From nek5000-users at lists.mcs.anl.gov Fri Jul 1 14:03:07 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 1 Jul 2016 19:03:07 +0000 Subject: [Nek5000-users] symmetry boundary conditions and genmap In-Reply-To: References: Message-ID: Hi Marco, It looks maybe like you replaced "W" by "SYM" ? In the .rea file, if a line has a character that is read by nek, then the line has to be formatted, which means that spaces in the line are important. Thus, you should replace "W " ('W-space-space) by "SYM" , i.e., all bcs are read as 3 character strings. Now, concerning SYM, there is another constraint --- namely the following: Any SYM boundary must be aligned with either X , Y, or Z unit normals, unless you're using the stress formulation. The reason is that, say, for a SYM boundary that has unit normal in the Z direction, the velocity bcs are: du/dz = 0 , dv/dz = 0, w=0 That is, Dirichlet for w and Neumann for u and v. If the SYM bc is not aligned, it ends up being a mixed bc for the 3 velocity components, which in Nek can at present be handled only with the stress formulation, which means PN-PN-2, and not PN-PN. 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, June 30, 2016 7:46 AM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] symmetry boundary conditions and genmap Hello, I have two rea files that are exactly identical but for the boundary conditions: one has ?W? and the other one has ?SYM?. If I am not mistaken, the ?SYM? boundary type is supported by Nek5000 but is causing problem when I try to generate a map file with genmap. It returns the following error message: reading .rea file data ... ERROR: error reading 1 79200 299357 aborting 530 in routine rdbdry. 1 quit The rea file with ?W? boundary type successfully goes through the genmap script. Is there anything I should be aware when setting SYM bc type in the rea file? I could not find any related post in the archive of the mailing list. Thanks, Marco _______________________________________________ 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 Jul 1 15:18:51 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 1 Jul 2016 20:18:51 +0000 Subject: [Nek5000-users] symmetry boundary conditions and genmap In-Reply-To: References: Message-ID: Paul, I fixed my python script and was able to generate the map file. I noticed, however, in the output the following message: not connected 1 3 9 0 Could you please explain what means this message? Thanks, Marco > On Jul 1, 2016, at 3:03 PM, nek5000-users at lists.mcs.anl.gov wrote: > > > Hi Marco, > > It looks maybe like you replaced "W" by "SYM" ? > > In the .rea file, if a line has a character that is read by nek, then the line has to be formatted, > which means that spaces in the line are important. > > Thus, you should replace "W " ('W-space-space) by "SYM" , i.e., all bcs are read as 3 character > strings. > > Now, concerning SYM, there is another constraint --- namely the following: > > Any SYM boundary must be aligned with either X , Y, or Z unit normals, unless you're using the > stress formulation. > > The reason is that, say, for a SYM boundary that has unit normal in the Z direction, the velocity > bcs are: > > du/dz = 0 , dv/dz = 0, w=0 > > That is, Dirichlet for w and Neumann for u and v. > > If the SYM bc is not aligned, it ends up being a mixed bc for the 3 velocity components, which > in Nek can at present be handled only with the stress formulation, which means PN-PN-2, and > not PN-PN. > > 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, June 30, 2016 7:46 AM > To: nek5000-users at lists.mcs.anl.gov > Subject: [Nek5000-users] symmetry boundary conditions and genmap > > Hello, > > I have two rea files that are exactly identical but for the boundary conditions: one has ?W? and the other one has ?SYM?. If I am not mistaken, the ?SYM? boundary type is supported by Nek5000 but is causing problem when I try to generate a map file with genmap. It returns the following error message: > reading .rea file data ... > ERROR: error reading 1 79200 299357 > aborting 530 in routine rdbdry. > > 1 quit > > The rea file with ?W? boundary type successfully goes through the genmap script. Is there anything I should be aware when setting SYM bc type in the rea file? > > I could not find any related post in the archive of the mailing list. > > 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 > From nek5000-users at lists.mcs.anl.gov Fri Jul 1 15:39:59 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 1 Jul 2016 20:39:59 +0000 Subject: [Nek5000-users] symmetry boundary conditions and genmap In-Reply-To: References: , Message-ID: Hi Marco, genmap uses recursive spectral bisection to partition the graph across processors. RSB does not guarantee connected subgraphs except in the continuous case (i.e., infinite resolution). We have several heuristics to repair disconnected subgraphs, if they all fail you get the warning below. For small integers, like the one shown, there is now worry. However, if the integers were in the 100s or higher it could be detrimental to parallel performance, particularly when using the (default) XXt-based coarse-grid solver. (AMG-based coarse grid solver is not so sensitive...) 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, July 01, 2016 3:18 PM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] symmetry boundary conditions and genmap Paul, I fixed my python script and was able to generate the map file. I noticed, however, in the output the following message: not connected 1 3 9 0 Could you please explain what means this message? Thanks, Marco > On Jul 1, 2016, at 3:03 PM, nek5000-users at lists.mcs.anl.gov wrote: > > > Hi Marco, > > It looks maybe like you replaced "W" by "SYM" ? > > In the .rea file, if a line has a character that is read by nek, then the line has to be formatted, > which means that spaces in the line are important. > > Thus, you should replace "W " ('W-space-space) by "SYM" , i.e., all bcs are read as 3 character > strings. > > Now, concerning SYM, there is another constraint --- namely the following: > > Any SYM boundary must be aligned with either X , Y, or Z unit normals, unless you're using the > stress formulation. > > The reason is that, say, for a SYM boundary that has unit normal in the Z direction, the velocity > bcs are: > > du/dz = 0 , dv/dz = 0, w=0 > > That is, Dirichlet for w and Neumann for u and v. > > If the SYM bc is not aligned, it ends up being a mixed bc for the 3 velocity components, which > in Nek can at present be handled only with the stress formulation, which means PN-PN-2, and > not PN-PN. > > 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, June 30, 2016 7:46 AM > To: nek5000-users at lists.mcs.anl.gov > Subject: [Nek5000-users] symmetry boundary conditions and genmap > > Hello, > > I have two rea files that are exactly identical but for the boundary conditions: one has ?W? and the other one has ?SYM?. If I am not mistaken, the ?SYM? boundary type is supported by Nek5000 but is causing problem when I try to generate a map file with genmap. It returns the following error message: > reading .rea file data ... > ERROR: error reading 1 79200 299357 > aborting 530 in routine rdbdry. > > 1 quit > > The rea file with ?W? boundary type successfully goes through the genmap script. Is there anything I should be aware when setting SYM bc type in the rea file? > > I could not find any related post in the archive of the mailing list. > > 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 From nek5000-users at lists.mcs.anl.gov Wed Jul 6 18:42:41 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 6 Jul 2016 23:42:41 +0000 Subject: [Nek5000-users] Turbulence Models not yet implemented Message-ID: I am trying to generate a set of DNS data for a turbulent channel flow, and I am currently trying to build my case in prex. When I try to select "Turbulence Model", it says "Turbulence Models not yet implemented". How can this be the case if there is already an example turbulent channel flow included with Nek5000? -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Jul 6 19:01:51 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 6 Jul 2016 17:01:51 -0700 Subject: [Nek5000-users] Turbulence Models not yet implemented In-Reply-To: References: Message-ID: Why would you need a Turbulence Model if you are going to do a DNS? Best regards, Yulia On Jul 6, 2016, at 4:42 PM, nek5000-users at lists.mcs.anl.gov wrote: > I am trying to generate a set of DNS data for a turbulent channel flow, and I am currently trying to build my case in prex. When I try to select ?Turbulence Model?, it says ?Turbulence Models not yet implemented?. How can this be the case if there is already an example turbulent channel flow included with Nek5000? > _______________________________________________ > 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 Jul 7 11:11:24 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 7 Jul 2016 09:11:24 -0700 Subject: [Nek5000-users] Turbulence Models not yet implemented In-Reply-To: References: Message-ID: Let me explain slightly better. For Direct Numerical Simulations (DNS), all the scales of turbulence are computed directly and no scales are modeled. Thus, no turbulence model is needed, you will get turbulence naturally as the direct solution of equations. Usually, some initial perturbation of the flow field is recommended to get the statistically-converged turbulence faster. For Large Eddy Simulations (LES), only the largest scales are computed directly, and the smaller scales are modeled (with the so-called sub grid-scale (SGS) models). SGS models for LES are available in Nek5000, including classical Smagorinsky and dynamic Smagorinsky models (they are in a TurbChannel example). For Reynolds Averaged Navier Stokes (RANS) simulations, all scales of motion are modeled. RANS models for Nek5000 are still in an exploratory stage and I believe are not yet part of the repo suite. Please, let me know if you have any further questions. Best regards, Yulia On Jul 6, 2016, at 4:42 PM, nek5000-users at lists.mcs.anl.gov wrote: > I am trying to generate a set of DNS data for a turbulent channel flow, and I am currently trying to build my case in prex. When I try to select ?Turbulence Model?, it says ?Turbulence Models not yet implemented?. How can this be the case if there is already an example turbulent channel flow included with