is possible with both... we've done that also. Unfortunately, I'm totally tied up till mid-week next week so cannot look at this until then. 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, March 29, 2017 6:37 PM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] NekNek with PN-PN That?s correct. Neknek is not currently implemented with Pn/Pn formulation. However, there are some ways around it if you use outflow boundary conditions instead of interpolation at the outflow boundaries. I am not sure if this example is in repo, but it should be doable, if this is what you need. Yulia On Mar 29, 2017, at 4:10 AM, nek5000-users at lists.mcs.anl.gov wrote: > Dear Nek users, > > I am coupling Navier-Stokes and Darcy equations using NekNek. I need to pass pressure from Navier-Stokes as the boundary condition for Darcy equation. Pn/Pn-2 formulations extrapolate pressure to GLL nodes and apply dsavg to compute C-0 continuous pressure field. Though the resulting pressure field is continuous it is not very smooth and exhibits oscillations near each element boundaries. Using this as the boundary condition for Darcy equation gives raise to convergence issues after some time steps. I tried to use neknek with Pn/Pn formulation which will avoid this problem. However, I endup with "ERROR: .... crs_solve: invalid handle" and the simulation breaks away after the first time step in "happy_check" subroutine. > > Is Neknek not implemented for Pn/Pn formulations? > > Thank you very much for your response, > > Best regards, > Sudhakar > Linne FLOW centre. > _______________________________________________ > 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 Mar 30 04:46:40 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 30 Mar 2017 11:46:40 +0200 Subject: [Nek5000-users] Interpolation between two meshes In-Reply-To: References: Message-ID: Please let me know how I can contact you off list. Stefan? On 29 Mar 2017, at 14:59, "nek5000-users at lists.mcs.anl.gov " > wrote: Hi Stefan, Thank you very much for your quick reply. 1. Yes, my source field is in double precision since I need to keep the accuracy. 2. I added several print lines in gfldr.f to check where the interpolation hangs (see below). I also put 'call nekgsync()' before and after findpts as you suggested. I can confirm that findpts is exactly where the interpolation hangs. The last output in the logfile is 'CHECK interp findpts before' and it never gets updated again. 3. I've just tested gfldr() with turbChannel example. Everything worked fine and the?source field was interpolated onto the turbChannel mesh (512 elements). So I moved on increasing the number of elements of turbChannel case. First, I used 234300 elements?in the turbChannel example (half of my current simulation size) and the interpolation was done successfully. Then, I used 468600 elements for?the turbChannel example (similar to my current simulation size), the interpolation hangs again at findpts. I guess it might be something to do with the memory. What do you think? Is there any solution to this? Best regards, Tony ??????? if(nid==0) print*,'CHECK interp findpts before' ??????? call nekgsync() ??????? call findpts(inth_gfldr, ???? &?????????????? rcode,1, ???? &?????????????? proc,1, ???? &?????????????? elid,1, ???? &?????????????? rst,ndim, ???? &?????????????? dist,1, ???? &?????????????? xm1,1, ???? &?????????????? ym1,1, ???? &?????????????? zm1,1,ntot) ??????? call nekgsync() ??????? if(nid==0) print*,'CHECK interp findpts after' -------------------------------- From: nek5000-users-bounces at lists.mcs.anl.gov > on behalf of nek5000-users-request at lists.mcs.anl.gov > Sent: 28 March 2017 22:15 To: nek5000-users at lists.mcs.anl.gov Subject: Nek5000-users Digest, Vol 97, Issue 35 ? Today's Topics: ?? 1. Re: Interpolation between two meshes ????? (nek5000-users at lists.mcs.anl.gov ) ?? 2. Re: Interpolation between two meshes ????? (nek5000-users at lists.mcs.anl.gov ) Message: 2 Date: Tue, 28 Mar 2017 23:14:56 +0200 From: nek5000-users at lists.mcs.anl.gov To: nek5000-users at lists.mcs.anl.gov ????? > Subject: Re: [Nek5000-users] Interpolation between two meshes Message-ID: ??????? > Content-Type: text/plain; charset=utf-8 Can you also call nekgsync() before and after findpts. Just trying to understand if it really hangs there. ? -----Original message----- > From:nek5000-users at lists.mcs.anl.gov > > Sent: Tuesday 28th March 2017 22:59 > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] Interpolation between two meshes > > We have tested glfdr() using different cases/machines and it worked fine. With the information below I cannot say what's going wrong. > > - Is your source fld in double precision? > - Do have any additional information where it hangs or crashes? > - Can you please test gfldr() say with turbChannel (NekExamples). > > Stefan _______________________________________________ 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 Mar 30 03:33:02 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 30 Mar 2017 10:33:02 +0200 Subject: [Nek5000-users] Accessing the value of drag and lift coefficients in usrchk Message-ID: Hi Nek, I was wondering whether it was possible to access the values of the drag and lift coefficient directly into usrchk? I know how to compute them but they only get printed in the logfile. I would need them for a control problem. Thanks a lot Jean-Christophe B. Loiseau Ma?tre de conf?rence DynFluid, Arts et M?tiers ParisTech Homepage -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Mar 30 04:16:14 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 30 Mar 2017 11:16:14 +0200 Subject: [Nek5000-users] NekNek with PN-PN In-Reply-To: References: Message-ID: Dear Paul and Yulia, Thank you very much for your responses. Regarding you comments, 1. I do not have any outflow boundary conditions in my simulations. 2. Coupling pressure in Pn/Pn-2 works fine for laminar flows, but once I get into the turbulent regime, the extrapolation used to map pressure to GLL points causes some trouble. I pass pressure from domain-1 to domain-2, and works on the gradient of pressure in domain-2. I see clearly the oscillations of pressure gradient at the element boundaries. (please see the attachment) Could you please give hints on how can I run neknek with PN/PN? Thanks once again, Best regards, Sudhakar On 03/30/2017 01:37 AM, nek5000-users at lists.mcs.anl.gov wrote: > That?s correct. Neknek is not currently implemented with Pn/Pn formulation. However, there are some ways around it if you use outflow boundary conditions instead of interpolation at the outflow boundaries. I am not sure if this example is in repo, but it should be doable, if this is what you need. > > Yulia > > > On Mar 29, 2017, at 4:10 AM, nek5000-users at lists.mcs.anl.gov wrote: > >> Dear Nek users, >> >> I am coupling Navier-Stokes and Darcy equations using NekNek. I need to pass pressure from Navier-Stokes as the boundary condition for Darcy equation. Pn/Pn-2 formulations extrapolate pressure to GLL nodes and apply dsavg to compute C-0 continuous pressure field. Though the resulting pressure field is continuous it is not very smooth and exhibits oscillations near each element boundaries. Using this as the boundary condition for Darcy equation gives raise to convergence issues after some time steps. I tried to use neknek with Pn/Pn formulation which will avoid this problem. However, I endup with "ERROR: .... crs_solve: invalid handle" and the simulation breaks away after the first time step in "happy_check" subroutine. >> >> Is Neknek not implemented for Pn/Pn formulations? >> >> Thank you very much for your response, >> >> Best regards, >> Sudhakar >> Linne FLOW centre. >> _______________________________________________ >> 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 -------------- A non-text attachment was scrubbed... Name: neknek-oscillation.pdf Type: application/pdf Size: 181847 bytes Desc: not available URL: From nek5000-users at lists.mcs.anl.gov Thu Mar 30 07:22:00 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 30 Mar 2017 12:22:00 +0000 Subject: [Nek5000-users] Accessing the value of drag and lift coefficients in usrchk In-Reply-To: References: Message-ID: Dear JC, Yes --- just pull a copy of the common block out of torq_calc in navier5.f: common /ctorq/ dragx(0:maxobj),dragpx(0:maxobj),dragvx(0:maxobj) $ , dragy(0:maxobj),dragpy(0:maxobj),dragvy(0:maxobj) $ , dragz(0:maxobj),dragpz(0:maxobj),dragvz(0:maxobj) c $ , torqx(0:maxobj),torqpx(0:maxobj),torqvx(0:maxobj) $ , torqy(0:maxobj),torqpy(0:maxobj),torqvy(0:maxobj) $ , torqz(0:maxobj),torqpz(0:maxobj),torqvz(0:maxobj) c $ , dpdx_mean,dpdy_mean,dpdz_mean $ , dgtq(3,4) c There you have access to all components, including breakdown into pressure and viscous contributions. If you have only one object (or surface), dragx(0) = force in x direction (typ., = drag) dragy(0) = force in y direction (typ., = lift) If you have multiple objects/surfaces, then dragx(k)=force in x direction on object k, k=1,... and dragx(0) = sum_k=1,.. dragx(k) 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, March 30, 2017 3:33 AM To: Nek 5000 Subject: [Nek5000-users] Accessing the value of drag and lift coefficients in usrchk Hi Nek, I was wondering whether it was possible to access the values of the drag and lift coefficient directly into usrchk? I know how to compute them but they only get printed in the logfile. I would need them for a control problem. Thanks a lot Jean-Christophe B. Loiseau Ma?tre de conf?rence DynFluid, Arts et M?tiers ParisTech Homepage -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Mar 30 07:23:45 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 