Nek5000? > _______________________________________________ > 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 Jul 7 12:35:51 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 7 Jul 2016 17:35:51 +0000 Subject: [Nek5000-users] Turbulence Models not yet implemented In-Reply-To: References: Message-ID: I apologize, I wasn't very clear in my previous message, at all. My question is this: there is a turbulent channel example included with Nek5000. According to the file turbChannel.usr, I have the understanding that this is an LES model of a turbulent channel at Re(tau)=590. How can this be an LES model if there are no turbulence models implemented in Nek5000? From: nek5000-users-bounces at lists.mcs.anl.gov [mailto:nek5000-users-bounces at lists.mcs.anl.gov] On Behalf Of nek5000-users at lists.mcs.anl.gov Sent: Thursday, July 07, 2016 11:11 AM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] Turbulence Models not yet implemented Let me explain slightly better. For Direct Numerical Simulations (DNS), all the scales of turbulence are computed directly and no scales are modeled. Thus, no turbulence model is needed, you will get turbulence naturally as the direct solution of equations. Usually, some initial perturbation of the flow field is recommended to get the statistically-converged turbulence faster. For Large Eddy Simulations (LES), only the largest scales are computed directly, and the smaller scales are modeled (with the so-called sub grid-scale (SGS) models). SGS models for LES are available in Nek5000, including classical Smagorinsky and dynamic Smagorinsky models (they are in a TurbChannel example). For Reynolds Averaged Navier Stokes (RANS) simulations, all scales of motion are modeled. RANS models for Nek5000 are still in an exploratory stage and I believe are not yet part of the repo suite. Please, let me know if you have any further questions. Best regards, Yulia On Jul 6, 2016, at 4:42 PM, nek5000-users at lists.mcs.anl.gov wrote: I am trying to generate a set of DNS data for a turbulent channel flow, and I am currently trying to build my case in prex. When I try to select "Turbulence Model", it says "Turbulence Models not yet implemented". How can this be the case if there is already an example turbulent channel flow included with Nek5000? _______________________________________________ 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 Jul 9 11:03:15 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sat, 9 Jul 2016 09:03:15 -0700 Subject: [Nek5000-users] Turbulence Models not yet implemented In-Reply-To: References: Message-ID: In turbChannel example. if param(30) = 1, then ifuservp is true, i.e., the uservp subroutine is being called which allows you to use the user-defined viscosity, in this case dynamic Smagorinsky based eddy viscosity. Also, if param(30) = 0, nek5000 uses a filter-based model based on the values of param(101), param(103). It is a little unconventional, but it can also be treated as an LES model, damping out smaller scales of motion. On Thu, Jul 7, 2016 at 10:35 AM, wrote: > I apologize, I wasn?t very clear in my previous message, at all. > > > > My question is this: there is a turbulent channel example included with > Nek5000. According to the file turbChannel.usr, I have the understanding > that this is an LES model of a turbulent channel at Re(tau)=590. How can > this be an LES model if there are no turbulence models implemented in > Nek5000? > > > > *From:* nek5000-users-bounces at lists.mcs.anl.gov [mailto: > nek5000-users-bounces at lists.mcs.anl.gov] *On Behalf Of * > nek5000-users at lists.mcs.anl.gov > *Sent:* Thursday, July 07, 2016 11:11 AM > *To:* nek5000-users at lists.mcs.anl.gov > *Subject:* Re: [Nek5000-users] Turbulence Models not yet implemented > > > > Let me explain slightly better. For Direct Numerical Simulations (DNS), > all the scales of turbulence are computed directly and no scales are > modeled. Thus, no turbulence model is needed, you will get turbulence > naturally as the direct solution of equations. Usually, some initial > perturbation of the flow field is recommended to get the > statistically-converged turbulence faster. For Large Eddy Simulations > (LES), only the largest scales are computed directly, and the smaller > scales are modeled (with the so-called sub grid-scale (SGS) models). SGS > models for LES are available in Nek5000, including classical Smagorinsky > and dynamic Smagorinsky models (they are in a TurbChannel example). For > Reynolds Averaged Navier Stokes (RANS) simulations, all scales of motion > are modeled. RANS models for Nek5000 are still in an exploratory stage and > I believe are not yet part of the repo suite. > > > > Please, let me know if you have any further questions. > > > > Best regards, > > Yulia > > > > On Jul 6, 2016, at 4:42 PM, nek5000-users at lists.mcs.anl.gov wrote: > > > > I am trying to generate a set of DNS data for a turbulent channel flow, > and I am currently trying to build my case in prex. When I try to select > ?Turbulence Model?, it says ?Turbulence Models not yet implemented?. How > can this be the case if there is already an example turbulent channel flow > included with Nek5000? > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Sun Jul 10 09:13:06 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 10 Jul 2016 16:13:06 +0200 Subject: [Nek5000-users] Turbulence Models not yet implemented In-Reply-To: References: Message-ID: Models typically "live" in the .usr file. There is no turbulence model in the code itself, except a legacy k-eps. Not sure if this implementation is up-to-date and well tested. > On 09.07.2016, at 18:03, nek5000-users at lists.mcs.anl.gov wrote: > > In turbChannel example. if param(30) = 1, then ifuservp is true, i.e., the uservp subroutine is being called which allows you to use the user-defined viscosity, in this case dynamic Smagorinsky based eddy viscosity. > > Also, if param(30) = 0, nek5000 uses a filter-based model based on the values of param(101), param(103). It is a little unconventional, but it can also be treated as an LES model, damping out smaller scales of motion. > >> On Thu, Jul 7, 2016 at 10:35 AM, wrote: >> I apologize, I wasn?t very clear in my previous message, at all. >> >> >> >> My question is this: there is a turbulent channel example included with Nek5000. According to the file turbChannel.usr, I have the understanding that this is an LES model of a turbulent channel at Re(tau)=590. How can this be an LES model if there are no turbulence models implemented in Nek5000? >> >> >> >> From: nek5000-users-bounces at lists.mcs.anl.gov [mailto:nek5000-users-bounces at lists.mcs.anl.gov] On Behalf Of nek5000-users at lists.mcs.anl.gov >> Sent: Thursday, July 07, 2016 11:11 AM >> To: nek5000-users at lists.mcs.anl.gov >> Subject: Re: [Nek5000-users] Turbulence Models not yet implemented >> >> >> >> Let me explain slightly better. For Direct Numerical Simulations (DNS), all the scales of turbulence are computed directly and no scales are modeled. Thus, no turbulence model is needed, you will get turbulence naturally as the direct solution of equations. Usually, some initial perturbation of the flow field is recommended to get the statistically-converged turbulence faster. For Large Eddy Simulations (LES), only the largest scales are computed directly, and the smaller scales are modeled (with the so-called sub grid-scale (SGS) models). SGS models for LES are available in Nek5000, including classical Smagorinsky and dynamic Smagorinsky models (they are in a TurbChannel example). For Reynolds Averaged Navier Stokes (RANS) simulations, all scales of motion are modeled. RANS models for Nek5000 are still in an exploratory stage and I believe are not yet part of the repo suite. >> >> >> >> Please, let me know if you have any further questions. >> >> >> >> Best regards, >> >> Yulia >> >> >> >> On Jul 6, 2016, at 4:42 PM, nek5000-users at lists.mcs.anl.gov wrote: >> >> >> >> >> I am trying to generate a set of DNS data for a turbulent channel flow, and I am currently trying to build my case in prex. When I try to select ?Turbulence Model?, it says ?Turbulence Models not yet implemented?. How can this be the case if there is already an example turbulent channel flow included with Nek5000? >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> >> >> >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Sun Jul 10 12:39:10 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 10 Jul 2016 19:39:10 +0200 Subject: [Nek5000-users] WSS on several processors Message-ID: Hi Neks, I am working with two routines (torq_calc and drgtrq )in navier5.f. I'm trying to collect viscous drag's values on the wall (in all the grid points) and write them into a file. If I run a calculation on the one CPU it works great, but it doesn't work with several processors: I have an impression that the information is written into result file from only one processors. How can I fix this problem? Thank you for any suggestion, Andrew -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jul 11 11:20:18 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 11 Jul 2016 18:20:18 +0200 Subject: [Nek5000-users] WSS on several processors In-Reply-To: References: Message-ID: PS: In fact I have the same issue as http://lists.mcs.anl.gov/pipermail/nek5000-users/2010-June/000674.html , but i didn't find the solution of this one. 2016-07-10 19:39 GMT+02:00 : > Hi Neks, > > I am working with two routines (torq_calc and drgtrq )in navier5.f. I'm > trying to collect viscous drag's values on the wall (in all the grid > points) and write them into a file. If I run a calculation on the one CPU > it works great, but it doesn't work with several processors: I have an > impression that the information is written into result file from only one > processors. How can I fix this problem? > > Thank you for any suggestion, > Andrew > > _______________________________________________ > 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 Jul 11 11:58:21 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 11 Jul 2016 16:58:21 +0000 Subject: [Nek5000-users] WSS on several processors In-Reply-To: References: Message-ID: Hi Andrew, torq_calc (which also computes drag as a byproduct) will generate integral quantities over several objects. So, you could have (say) the upper and lower wall as two separate objects, and you can get the drag on each. This amounts to 2 vector quantities (3 numbers each: fx,fy,fz) at each time step and is written out by node 0. It sounds like you are asking for something different, e.g., the wall shear stress as a function of position --- that requires a bit more sophistication but is certainly accessible. What are you looking for? Best, Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Sunday, July 10, 2016 12:39 PM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] WSS on several processors Hi Neks, I am working with two routines (torq_calc and drgtrq )in navier5.f. I'm trying to collect viscous drag's values on the wall (in all the grid points) and write them into a file. If I run a calculation on the one CPU it works great, but it doesn't work with several processors: I have an impression that the information is written into result file from only one processors. How can I fix this problem? Thank you for any suggestion, Andrew -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Jul 12 03:30:47 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 12 Jul 2016 10:30:47 +0200 Subject: [Nek5000-users] WSS on several processors In-Reply-To: References: Message-ID: Hi Paul, Yes, torq_calc generates integral quantities, viscous drag (dragvx, dragvy, dragvz) for example. You are right, my issue is different: I defined an object, which is a cylindric pipe's wall, with set_obj; and now I' m trying to find all the coordinates of this object and quantities dg(1,2), dg(2,2), dg(3,2) in these coordinates. My code works fine for the serial setting but with parallel setting only a part of coordinates is dumped into the file. And this part corresponds to the values of one CPU (I run my case with 16 CPU on one node). I have tried to use subroutine gop(x, w op, n) but it doesn't work. Best regards, Andrew 2016-07-11 18:58 GMT+02:00 : > > Hi Andrew, > > torq_calc (which also computes drag as a byproduct) will generate integral > quantities over several > objects. > > So, you could have (say) the upper and lower wall as two separate objects, > and you can get the > drag on each. This amounts to 2 vector quantities (3 numbers each: > fx,fy,fz) at each time step > and is written out by node 0. > > It sounds like you are asking for something different, e.g., the wall > shear stress as a function of > position --- that requires a bit more sophistication but is certainly > accessible. > > What are you looking for? > > Best, Paul > > ------------------------------ > *From:* nek5000-users-bounces at lists.mcs.anl.gov [ > nek5000-users-bounces at lists.mcs.anl.gov] on behalf of > nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > *Sent:* Sunday, July 10, 2016 12:39 PM > *To:* nek5000-users at lists.mcs.anl.gov > *Subject:* [Nek5000-users] WSS on several processors > > Hi Neks, > > I am working with two routines (torq_calc and drgtrq )in navier5.f. I'm > trying to collect viscous drag's values on the wall (in all the grid > points) and write them into a file. If I run a calculation on the one CPU > it works great, but it doesn't work with several processors: I have an > impression that the information is written into result file from only one > processors. How can I fix this problem? > > Thank you for any suggestion, > Andrew > > _______________________________________________ > 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 Jul 12 04:42:52 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 12 Jul 2016 11:42:52 +0200 Subject: [Nek5000-users] NeK5000+SuperMUC Message-ID: Dear all, I am writing to kindly ask if anyone has experience of running NeK5000 on German HPC Systems (SuperMUC, Juqeen, HazelHen). In particular, I would like to know that if the nek5000 codes run on any of these machines, especially on SuperMUC? Many thanks, Hamed Sadeghi PostDoc Research Fellow, TU Darmstadt -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Jul 12 08:13:57 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 12 Jul 2016 13:13:57 +0000 Subject: [Nek5000-users] NeK5000+SuperMUC In-Reply-To: References: Message-ID: Hi Hamed, Nek will run on any platform that supports MPI -- I would assume that these would do so. Generally the only tuning required might be to change the mxm (matrix-matrix product) routines, but the defaults are also quite good. 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, July 12, 2016 4:42 AM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] NeK5000+SuperMUC Dear all, I am writing to kindly ask if anyone has experience of running NeK5000 on German HPC Systems (SuperMUC, Juqeen, HazelHen). In particular, I would like to know that if the nek5000 codes run on any of these machines, especially on SuperMUC? Many thanks, Hamed Sadeghi PostDoc Research Fellow, TU Darmstadt -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Jul 12 08:31:11 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 12 Jul 2016 13:31:11 +0000 Subject: [Nek5000-users] WSS on several processors In-Reply-To: References: , Message-ID: Hi Andrew, How you write to the file depends on the underlying structure that you want at output. I'm assuming there is no particular order in this case and therefore you also need to write out the coordinates. Presumably you've already addressed these questions in your working serial version. Let's assume you have an array with 6 quantities per grid point: my_data(6,n) and let's assume that you've already figured out how to write it in serial. To do a parallel write, one processor at a time (which actually is a serial write... but it's ok), you could do the following: real my_data(6,nmax...) do mid=0,np-1 ! march over all processors if (mid.eq.0.and.nid.eq.0) then open(unit=50,file='my_file.out') write(6,1) ((my_data(k,j),k=1,6),j=1,n) elseif (mid.gt.0.and.mid.eq.0) then handshake=1 len=wdsize len4=4 mtag=777 call csend(mtag,handshake,len,mid,0) ! send handshake to mid call crecv(mtag,n,len4) ! get number of incoming words call csend(mtag,handshake,len,mid,0) ! send handshake to mid len = wdsize*n*6 call crecv(my_data,n,len) ! get data from mid write(6,1) ((my_data(k,j),k=1,6),j=1,n) else ! mid > 0 len = wdsize len4=4 call crecv(mtag,handshake,len) call csend(mtag,n,len4,0,0) ! send data size to node 0 call crecv(mtag,handshake,len) len = wdsize*n*6 call csend(mtag,my_data,len,0,0) endif if (nid.eq.0) close(50) 1 format(1p6e19.11) I've not tested this... but it should be reasonably close to working... 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, July 12, 2016 3:30 AM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] WSS on several processors Hi Paul, Yes, torq_calc generates integral quantities, viscous drag (dragvx, dragvy, dragvz) for example. You are right, my issue is different: I defined an object, which is a cylindric pipe's wall, with set_obj; and now I' m trying to find all the coordinates of this object and quantities dg(1,2), dg(2,2), dg(3,2) in these coordinates. My code works fine for the serial setting but with parallel setting only a part of coordinates is dumped into the file. And this part corresponds to the values of one CPU (I run my case with 16 CPU on one node). I have tried to use subroutine gop(x, w op, n) but it doesn't work. Best regards, Andrew 2016-07-11 18:58 GMT+02:00 >: Hi Andrew, torq_calc (which also computes drag as a byproduct) will generate integral quantities over several objects. So, you could have (say) the upper and lower wall as two separate objects, and you can get the drag on each. This amounts to 2 vector quantities (3 numbers each: fx,fy,fz) at each time step and is written out by node 0. It sounds like you are asking for something different, e.g., the wall shear stress as a function of position --- that requires a bit more sophistication but is certainly accessible. What are you looking for? Best, Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Sunday, July 10, 2016 12:39 PM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] WSS on several processors Hi Neks, I am working with two routines (torq_calc and drgtrq )in navier5.f. I'm trying to collect viscous drag's values on the wall (in all the grid points) and write them into a file. If I run a calculation on the one CPU it works great, but it doesn't work with several processors: I have an impression that the information is written into result file from only one processors. How can I fix this problem? Thank you for any suggestion, Andrew _______________________________________________ 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 Jul 12 11:25:53 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 12 Jul 2016 11:25:53 -0500 Subject: [Nek5000-users] Postnek Issue on Github Message-ID: Hi All, I've noticed that when I try to make the tools using the Github version of Nek, it results in an error while trying to make postnek. I found the issue raised for this problem on Github ( https://github.com/Nek5000/nek5000/issues/16), but I don't see a corresponding open pull request; is someone planning to submit a PR? Regards, Kento -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Jul 12 11:36:00 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 12 Jul 2016 11:36:00 -0500 Subject: [Nek5000-users] Postnek Issue on Github In-Reply-To: References: Message-ID: Hi Kento, Thanks for the reminder. I'll submit a PR today. Best, Ron On Tue, Jul 12, 2016 at 11:25 AM, wrote: > Hi All, > > I've noticed that when I try to make the tools using the Github version of > Nek, it results in an error while trying to make postnek. I found the issue > raised for this problem on Github ( > https://github.com/Nek5000/nek5000/issues/16), but I don't see a > corresponding open pull request; is someone planning to submit a PR? > > Regards, > Kento > > _______________________________________________ > 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 Jul 13 10:20:38 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 13 Jul 2016 15:20:38 +0000 Subject: [Nek5000-users] Access to an undefined portion of a memory object. Message-ID: Hello, I have a subroutine that interpolates the velocity for a list of points and have a strange error message when I try to run it. It seems that the variables ?nx1?, ?ny1? and nz1? are not defined even though ?SIZE? is included in the subroutine. As far I understand, the variables ?nx1?, ?ny1? and 'nz1? are made available in a subroutine by simply including ?SIZE? at the beginning. I attached the case to reproduce the error message that is: Access to an undefined portion of a memory object. Any help would be appreciated. Marco -------------- next part -------------- A non-text attachment was scrubbed... Name: 3d-pipe-recycling-bcs.zip Type: application/zip Size: 17832866 bytes Desc: 3d-pipe-recycling-bcs.zip URL: From nek5000-users at lists.mcs.anl.gov Wed Jul 13 11:10:44 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 13 Jul 2016 16:10:44 +0000 Subject: [Nek5000-users] Access to an undefined portion of a memory object. In-Reply-To: References: Message-ID: Hi Marco, It looks to me like you're trying to overwrite a constant in interp_vt(). I see the following: call interp_vt(ih_rbc,uvwt,xyz,npts,.false.) ! interpolation : : : subroutine interp_vt(ihandle,uvwt,xyz,n,iftmp) : : iftmp = .false. ! no temperature which is trying to overwrite ".false." ... ? Please let me know if this resolves your issue. Also, I see in your SIZE file that lelt=10000. Are you running only on one processor? If the number of elements in your .rea file is ~10,000 and you are running on (say) 1024 MPI ranks, then you only need lelt=10. Resetting lelt and lelv in this way would result in a significant reduction in memory footprint and possible increase in performance. 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: Wednesday, July 13, 2016 10:20 AM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] Access to an undefined portion of a memory object. Hello, I have a subroutine that interpolates the velocity for a list of points and have a strange error message when I try to run it. It seems that the variables ?nx1?, ?ny1? and nz1? are not defined even though ?SIZE? is included in the subroutine. As far I understand, the variables ?nx1?, ?ny1? and 'nz1? are made available in a subroutine by simply including ?SIZE? at the beginning. I attached the case to reproduce the error message that is: Access to an undefined portion of a memory object. Any help would be appreciated. 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 Wed Jul 13 11:51:03 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 13 Jul 2016 16:51:03 +0000 Subject: [Nek5000-users] Access to an undefined portion of a memory object. In-Reply-To: References: Message-ID: Paul, thanks for you reply. It did solve the problem. I was running on one processor for debugging purposes only. Marco On Jul 13, 2016, at 12:10 PM, nek5000-users at lists.mcs.anl.gov wrote: Hi Marco, It looks to me like you're trying to overwrite a constant in interp_vt(). I see the following: call interp_vt(ih_rbc,uvwt,xyz,npts,.false.) ! interpolation : : : subroutine interp_vt(ihandle,uvwt,xyz,n,iftmp) : : iftmp = .false. ! no temperature which is trying to overwrite ".false." ... ? Please let me know if this resolves your issue. Also, I see in your SIZE file that lelt=10000. Are you running only on one processor? If the number of elements in your .rea file is ~10,000 and you are running on (say) 1024 MPI ranks, then you only need lelt=10. Resetting lelt and lelv in this way would result in a significant reduction in memory footprint and possible increase in performance. 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: Wednesday, July 13, 2016 10:20 AM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] Access to an undefined portion of a memory object. Hello, I have a subroutine that interpolates the velocity for a list of points and have a strange error message when I try to run it. It seems that the variables ?nx1?, ?ny1? and nz1? are not defined even though ?SIZE? is included in the subroutine. As far I understand, the variables ?nx1?, ?ny1? and 'nz1? are made available in a subroutine by simply including ?SIZE? at the beginning. I attached the case to reproduce the error message that is: Access to an undefined portion of a memory object. Any help would be appreciated. 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 Wed Jul 13 15:27:38 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 13 Jul 2016 20:27:38 +0000 Subject: [Nek5000-users] problems in compiling the code for parallel run Message-ID: Hello Users, I have Redhat linux workstation, I have already compiled code with nekb by making changes in makenek file, but now I want to run it parallel. At first when I compiled it by making F77 = mpif77 and cc= mpicc and commenting IFMPI ="false" I got errors that mpi not found than I installed openmpi Now when I compile using makenek it gets compiled successfully but when I try to run it using nekbmpi i get errors like mv: cannot stat `eddy_uv.sch': No such file or directory and sometimes if i do ./nekbmpi eddy_uv 4 it and put enter i get no errors on first time but if i enter again for second time I get same error that is mv: cannot stat `eddy_uv.sch': No such file or directory I want to understand what mistake I am doing and what should I do to get rid of errors and also which file can help me to see whats going on in simulation Thanks, Mansi Patel -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Jul 14 07:20:10 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 14 Jul 2016 07:20:10 -0500 Subject: [Nek5000-users] problems in compiling the code for parallel run In-Reply-To: References: Message-ID: Hi Mansi, I suspect that you can safely ignore the error. The error probably comes from line 7 of the "nekbmpi" script: mv $1.sch $1.sch1 This command is intended to move the .sch file from a previous run, in case there's one in your directory. If this is your first run, there will be no .sch file in your directory, and the "mv" command will give the error you saw. So it probably doesn't indicate a problem. Best, Ron Rahaman Argonne National Laboratory, Math and Computer Science Division University of Chicago, Department of Computer Science On Wed, Jul 13, 2016 at 3:27 PM, wrote: > Hello Users, > > I have Redhat linux workstation, I have already compiled code with nekb by > making changes in makenek file, but now I want to run it parallel. At first > when I compiled it by making F77 = mpif77 and cc= mpicc and commenting > IFMPI ="false" I got errors that mpi not found than I installed openmpi > > Now when I compile using makenek it gets compiled successfully but when I > try to run it using nekbmpi i get errors like > mv: cannot stat `eddy_uv.sch': No such file or directory > and sometimes if i do ./nekbmpi eddy_uv 4 it and put enter i get no errors > on first time but if i enter again for second time I get same error that is mv: > cannot stat `eddy_uv.sch': No such file or directory > I want to understand what mistake I am doing and what should I do to get > rid of errors and also which file can help me to see whats going on in > simulation > > > Thanks, > Mansi Patel > > > _______________________________________________ > 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 Jul 15 03:29:26 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 15 Jul 2016 10:29:26 +0200 Subject: [Nek5000-users] (no subject) Message-ID: Hello Users, I have started running the basic example to understand the functioning of the code. I am using a windows 10 system and finding difficulties with the basic compiling of maketools and makenek file. I think this is happening because of system variable and compiler issues. I am using gcc and gfortran compilers. Has anyone gone through such kind of problems? Your suggestions will be of great help ! -- -------------------------------------- Shivang Aggarwal Faculty of Aerospace Engineering TU Delft -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Fri Jul 15 08:24:32 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 15 Jul 2016 13:24:32 +0000 Subject: [Nek5000-users] (no subject) In-Reply-To: References: Message-ID: Hi Shivang, Does the rest of the code (i.e., nek5000 proper) run ok? If so, then your problem likely is the xlib interface on your platform. For post processing you have an alternative in VisIt, which is also freely downloadable. For preprocessing there is, say, Cubit, for which there are a few converters available but which at present are really in beta form as far as I know. Your best bet is to be able to have prenek and postnek working.. and for this you need X windows to work on your PC. 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, July 15, 2016 3:29 AM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] (no subject) Hello Users, I have started running the basic example to understand the functioning of the code. I am using a windows 10 system and finding difficulties with the basic compiling of maketools and makenek file. I think this is happening because of system variable and compiler issues. I am using gcc and gfortran compilers. Has anyone gone through such kind of problems? Your suggestions will be of great help ! -- -------------------------------------- Shivang Aggarwal Faculty of Aerospace Engineering TU Delft -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jul 18 08:17:11 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 18 Jul 2016 13:17:11 +0000 Subject: [Nek5000-users] Recycling boundaries with multiple inlets and outlets Message-ID: Hello, I have been successfully using a recycling boundary script on a 3-d pipe thanks to Aleks and am now looking at a more complicated mesh that involves multiple inlets and outlets. For the sake of simplicity, let assume that there are two inlets I1 and I2 and two outlets O1 and O2. My objective is to set recycling bc with the following pattern: I1->O1 and I2->O2. Aleks suggested to tag each boundary and use some sort of it statement in ?userchk?. * is this the correct approach? * if it is, how do I implement this in Nek5000? Any help/comment would be appreciated. Thanks, Marco -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Jul 19 20:54:12 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 20 Jul 2016 01:54:12 +0000 Subject: [Nek5000-users] Free surface running Message-ID: Dear Nekers, I?m running the example of 2D free surface (fs_2). The domain is rectangular, with boundary conditions of ?P?,?P?,?W?,?MS? on the left, right, bottom and top boundaries. When I initialize a flow, say ux=1, uy=0, the left and right boundaries of the domain are tilted to the right due to the rightward flow. So, I was wondering if there is an option that only allows the top boundary moving while keeping the left and right boundaries stationary. (The b.c. of ?P? ?P? ?W? are still wanted on the left, right and bottom boundaries.) Any suggestion on this? Thank you, Peng From nek5000-users at lists.mcs.anl.gov Tue Jul 19 18:57:50 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 19 Jul 2016 19:57:50 -0400 Subject: [Nek5000-users] obtain Re number curves in Visit Message-ID: Dear Neks I am trying to simulate turbulent flow in a cylindrical pipe. I am fairly new to this. I wanted to know how to get plots for Re similar to the already existing velocity and pressure options there. Rudra -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Jul 19 19:12:12 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 19 Jul 2016 20:12:12 -0400 Subject: [Nek5000-users] nek workshops Message-ID: are there any workshops for people who want to learn NEK5000 from scratch? Apoorva -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Jul 21 14:47:18 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 21 Jul 2016 19:47:18 +0000 Subject: [Nek5000-users] Extract 2d output file for 3d data Message-ID: I am trying to extract the bottom plane data from a 3d run. I saw from a previous thread (Writing 2d output files for 3d data) that Paul suggested to use z_slice_g() and outfld2d() routines to extract and output a 2d cut from the 3d domain. I am however new to Nek5000 and have not been able to successfully use the above 2 routines. Can someone point me to an example where these 2 routines are used? Thanks, Nadim Nadim Zgheib Post Doctoral Associate Computational MultiPhysics Group University of Florida University Ave Gainesville, FL 32611 -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Fri Jul 22 13:04:50 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 22 Jul 2016 18:04:50 +0000 Subject: [Nek5000-users] avg_all and visnek Message-ID: All, I am using the built-in function avg_all() to save the time-average values in my simulation and run in the following error message when trying to open the ?avg? output files in Visit: 'The first time step in a Nek file must contain a mesh?. I can visualize the other output files just fine with Visit, i.e. inlet3d0.f000* where inlet3d in the case name. Is there a flag or input parameters in the rea file that I am supposed to change in order to dump the mesh data in the avg output files? Thanks, marco -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Fri Jul 22 13:17:03 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 22 Jul 2016 18:17:03 +0000 Subject: [Nek5000-users] avg_all and visnek In-Reply-To: References: Message-ID: Hi Marco, Did you have logical 'F' for the output specification of coordinate in your .rea file? One way to get the mesh coordinates into VisIt is to link or copy your first instantaneous field dump file (that is forced by Nek to have coordinates in it regardless of the output specification) into avg*0.f00000 and modify your visnek's .nek5000 file to point to this extra file modifying numtimesteps and firsttimestep: 0 Aleks ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Friday, July 22, 2016 1:04 PM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] avg_all and visnek All, I am using the built-in function avg_all() to save the time-average values in my simulation and run in the following error message when trying to open the ?avg? output files in Visit: 'The first time step in a Nek file must contain a mesh?. I can visualize the other output files just fine with Visit, i.e. inlet3d0.f000* where inlet3d in the case name. Is there a flag or input parameters in the rea file that I am supposed to change in order to dump the mesh data in the avg output files? Thanks, marco -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Fri Jul 22 13:52:10 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 22 Jul 2016 18:52:10 +0000 Subject: [Nek5000-users] avg_all and visnek In-Reply-To: References: Message-ID: Hi Aleks, thanks for your help. I did set CORDINATES to T in the block ?SPECIFICATIONS FOLLOW?. It was originally set to F. I copied my instantaneous dump file into avg*0.f00000 and then substituted firsttimestep:1 to firsttimestep:0. It did work. This is the first time I have to do such a thing when using avg_all() even though I have used avg_all() in the past. Is there anything that has changed in the code? Thanks, Marco On Jul 22, 2016, at 2:17 PM, nek5000-users at lists.mcs.anl.gov wrote: firsttimestep -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Fri Jul 22 14:34:45 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 22 Jul 2016 19:34:45 +0000 Subject: [Nek5000-users] avg_all and visnek In-Reply-To: References: , Message-ID: Interesting... Check whether there is a statement ifxyo = .false. in usrchk() which overrides .rea specification (typically after the first dump to save the disk space) Aleks ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Friday, July 22, 2016 1:52 PM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] avg_all and visnek Hi Aleks, thanks for your help. I did set CORDINATES to T in the block ?SPECIFICATIONS FOLLOW?. It was originally set to F. I copied my instantaneous dump file into avg*0.f00000 and then substituted firsttimestep:1 to firsttimestep:0. It did work. This is the first time I have to do such a thing when using avg_all() even though I have used avg_all() in the past. Is there anything that has changed in the code? Thanks, Marco On Jul 22, 2016, at 2:17 PM, nek5000-users at lists.mcs.anl.gov wrote: firsttimestep -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Fri Jul 22 14:48:52 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 22 Jul 2016 19:48:52 +0000 Subject: [Nek5000-users] avg_all and visnek In-Reply-To: References: Message-ID: Here is what I have in my usrchk(): subroutine userchk include 'SIZE' include 'TOTAL' include 'ZPER' ! Needed to communicate nelx,nely,nelz to my_stats common /my_recycle/ nslab,n_in_slab ifxyo = .true. if (istep.eq.0) call outpost(vx,vy,vz,pr,t,' ') ifxyo = .false. c call set_inflow(nslab,n_in_slab) ! set up inflow BCs nelx = n_in_slab nely = 1 nelz = nelgv/(nelx*nely) c if (istep.gt.0) call my_stats call avg_all() return end Marco On Jul 22, 2016, at 3:34 PM, nek5000-users at lists.mcs.anl.gov wrote: Interesting... Check whether there is a statement ifxyo = .false. in usrchk() which overrides .rea specification (typically after the first dump to save the disk space) Aleks ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Friday, July 22, 2016 1:52 PM To: nek5000-users at lists.mcs.anl.gov Subject: Re: [Nek5000-users] avg_all and visnek Hi Aleks, thanks for your help. I did set CORDINATES to T in the block ?SPECIFICATIONS FOLLOW?. It was originally set to F. I copied my instantaneous dump file into avg*0.f00000 and then substituted firsttimestep:1 to firsttimestep:0. It did work. This is the first time I have to do such a thing when using avg_all() even though I have used avg_all() in the past. Is there anything that has changed in the code? Thanks, Marco On Jul 22, 2016, at 2:17 PM, nek5000-users at lists.mcs.anl.gov wrote: firsttimestep _______________________________________________ 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 Jul 25 00:38:18 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Sun, 24 Jul 2016 22:38:18 -0700 Subject: [Nek5000-users] avg_all and visnek In-Reply-To: References: Message-ID: Hi Marco, It seems like ifxyo overwrites itself to .false. after istep .eq. 0 conditional statement. If you have the flexibility of running the code again (if it runs quickly), you can set ifxyo = .true. just before the avg_all() call. Otherwise, you can run, nek5000 is post-processing mode as follows. subroutine userchk include 'SIZE' include 'TOTAL' include 'ZPER' ! Needed to communicate nelx,nely,nelz to my_stats include 'RESTART' character*80 filename filename = 'avg.....fld..' call load_fld(filename) ifxyo = .true. call outpost(vx,vy,vz,pr,t,'avx') call exitt return end On Fri, Jul 22, 2016 at 12:48 PM, wrote: > Here is what I have in my usrchk(): > > subroutine userchk > include 'SIZE' > include 'TOTAL' > include 'ZPER' ! Needed to communicate nelx,nely,nelz to my_stats > > common /my_recycle/ nslab,n_in_slab > > ifxyo = .true. > if (istep.eq.0) call outpost(vx,vy,vz,pr,t,' ') > ifxyo = .false. > > c call set_inflow(nslab,n_in_slab) ! set up inflow BCs > > nelx = n_in_slab > nely = 1 > nelz = nelgv/(nelx*nely) > > c if (istep.gt.0) call my_stats > > call avg_all() > > return > end > > Marco > > On Jul 22, 2016, at 3:34 PM, nek5000-users at lists.mcs.anl.gov wrote: > > Interesting... Check whether there is a statement > > ifxyo = .false. in usrchk() which overrides .rea specification (typically > after the first dump to save the disk space) > > Aleks > ------------------------------ > *From:* nek5000-users-bounces at lists.mcs.anl.gov [ > nek5000-users-bounces at lists.mcs.anl.gov] on behalf of > nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] > *Sent:* Friday, July 22, 2016 1:52 PM > *To:* nek5000-users at lists.mcs.anl.gov > *Subject:* Re: [Nek5000-users] avg_all and visnek > > Hi Aleks, > > thanks for your help. > > I did set CORDINATES to T in the block ?SPECIFICATIONS FOLLOW?. It was > originally set to F. > > I copied my instantaneous dump file into avg*0.f00000 and then substituted > firsttimestep:1 to firsttimestep:0. It did work. > > This is the first time I have to do such a thing when using avg_all() even > though I have used avg_all() in the past. Is there anything that has > changed in the code? > > Thanks, > Marco > > On Jul 22, 2016, at 2:17 PM, nek5000-users at lists.mcs.anl.gov wrote: > > firsttimestep > > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jul 25 09:35:10 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 25 Jul 2016 16:35:10 +0200 Subject: [Nek5000-users] maketools prenek Message-ID: Hello Users, I am trying to build tools using maketools but, there are following errors in building prenek. Can anyone please help me understanding what is going wrong here? And what does Error 1 flag denotes? make[1]: Entering directory '/cygdrive/c/nek5_svn/trunk/tools/prenek' gcc -mcmodel=medium -c -DUNDERSCORE -Dr8 xdriver.c :0:4: error: expected identifier or ?(? before numeric constant xdriver.c: In function ?mainc_?: xdriver.c:875:5: warning: implicit declaration of function ?fprep_? [-Wimplicit-function-declaration] fprep_ (); /* run Fortran Main code */ ^ make[1]: *** [makefile:66: xdriver.o] Error 1 make[1]: Leaving directory '/cygdrive/c/nek5_svn/trunk/tools/prenek' make: *** [makefile:4: all] Error 1 ------------------------- Shivang Aggarwal MSc. Student Aerospace Engineering TU Delft,The Netherlands -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Mon Jul 25 09:31:46 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 25 Jul 2016 14:31:46 +0000 Subject: [Nek5000-users] Maketools Prenek Message-ID: Hello Users, I am trying to build tools using maketools but, there are following errors in building prenek. Can anyone please help me understanding what is going wrong here? And what does Error 1 flag denotes? make[1]: Entering directory '/cygdrive/c/nek5_svn/trunk/tools/prenek' gcc -mcmodel=medium -c -DUNDERSCORE -Dr8 xdriver.c :0:4: error: expected identifier or ?(? before numeric constant xdriver.c: In function ?mainc_?: xdriver.c:875:5: warning: implicit declaration of function ?fprep_? [-Wimplicit-function-declaration] fprep_ (); /* run Fortran Main code */ ^ make[1]: *** [makefile:66: xdriver.o] Error 1 make[1]: Leaving directory '/cygdrive/c/nek5_svn/trunk/tools/prenek' make: *** [makefile:4: all] Error 1 ------------------------- Shivang Aggarwal MSc. Student Aerospace Engineering TU Delft,The Netherlands From nek5000-users at lists.mcs.anl.gov Mon Jul 25 15:04:09 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 25 Jul 2016 20:04:09 +0000 Subject: [Nek5000-users] maketools prenek In-Reply-To: References: Message-ID: Hi Shivang, What platform are you compiling on? You might try, in make tools, turning BIGMEM to false... Just set: BIGMEM="true" to #BIGMEM="true" Then: maketools clean maketools all 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, July 25, 2016 9:35 AM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] maketools prenek Hello Users, I am trying to build tools using maketools but, there are following errors in building prenek. Can anyone please help me understanding what is going wrong here? And what does Error 1 flag denotes? make[1]: Entering directory '/cygdrive/c/nek5_svn/trunk/tools/prenek' gcc -mcmodel=medium -c -DUNDERSCORE -Dr8 xdriver.c :0:4: error: expected identifier or ?(? before numeric constant xdriver.c: In function ?mainc_?: xdriver.c:875:5: warning: implicit declaration of function ?fprep_? [-Wimplicit-function-declaration] fprep_ (); /* run Fortran Main code */ ^ make[1]: *** [makefile:66: xdriver.o] Error 1 make[1]: Leaving directory '/cygdrive/c/nek5_svn/trunk/tools/prenek' make: *** [makefile:4: all] Error 1 ------------------------- Shivang Aggarwal MSc. Student Aerospace Engineering TU Delft,The Netherlands -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Jul 26 14:12:26 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 26 Jul 2016 19:12:26 +0000 Subject: [Nek5000-users] Velocity inlet boundary condition issue Message-ID: Dear users, I have a channel simulation where I set the boundary condition of one of the domain side as 'v' (in the box file). Then in the userbc subroutine, I define the velocity at that boundary as a constant (say 0.1). After I run my simulation and visualise the result, the velocity at that boundary is not exactly the constant I put in the user file. Do you have any idea how this could happen? Thank you in advance. Best regards, Toon -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Jul 26 14:21:21 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 26 Jul 2016 19:21:21 +0000 Subject: [Nek5000-users] Velocity inlet boundary condition issue In-Reply-To: References: Message-ID: Hi Toon, If you also have Walls, then v=0 at the all, and 0.1 at the other grid points. However, what you have is a polynomial that is 0 at one point and 0.1 at the others... such a thing will be oscillatory. (Similar to Gibbs phenomena for Fourier representation of a square wave.) Usually, we would have a boundary layer that smoothly transitions from a constant down to zero at the wall. I usually do this with a polynomial fit that uses a polynomial order = (lx1-1) Paul ________________________________ From: nek5000-users-bounces at lists.mcs.anl.gov [nek5000-users-bounces at lists.mcs.anl.gov] on behalf of nek5000-users at lists.mcs.anl.gov [nek5000-users at lists.mcs.anl.gov] Sent: Tuesday, July 26, 2016 2:12 PM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] Velocity inlet boundary condition issue Dear users, I have a channel simulation where I set the boundary condition of one of the domain side as 'v' (in the box file). Then in the userbc subroutine, I define the velocity at that boundary as a constant (say 0.1). After I run my simulation and visualise the result, the velocity at that boundary is not exactly the constant I put in the user file. Do you have any idea how this could happen? Thank you in advance. Best regards, Toon -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Jul 27 10:01:53 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 27 Jul 2016 15:01:53 +0000 Subject: [Nek5000-users] Vortex within cylinder with rotating lid AND How to import from Soldiworks to Nek5000? Message-ID: Hello all, I have just recently started to familiarise myself using Linux and Nek5000 so my knowledge is quite limited(please bare with me). I am currently doing a summer project proposing to use Nek5000 rather than ANSYS Fluent to simulate swirling flow to investigate vortex breakdown. I am currently going over the examples within the SVN repository I downloaded to which I stumbled upon the vortex problem within a cylinder with a rotating lid. I was interested in finding out how to change the aspect ratio of the geometry. Additionally, I also wanted to confirm if its possible to import geometry from Solidworks into Nek5000? I have read that you can do it through Gambit but I am looking for some guide on how to do so. Kind Regards Dipendra -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Jul 27 10:38:51 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 27 Jul 2016 17:38:51 +0200 Subject: [Nek5000-users] Compiling with MOAB - no implicit type Message-ID: Hi How is Nek compiled with MOAB? (I?m a newbie on NEK) Implicit none is used extensively in the subroutines in moab.f but it seems that a lot of the variables in the include files are declared implicit so I get compile error no implicit type If implicit none is removed then it compiles I have a feeling I am missing something, is there a compiler setting that should be set? (gnu compiler on ubuntu 14.04) Best regards, Per -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Jul 27 12:04:23 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 27 Jul 2016 17:04:23 +0000 Subject: [Nek5000-users] Vortex within cylinder with rotating lid AND How to import from Soldiworks to Nek5000? In-Reply-To: References: Message-ID: Dipendra, You can stretch the height of the domain with the following call in usrdat2: z0 = 0.0 z1 = 5.0 ! New height call rescale_x(zm1,z0,z1) ... There is also discussion of mesh morphing in the user manual. Note that this morphing effectively lowers resolution (since the number of elements is unchanged). You can boost resolution by increasing N (lx1 in SIZE file). You might not need to do this, however. If you really stretch a lot you probably should rebuild the geometry in z using a 2D mesh of a disk, followed by n2to3 to extrude the 2D geometry to 3D. 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, July 27, 2016 10:01 AM To: nek5000-users at lists.mcs.anl.gov Subject: [Nek5000-users] Vortex within cylinder with rotating lid AND How to import from Soldiworks to Nek5000? Hello all, I have just recently started to familiarise myself using Linux and Nek5000 so my knowledge is quite limited(please bare with me). I am currently doing a summer project proposing to use Nek5000 rather than ANSYS Fluent to simulate swirling flow to investigate vortex breakdown. I am currently going over the examples within the SVN repository I downloaded to which I stumbled upon the vortex problem within a cylinder with a rotating lid. I was interested in finding out how to change the aspect ratio of the geometry. Additionally, I also wanted to confirm if its possible to import geometry from Solidworks into Nek5000? I have read that you can do it through Gambit but I am looking for some guide on how to do so. Kind Regards Dipendra -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Jul 27 14:40:41 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 27 Jul 2016 14:40:41 -0500 Subject: [Nek5000-users] Compiling with MOAB - no implicit type In-Reply-To: References: Message-ID: > Implicit none is used extensively in the subroutines in moab.f but it seems > that a lot of the variables in the include files are declared implicit so I > get compile error no implicit type? Yes, it was originally written this way to make sure the right variables are being set across various calls to moab.f. However, since the bulk of the code has been verified, we could potentially remove the "implicit none" statements and have it working cleanly. I also have a fix for adding the variable to NEKMOAB to remove the compiler error. However this is in a separate fork and I can submit a PR with the change. Ron, can you take a look at this if you have some time now ? > If implicit none is removed then it compiles? I have a feeling I am missing > something, is there a compiler setting that should be set? (gnu compiler on > ubuntu 14.04) The behavior is compiler independent. There is a bit of rearrangement going on with the move to Git and we are trying to come up with a clean process to push future changes to this interface seamlessly. With Github thankfully, this should be quite easy. Vijay On Wed, Jul 27, 2016 at 10:38 AM, wrote: > Hi > > > > How is Nek compiled with MOAB? (I?m a newbie on NEK) > > Implicit none is used extensively in the subroutines in moab.f but it seems > that a lot of the variables in the include files are declared implicit so I > get compile error no implicit type? > > If implicit none is removed then it compiles? I have a feeling I am missing > something, is there a compiler setting that should be set? (gnu compiler on > ubuntu 14.04) > > > > Best regards, > > > > Per > > > _______________________________________________ > 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 Jul 27 14:46:26 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 27 Jul 2016 14:46:26 -0500 Subject: [Nek5000-users] Compiling with MOAB - no implicit type In-Reply-To: References: Message-ID: Temporarily, can you try cherry-picking d0ef99a from my fork [1] ? Let me know if that solves the compiler errors. If not, please send the error messages so that we can fix any other pending issues. Vijay [1] https://github.com/vijaysm/Nek5000.git On Wed, Jul 27, 2016 at 2:40 PM, Vijay S. Mahadevan wrote: >> Implicit none is used extensively in the subroutines in moab.f but it seems >> that a lot of the variables in the include files are declared implicit so I >> get compile error no implicit type? > > Yes, it was originally written this way to make sure the right > variables are being set across various calls to moab.f. However, since > the bulk of the code has been verified, we could potentially remove > the "implicit none" statements and have it working cleanly. > > I also have a fix for adding the variable to NEKMOAB to remove the > compiler error. However this is in a separate fork and I can submit a > PR with the change. Ron, can you take a look at this if you have some > time now ? > >> If implicit none is removed then it compiles? I have a feeling I am missing >> something, is there a compiler setting that should be set? (gnu compiler on >> ubuntu 14.04) > > The behavior is compiler independent. There is a bit of rearrangement > going on with the move to Git and we are trying to come up with a > clean process to push future changes to this interface seamlessly. > With Github thankfully, this should be quite easy. > > Vijay > > On Wed, Jul 27, 2016 at 10:38 AM, wrote: >> Hi >> >> >> >> How is Nek compiled with MOAB? (I?m a newbie on NEK) >> >> Implicit none is used extensively in the subroutines in moab.f but it seems >> that a lot of the variables in the include files are declared implicit so I >> get compile error no implicit type? >> >> If implicit none is removed then it compiles? I have a feeling I am missing >> something, is there a compiler setting that should be set? (gnu compiler on >> ubuntu 14.04) >> >> >> >> Best regards, >> >> >> >> Per >> >> >> _______________________________________________ >> 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 Jul 28 03:09:51 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 28 Jul 2016 10:09:51 +0200 Subject: [Nek5000-users] Compiling with MOAB - no implicit type In-Reply-To: References: Message-ID: Hi Vijay Thanks, adding UPARAM takes care of the implicit variables :) In the moab example the SIZE file gives too large partiions - setting lelt=1374, lpp=4 and lelg=5496 takes care of that and makes it runnable Per Quoting nek5000-users at lists.mcs.anl.gov: > Temporarily, can you try cherry-picking d0ef99a from my fork [1] ? Let > me know if that solves the compiler errors. If not, please send the > error messages so that we can fix any other pending issues. > > Vijay > > [1] https://github.com/vijaysm/Nek5000.git > > On Wed, Jul 27, 2016 at 2:40 PM, Vijay S. Mahadevan > wrote: >>> Implicit none is used extensively in the subroutines in moab.f but it seems >>> that a lot of the variables in the include files are declared >>> implicit so I >>> get compile error no implicit type? >> >> Yes, it was originally written this way to make sure the right >> variables are being set across various calls to moab.f. However, since >> the bulk of the code has been verified, we could potentially remove >> the "implicit none" statements and have it working cleanly. >> >> I also have a fix for adding the variable to NEKMOAB to remove the >> compiler error. However this is in a separate fork and I can submit a >> PR with the change. Ron, can you take a look at this if you have some >> time now ? >> >>> If implicit none is removed then it compiles? I have a feeling I am missing >>> something, is there a compiler setting that should be set? (gnu compiler on >>> ubuntu 14.04) >> >> The behavior is compiler independent. There is a bit of rearrangement >> going on with the move to Git and we are trying to come up with a >> clean process to push future changes to this interface seamlessly. >> With Github thankfully, this should be quite easy. >> >> Vijay >> >> On Wed, Jul 27, 2016 at 10:38 AM, wrote: >>> Hi >>> >>> >>> >>> How is Nek compiled with MOAB? (I?m a newbie on NEK) >>> >>> Implicit none is used extensively in the subroutines in moab.f but it seems >>> that a lot of the variables in the include files are declared >>> implicit so I >>> get compile error no implicit type? >>> >>> If implicit none is removed then it compiles? I have a feeling I am missing >>> something, is there a compiler setting that should be set? (gnu compiler on >>> ubuntu 14.04) >>> >>> >>> >>> Best regards, >>> >>> >>> >>> Per >>> >>> >>> _______________________________________________ >>> 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 Jul 28 09:04:02 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 28 Jul 2016 14:04:02 +0000 Subject: [Nek5000-users] maketools prenek In-Reply-To: References: , Message-ID: Hello Paul, I had already tried switching BIGMEM to false but the same error appears. I am using Cygwin platform on windows to provide the linux environment and compiling on gcc 5.4.0 and gfortran compilers. Shivang -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Jul 28 22:05:36 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 29 Jul 2016 11:05:36 +0800 (GMT+08:00) Subject: [Nek5000-users] Vortex within cylinder with rotating lid AND How to import from Soldiworks to Nek5000? (nek5000-users@lists.mcs.anl.gov) In-Reply-To: References: Message-ID: Hello Dipendra, I am interested in you rotating lid-driver cylinder case. I wonder how to set the lid boundary condition in that case. Could you please give some advice? I will be very appreciated. B. L. Xu > -----????----- > ???: nek5000-users-request at lists.mcs.anl.gov > ????: 2016-07-29 01:00:12 (???) > ???: nek5000-users at lists.mcs.anl.gov > ??: > ??: Nek5000-users Digest, Vol 89, Issue 19 > > 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: Vortex within cylinder with rotating lid AND How to > import from Soldiworks to Nek5000? (nek5000-users at lists.mcs.anl.gov) > 2. Re: Compiling with MOAB - no implicit type > (nek5000-users at lists.mcs.anl.gov) > 3. Re: Compiling with MOAB - no implicit type > (nek5000-users at lists.mcs.anl.gov) > 4. Re: Compiling with MOAB - no implicit type > (nek5000-users at lists.mcs.anl.gov) > 5. maketools prenek (nek5000-users at lists.mcs.anl.gov) > > > ---------------------------------------------------------------------- > > Message: 1 > Date: Wed, 27 Jul 2016 17:04:23 +0000 > From: nek5000-users at lists.mcs.anl.gov > To: "nek5000-users at lists.mcs.anl.gov" > > Subject: Re: [Nek5000-users] Vortex within cylinder with rotating lid > AND How to import from Soldiworks to Nek5000? > Message-ID: > > Content-Type: text/plain; charset="iso-8859-1" > > > Dipendra, > > You can stretch the height of the domain with the following call in usrdat2: > > z0 = 0.0 > z1 = 5.0 ! New height > call rescale_x(zm1,z0,z1) > > ... > > There is also discussion of mesh morphing in the user manual. > > Note that this morphing effectively lowers resolution (since the number of elements > is unchanged). You can boost resolution by increasing N (lx1 in SIZE file). You might > not need to do this, however. > > If you really stretch a lot you probably should rebuild the geometry in z using a 2D mesh of > a disk, followed by n2to3 to extrude the 2D geometry to 3D. > > 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, July 27, 2016 10:01 AM > To: nek5000-users at lists.mcs.anl.gov > Subject: [Nek5000-users] Vortex within cylinder with rotating lid AND How to import from Soldiworks to Nek5000? > > > Hello all, > > I have just recently started to familiarise myself using Linux and Nek5000 so my knowledge is quite limited(please bare with me). I am currently doing a summer project proposing to use Nek5000 rather than ANSYS Fluent to simulate swirling flow to investigate vortex breakdown. I am currently going over the examples within the SVN repository I downloaded to which I stumbled upon the vortex problem within a cylinder with a rotating lid. I was interested in finding out how to change the aspect ratio of the geometry. > > > Additionally, I also wanted to confirm if its possible to import geometry from Solidworks into Nek5000? I have read that you can do it through Gambit but I am looking for some guide on how to do so. > > > Kind Regards > > Dipendra > -------------- next part -------------- > An HTML attachment was scrubbed... > URL: > > ------------------------------ > > Message: 2 > Date: Wed, 27 Jul 2016 14:40:41 -0500 > From: nek5000-users at lists.mcs.anl.gov > To: nek5000-users , Ron Rahaman > > Subject: Re: [Nek5000-users] Compiling with MOAB - no implicit type > Message-ID: > > Content-Type: text/plain; charset=UTF-8 > > > Implicit none is used extensively in the subroutines in moab.f but it seems > > that a lot of the variables in the include files are declared implicit so I > > get compile error no implicit type? > > Yes, it was originally written this way to make sure the right > variables are being set across various calls to moab.f. However, since > the bulk of the code has been verified, we could potentially remove > the "implicit none" statements and have it working cleanly. > > I also have a fix for adding the variable to NEKMOAB to remove the > compiler error. However this is in a separate fork and I can submit a > PR with the change. Ron, can you take a look at this if you have some > time now ? > > > If implicit none is removed then it compiles? I have a feeling I am missing > > something, is there a compiler setting that should be set? (gnu compiler on > > ubuntu 14.04) > > The behavior is compiler independent. There is a bit of rearrangement > going on with the move to Git and we are trying to come up with a > clean process to push future changes to this interface seamlessly. > With Github thankfully, this should be quite easy. > > Vijay > > On Wed, Jul 27, 2016 at 10:38 AM, wrote: > > Hi > > > > > > > > How is Nek compiled with MOAB? (I?m a newbie on NEK) > > > > Implicit none is used extensively in the subroutines in moab.f but it seems > > that a lot of the variables in the include files are declared implicit so I > > get compile error no implicit type? > > > > If implicit none is removed then it compiles? I have a feeling I am missing > > something, is there a compiler setting that should be set? (gnu compiler on > > ubuntu 14.04) > > > > > > > > Best regards, > > > > > > > > Per > > > > > > _______________________________________________ > > Nek5000-users mailing list > > Nek5000-users at lists.mcs.anl.gov > > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > > > ------------------------------ > > Message: 3 > Date: Wed, 27 Jul 2016 14:46:26 -0500 > From: nek5000-users at lists.mcs.anl.gov > To: nek5000-users , Ron Rahaman > > Subject: Re: [Nek5000-users] Compiling with MOAB - no implicit type > Message-ID: > > Content-Type: text/plain; charset=UTF-8 > > Temporarily, can you try cherry-picking d0ef99a from my fork [1] ? Let > me know if that solves the compiler errors. If not, please send the > error messages so that we can fix any other pending issues. > > Vijay > > [1] https://github.com/vijaysm/Nek5000.git > > On Wed, Jul 27, 2016 at 2:40 PM, Vijay S. Mahadevan wrote: > >> Implicit none is used extensively in the subroutines in moab.f but it seems > >> that a lot of the variables in the include files are declared implicit so I > >> get compile error no implicit type? > > > > Yes, it was originally written this way to make sure the right > > variables are being set across various calls to moab.f. However, since > > the bulk of the code has been verified, we could potentially remove > > the "implicit none" statements and have it working cleanly. > > > > I also have a fix for adding the variable to NEKMOAB to remove the > > compiler error. However this is in a separate fork and I can submit a > > PR with the change. Ron, can you take a look at this if you have some > > time now ? > > > >> If implicit none is removed then it compiles? I have a feeling I am missing > >> something, is there a compiler setting that should be set? (gnu compiler on > >> ubuntu 14.04) > > > > The behavior is compiler independent. There is a bit of rearrangement > > going on with the move to Git and we are trying to come up with a > > clean process to push future changes to this interface seamlessly. > > With Github thankfully, this should be quite easy. > > > > Vijay > > > > On Wed, Jul 27, 2016 at 10:38 AM, wrote: > >> Hi > >> > >> > >> > >> How is Nek compiled with MOAB? (I?m a newbie on NEK) > >> > >> Implicit none is used extensively in the subroutines in moab.f but it seems > >> that a lot of the variables in the include files are declared implicit so I > >> get compile error no implicit type? > >> > >> If implicit none is removed then it compiles? I have a feeling I am missing > >> something, is there a compiler setting that should be set? (gnu compiler on > >> ubuntu 14.04) > >> > >> > >> > >> Best regards, > >> > >> > >> > >> Per > >> > >> > >> _______________________________________________ > >> Nek5000-users mailing list > >> Nek5000-users at lists.mcs.anl.gov > >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > >> > > > ------------------------------ > > Message: 4 > Date: Thu, 28 Jul 2016 10:09:51 +0200 > From: nek5000-users at lists.mcs.anl.gov > To: nek5000-users at lists.mcs.anl.gov > Subject: Re: [Nek5000-users] Compiling with MOAB - no implicit type > Message-ID: > > Content-Type: text/plain; charset=UTF-8; DelSp="Yes"; format="flowed" > > Hi Vijay > > Thanks, adding UPARAM takes care of the implicit variables :) > In the moab example the SIZE file gives too large partiions - setting > lelt=1374, lpp=4 and lelg=5496 takes care of that and makes it runnable > > Per > > Quoting nek5000-users at lists.mcs.anl.gov: > > > Temporarily, can you try cherry-picking d0ef99a from my fork [1] ? Let > > me know if that solves the compiler errors. If not, please send the > > error messages so that we can fix any other pending issues. > > > > Vijay > > > > [1] https://github.com/vijaysm/Nek5000.git > > > > On Wed, Jul 27, 2016 at 2:40 PM, Vijay S. Mahadevan > > wrote: > >>> Implicit none is used extensively in the subroutines in moab.f but it seems > >>> that a lot of the variables in the include files are declared > >>> implicit so I > >>> get compile error no implicit type? > >> > >> Yes, it was originally written this way to make sure the right > >> variables are being set across various calls to moab.f. However, since > >> the bulk of the code has been verified, we could potentially remove > >> the "implicit none" statements and have it working cleanly. > >> > >> I also have a fix for adding the variable to NEKMOAB to remove the > >> compiler error. However this is in a separate fork and I can submit a > >> PR with the change. Ron, can you take a look at this if you have some > >> time now ? > >> > >>> If implicit none is removed then it compiles? I have a feeling I am missing > >>> something, is there a compiler setting that should be set? (gnu compiler on > >>> ubuntu 14.04) > >> > >> The behavior is compiler independent. There is a bit of rearrangement > >> going on with the move to Git and we are trying to come up with a > >> clean process to push future changes to this interface seamlessly. > >> With Github thankfully, this should be quite easy. > >> > >> Vijay > >> > >> On Wed, Jul 27, 2016 at 10:38 AM, wrote: > >>> Hi > >>> > >>> > >>> > >>> How is Nek compiled with MOAB? (I?m a newbie on NEK) > >>> > >>> Implicit none is used extensively in the subroutines in moab.f but it seems > >>> that a lot of the variables in the include files are declared > >>> implicit so I > >>> get compile error no implicit type? > >>> > >>> If implicit none is removed then it compiles? I have a feeling I am missing > >>> something, is there a compiler setting that should be set? (gnu compiler on > >>> ubuntu 14.04) > >>> > >>> > >>> > >>> Best regards, > >>> > >>> > >>> > >>> Per > >>> > >>> > >>> _______________________________________________ > >>> 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 > > > > > > > ------------------------------ > > Message: 5 > Date: Thu, 28 Jul 2016 14:04:02 +0000 > From: nek5000-users at lists.mcs.anl.gov > To: "nek5000-users at lists.mcs.anl.gov" > > Subject: [Nek5000-users] maketools prenek > Message-ID: > > Content-Type: text/plain; charset="iso-8859-1" > > Hello Paul, > > I had already tried switching BIGMEM to false but the same error appears. I am using Cygwin platform on windows to provide the linux environment and compiling on gcc 5.4.0 and gfortran compilers. > > Shivang > -------------- 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 89, Issue 19 > ********************************************* -- Xu Bolun, University of Science and Techonology of China, Hefei,Anhui,China From nek5000-users at lists.mcs.anl.gov Fri Jul 29 12:12:03 2016 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 29 Jul 2016 19:12:03 +0200 Subject: [Nek5000-users] Compiling with MOAB - no implicit type In-Reply-To: References: Message-ID: Hi Vijay When modifying the turbChannel example with with the the parameters defined in SIZE gives no implicit type error After commenting the implicit none and adding userq2 then it compiles But the following error comes when I try to run it /----------------------------------------------------------\\ | _ __ ______ __ __ ______ ____ ____ ____ | | / | / // ____// //_/ / ____/ / __ \\ / __ \\ / __ \\ | | / |/ // __/ / ,< /___ \\ / / / // / / // / / / | | / /| // /___ / /| | ____/ / / /_/ // /_/ // /_/ / | | /_/ |_//_____//_/ |_|/_____/ \\____/ \\____/ \\____/ | | | |----------------------------------------------------------| | | | NEK5000: Open Source Spectral Element Solver | | COPYRIGHT (c) 2008-2010 UCHICAGO ARGONNE, LLC | | Version: 1.0rc1 / SVN r1115 | | Web: http://nek5000.mcs.anl.gov | | | \\----------------------------------------------------------/ Number of processors: 8 REAL wdsize : 8 INTEGER wdsize : 4 Timer accuracy : 9.54E-08 Reading /home/per/nekwork/turbChannelCube/turbChannel.rea At line 86 of file /home/per/nek5000/core/connect2.f (unit = 9, file = '/home/per/nekwork/turbChannelCube/turbChannel.rea') Fortran runtime error: Bad integer for item 1 in list input Best regards, Per Quoting nek5000-users at lists.mcs.anl.gov: > Temporarily, can you try cherry-picking d0ef99a from my fork [1] ? Let > me know if that solves the compiler errors. If not, please send the > error messages so that we can fix any other pending issues. > > Vijay > > [1] https://github.com/vijaysm/Nek5000.git > > On Wed, Jul 27, 2016 at 2:40 PM, Vijay S. Mahadevan > wrote: >>> Implicit none is used extensively in the subroutines in moab.f but it seems >>> that a lot of the variables in the include files are declared >>> implicit so I >>> get compile error no implicit type? >> >> Yes, it was originally written this way to make sure the right >> variables are being set across various calls to moab.f. However, since >> the bulk of the code has been verified, we could potentially remove >> the "implicit none" statements and have it working cleanly. >> >> I also have a fix for adding the variable to NEKMOAB to remove the >> compiler error. However this is in a separate fork and I can submit a >> PR with the change. Ron, can you take a look at this if you have some >> time now ? >> >>> If implicit none is removed then it compiles? I have a feeling I am missing >>> something, is there a compiler setting that should be set? (gnu compiler on >>> ubuntu 14.04) >> >> The behavior is compiler independent. There is a bit of rearrangement >> going on with the move to Git and we are trying to come up with a >> clean process to push future changes to this interface seamlessly. >> With Github thankfully, this should be quite easy. >> >> Vijay >> >> On Wed, Jul 27, 2016 at 10:38 AM, wrote: >>> Hi >>> >>> >>> >>> How is Nek compiled with MOAB? (I?m a newbie on NEK) >>> >>> Implicit none is used extensively in the subroutines in moab.f but it seems >>> that a lot of the variables in the include files are declared >>> implicit so I >>> get compile error no implicit type? >>> >>> If implicit none is removed then it compiles? I have a feeling I am missing >>> something, is there a compiler setting that should be set? (gnu compiler on >>> ubuntu 14.04) >>> >>> >>> >>> Best regards, >>> >>> >>> >>> Per >>> >>> >>> _______________________________________________ >>> 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 > Venlig hilsen Per J?rgen J?rgensen Tlf: +45 26 22 31 06 Vind-vind ApS Langelandsvej 43, st. DK-2000 Frederiksberg