30 Mar 2017 14:23:45 +0200 Subject: [Nek5000-users] Accessing the value of drag and lift coefficients in usrchk In-Reply-To: References: Message-ID: Thanks a lot Paul! That is exactly what I was looking for (and what I had assumed) although I prefer to double check :) Regards, Jean-Christophe B. Loiseau Ma?tre de conf?rence DynFluid, Arts et M?tiers ParisTech Homepage > On 30 Mar 2017, at 14:22, nek5000-users at lists.mcs.anl.gov wrote: > > > Dear JC, > > Yes --- just pull a copy of the common block out of torq_calc in navier5.f: > > > common /ctorq/ dragx(0:maxobj),dragpx(0:maxobj),dragvx(0:maxobj) > > $ , dragy(0:maxobj),dragpy(0:maxobj),dragvy(0:maxobj) > > $ , dragz(0:maxobj),dragpz(0:maxobj),dragvz(0:maxobj) > > c > > $ , torqx(0:maxobj),torqpx(0:maxobj),torqvx(0:maxobj) > > $ , torqy(0:maxobj),torqpy(0:maxobj),torqvy(0:maxobj) > > $ , torqz(0:maxobj),torqpz(0:maxobj),torqvz(0:maxobj) > > c > > $ , dpdx_mean,dpdy_mean,dpdz_mean > > $ , dgtq(3,4) > > c > > > > There you have access to all components, including breakdown into pressure and viscous > contributions. > > If you have only one object (or surface), > > dragx(0) = force in x direction (typ., = drag) > dragy(0) = force in y direction (typ., = lift) > > If you have multiple objects/surfaces, then dragx(k)=force in x direction on object k, k=1,... > and dragx(0) = sum_k=1,.. dragx(k) > > 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, March 30, 2017 3:33 AM > To: Nek 5000 > Subject: [Nek5000-users] Accessing the value of drag and lift coefficients in usrchk > > Hi Nek, > > I was wondering whether it was possible to access the values of the drag and lift coefficient directly into usrchk? > I know how to compute them but they only get printed in the logfile. I would need them for a control problem. > > Thanks a lot > > Jean-Christophe B. Loiseau > Ma?tre de conf?rence > DynFluid, Arts et M?tiers ParisTech > > 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 Mar 30 11:38:22 2017 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 30 Mar 2017 16:38:22 +0000 Subject: [Nek5000-users] Interpolation between two meshes In-Reply-To: References: Message-ID: Hi Stefan, Many thanks for your reply. Please contact me via wzx1989221 at gmail.com. Best regards, Tony ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov on behalf of nek5000-users-request at lists.mcs.anl.gov Sent: 30 March 2017 13:17 To: nek5000-users at lists.mcs.anl.gov Subject: Nek5000-users Digest, Vol 97, Issue 37 Today's Topics: 1. Outflow BC with negative velocity (nek5000-users at lists.mcs.anl.gov) 2. Re: NekNek with PN-PN (nek5000-users at lists.mcs.anl.gov) 3. Re: NekNek with PN-PN (nek5000-users at lists.mcs.anl.gov) 4. Re: Interpolation between two meshes (nek5000-users at lists.mcs.anl.gov) 5. Accessing the value of drag and lift coefficients in usrchk (nek5000-users at lists.mcs.anl.gov) Message: 4 Date: Thu, 30 Mar 2017 11:46:40 +0200 From: nek5000-users at lists.mcs.anl.gov To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Interpolation between two meshes Message-ID: Content-Type: text/plain; charset="utf-8" Please let me know how I can contact you off list. Stefan? On 29 Mar 2017, at 14:59, "nek5000-users at lists.mcs.anl.gov " > wrote: Hi Stefan, Thank you very much for your quick reply. 1. Yes, my source field is in double precision since I need to keep the accuracy. 2. I added several print lines in gfldr.f to check where the interpolation hangs (see below). I also put 'call nekgsync()' before and after findpts as you suggested. I can confirm that findpts is exactly where the interpolation hangs. The last output in the logfile is 'CHECK interp findpts before' and it never gets updated again. 3. I've just tested gfldr() with turbChannel example. Everything worked fine and the?source field was interpolated onto the turbChannel mesh (512 elements). So I moved on increasing the number of elements of turbChannel case. First, I used 234300 elements?in the turbChannel example (half of my current simulation size) and the interpolation was done successfully. Then, I used 468600 elements for?the turbChannel example (similar to my current simulation size), the interpolation hangs again at findpts. I guess it might be something to do with the memory. What do you think? Is there any solution to this? Best regards, Tony ??????? if(nid==0) print*,'CHECK interp findpts before' ??????? call nekgsync() ??????? call findpts(inth_gfldr, ???? &?????????????? rcode,1, ???? &?????????????? proc,1, ???? &?????????????? elid,1, ???? &?????????????? rst,ndim, ???? &?????????????? dist,1, ???? &?????????????? xm1,1, ???? &?????????????? ym1,1, ???? &?????????????? zm1,1,ntot) ??????? call nekgsync() ??????? if(nid==0) print*,'CHECK interp findpts after' -------------- next part -------------- An HTML attachment was scrubbed... URL: