From nek5000-users at lists.mcs.anl.gov Thu Sep 2 00:38:10 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 02 Sep 2010 11:08:10 +0530 Subject: [Nek5000-users] Function to calculate volume intergral Message-ID: <4C7F3842.4030307@iitk.ac.in> Hi, Is there a function one can use in Nek that computes volume integrals. I'd like to compute the Nusselt number for Rayleigh-Benard convection (=1 + ), where Vy is the vertical velocity and <> is the volume integral. Thanks, Mani From nek5000-users at lists.mcs.anl.gov Thu Sep 2 07:26:49 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 2 Sep 2010 06:26:49 -0600 (GMT-06:00) Subject: [Nek5000-users] Function to calculate volume intergral In-Reply-To: <4C7F3842.4030307@iitk.ac.in> Message-ID: <196460858.178611283430409479.JavaMail.root@zimbra.anl.gov> Hi Mani, You can use n = nx1*ny1*nz*nelv vytvol = glsc3(vy,t,bm1,n) for the volume integral of Vy and temperature Best, Aleks ----- Original Message ----- From: nek5000-users at lists.mcs.anl.gov To: nek5000-users at lists.mcs.anl.gov Sent: Thursday, September 2, 2010 12:38:10 AM GMT -06:00 US/Canada Central Subject: [Nek5000-users] Function to calculate volume intergral Hi, Is there a function one can use in Nek that computes volume integrals. I'd like to compute the Nusselt number for Rayleigh-Benard convection (=1 + ), where Vy is the vertical velocity and <> is the volume integral. Thanks, Mani _______________________________________________ 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 Sep 2 07:31:13 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 2 Sep 2010 06:31:13 -0600 (GMT-06:00) Subject: [Nek5000-users] Function to calculate volume intergral In-Reply-To: <196460858.178611283430409479.JavaMail.root@zimbra.anl.gov> Message-ID: <1847844155.178681283430673453.JavaMail.root@zimbra.anl.gov> P.S. Mani, it should be n = nx1*ny1*nz1*nelv Aleks ----- Original Message ----- From: nek5000-users at lists.mcs.anl.gov To: nek5000-users at lists.mcs.anl.gov Sent: Thursday, September 2, 2010 7:26:49 AM GMT -06:00 US/Canada Central Subject: Re: [Nek5000-users] Function to calculate volume intergral Hi Mani, You can use n = nx1*ny1*nz*nelv vytvol = glsc3(vy,t,bm1,n) for the volume integral of Vy and temperature Best, Aleks ----- Original Message ----- From: nek5000-users at lists.mcs.anl.gov To: nek5000-users at lists.mcs.anl.gov Sent: Thursday, September 2, 2010 12:38:10 AM GMT -06:00 US/Canada Central Subject: [Nek5000-users] Function to calculate volume intergral Hi, Is there a function one can use in Nek that computes volume integrals. I'd like to compute the Nusselt number for Rayleigh-Benard convection (=1 + ), where Vy is the vertical velocity and <> is the volume integral. Thanks, Mani _______________________________________________ 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 Sep 2 07:51:55 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 02 Sep 2010 18:21:55 +0530 Subject: [Nek5000-users] [*] Re: Function to calculate volume intergral In-Reply-To: <196460858.178611283430409479.JavaMail.root@zimbra.anl.gov> References: <196460858.178611283430409479.JavaMail.root@zimbra.anl.gov> Message-ID: <4C7F9DEB.7010407@iitk.ac.in> Thanks! I tried that earlier but it was seg faulting cause I put in temperature as 'temp' and not 't'. Mani On 09/02/2010 05:56 PM, nek5000-users at lists.mcs.anl.gov wrote: > Hi Mani, > > You can use > > n = nx1*ny1*nz*nelv > vytvol = glsc3(vy,t,bm1,n) > > for the volume integral of Vy and temperature > > Best, > Aleks > > > ----- Original Message ----- > From: nek5000-users at lists.mcs.anl.gov > To: nek5000-users at lists.mcs.anl.gov > Sent: Thursday, September 2, 2010 12:38:10 AM GMT -06:00 US/Canada Central > Subject: [Nek5000-users] Function to calculate volume intergral > > Hi, > > Is there a function one can use in Nek that computes volume > integrals. I'd like to compute the Nusselt number for Rayleigh-Benard > convection (=1 +), where Vy is the vertical velocity and<> is > the volume integral. > > Thanks, > Mani > _______________________________________________ > 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 Sep 2 08:11:08 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 2 Sep 2010 07:11:08 -0600 (GMT-06:00) Subject: [Nek5000-users] [*] Re: Function to calculate volume intergral In-Reply-To: <171770668.179401283432542513.JavaMail.root@zimbra.anl.gov> Message-ID: <1003750450.179461283433068712.JavaMail.root@zimbra.anl.gov> Mani, A variable temp can be used only in the subroutines which are called with the arguments of collocation point coordinates and global element number: ix,iy,iz,ieg These routines are userf, userq, userbc and useric where temp has the following meaning (updated through NEKUSE) temp = t(ix,iy,iz,gllel(ieg)) Note that gllel(ieg) returns the local element number on a processor for a global element number ieg. Similar meaning there have ux,uy,uz and ps(1),ps(2)...,ps(ldimt), namely, velocity components and passive scalars at the point ix,iy,iz,ieg Best, Aleks ----- Original Message ----- From: nek5000-users at lists.mcs.anl.gov To: nek5000-users at lists.mcs.anl.gov Sent: Thursday, September 2, 2010 7:51:55 AM GMT -06:00 US/Canada Central Subject: Re: [Nek5000-users] [*] Re: Function to calculate volume intergral Thanks! I tried that earlier but it was seg faulting cause I put in temperature as 'temp' and not 't'. Mani On 09/02/2010 05:56 PM, nek5000-users at lists.mcs.anl.gov wrote: > Hi Mani, > > You can use > > n = nx1*ny1*nz*nelv > vytvol = glsc3(vy,t,bm1,n) > > for the volume integral of Vy and temperature > > Best, > Aleks > > > ----- Original Message ----- > From: nek5000-users at lists.mcs.anl.gov > To: nek5000-users at lists.mcs.anl.gov > Sent: Thursday, September 2, 2010 12:38:10 AM GMT -06:00 US/Canada Central > Subject: [Nek5000-users] Function to calculate volume intergral > > Hi, > > Is there a function one can use in Nek that computes volume > integrals. I'd like to compute the Nusselt number for Rayleigh-Benard > convection (=1 +), where Vy is the vertical velocity and<> is > the volume integral. > > Thanks, > Mani > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Thu Sep 2 18:13:54 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 2 Sep 2010 18:13:54 -0500 (CDT) Subject: [Nek5000-users] Grid to grid interpolation In-Reply-To: <2044462402.259521283468992293.JavaMail.root@neo-mail-3> Message-ID: <1281752463.260811283469234581.JavaMail.root@neo-mail-3> Hi Stefan, I have a question about this routine.? I haven't tried this yet, but I am curious if the "overall domain" of the new mesh needs to be exactly the same as the old mesh?? Or if you can remove a portion of the domain completely, but still use g2gi to interpolate onto the new, remaining mesh? Thanks for any info! - Michael ----- Original Message ----- From: nek5000-users at lists.mcs.anl.gov To: nek5000-users at lists.mcs.anl.gov Sent: Tuesday, August 24, 2010 1:45:24 AM GMT -06:00 US/Canada Central Subject: Re: [Nek5000-users] Grid to grid interpolation Shriram: The g2gi() routine can be used to interpolate an existing field file onto a new mesh - so it will do exactly what you want to do. For more details: http://nek5000.mcs.anl.gov/index.php/Data_processing_example Stefan On Tue, Aug 24, 2010 at 3:31 AM, < nek5000-users at lists.mcs.anl.gov > wrote: Hi, Recently there was an updated routine in nek called grid-to-grid interpolation (g2gi). I tried to understand it by grepping to source code, but couldn't make much sense out of it. Could anyone brief what it is it for ? I have a nek simulation in which I have got lots of data, but for some comparisons, would like to do a grid refinement (quad/oct from prenek) and restart from the existing field files if that is possible. I know that for h-type refinement, usually the simulation has to be started afresh. But I was wondering if g2gi would make it possible to restart from a previous simulation. Thanks Shriram _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Sep 2 21:17:43 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 2 Sep 2010 21:17:43 -0500 Subject: [Nek5000-users] Grid to grid interpolation In-Reply-To: <1281752463.260811283469234581.JavaMail.root@neo-mail-3> References: <2044462402.259521283468992293.JavaMail.root@neo-mail-3> <1281752463.260811283469234581.JavaMail.root@neo-mail-3> Message-ID: Sure you can interpolate onto a smaller mesh as well. Stefan On Thu, Sep 2, 2010 at 6:13 PM, wrote: > Hi Stefan, > > > > I have a question about this routine. I haven't tried this yet, but I am > curious if the "overall domain" > > of the new mesh needs to be exactly the same as the old mesh? Or if you > can remove a portion of > > the domain completely, but still use g2gi to interpolate onto the new, > remaining mesh? > > > > Thanks for any info! > > > > - Michael > > > ----- Original Message ----- > From: nek5000-users at lists.mcs.anl.gov > To: nek5000-users at lists.mcs.anl.gov > Sent: Tuesday, August 24, 2010 1:45:24 AM GMT -06:00 US/Canada Central > Subject: Re: [Nek5000-users] Grid to grid interpolation > > Shriram: > > The g2gi() routine can be used to interpolate an existing field file onto a > new mesh - so it will do exactly what you want to do. > For more details: > http://nek5000.mcs.anl.gov/index.php/Data_processing_example > > Stefan > > > On Tue, Aug 24, 2010 at 3:31 AM, wrote: > >> Hi, >> >> Recently there was an updated routine in nek called grid-to-grid >> interpolation (g2gi). I tried to understand it by grepping to source code, >> but couldn't make much sense out of it. Could anyone brief what it is it for >> ? >> >> I have a nek simulation in which I have got lots of data, but for some >> comparisons, would like to do a grid refinement (quad/oct from prenek) and >> restart from the existing field files if that is possible. I know that for >> h-type refinement, usually the simulation has to be started afresh. But I >> was wondering if g2gi would make it possible to restart from a previous >> simulation. >> >> Thanks >> Shriram >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> >> > > _______________________________________________ Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Fri Sep 3 15:01:06 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 3 Sep 2010 15:01:06 -0500 (CDT) Subject: [Nek5000-users] Grid to grid interpolation In-Reply-To: <1281752463.260811283469234581.JavaMail.root@neo-mail-3> References: <1281752463.260811283469234581.JavaMail.root@neo-mail-3> Message-ID: Hi Stefan, I have a question about the grid to grid interpolation. Does it work for both binary file formats, *.fld01 and *0.f00001? I use blah.fld* format more. Thanks, Harish. On Thu, 2 Sep 2010 nek5000-users at lists.mcs.anl.gov wrote: > > > Hi Stefan, > > > > I have a question about this routine.?? I haven't tried this yet, but I am curious if the "overall domain" > > of the new mesh needs to be exactly the same as the old mesh??? Or if you can remove a portion of > > the domain completely, but still use g2gi to interpolate onto the new, remaining mesh? > > > > Thanks for any info! > > > > - Michael > > > ----- Original Message ----- > From: nek5000-users at lists.mcs.anl.gov > To: nek5000-users at lists.mcs.anl.gov > Sent: Tuesday, August 24, 2010 1:45:24 AM GMT -06:00 US/Canada Central > Subject: Re: [Nek5000-users] Grid to grid interpolation > > > Shriram: > > The g2gi() routine can be used to interpolate an existing field file onto a new mesh - so it will do exactly what you want to do. > For more details: http://nek5000.mcs.anl.gov/index.php/Data_processing_example > > > > Stefan > > > > On Tue, Aug 24, 2010 at 3:31 AM, < nek5000-users at lists.mcs.anl.gov > wrote: > > > > Hi, > > > Recently there was an updated routine in nek called grid-to-grid interpolation (g2gi). I tried to understand it by grepping to source code, but couldn't make much sense out of it. Could anyone brief what it is it for ? > > > I have a nek simulation in which I have got lots of data, but for some comparisons, would like to do a grid refinement (quad/oct from prenek) and restart from the existing field files if that is possible. I know that for h-type refinement, usually the simulation has to be started afresh. But I was wondering if g2gi would make it possible to restart from a previous simulation. > > > Thanks > Shriram > > _______________________________________________ > 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 Sep 3 15:03:37 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 3 Sep 2010 15:03:37 -0500 Subject: [Nek5000-users] Grid to grid interpolation In-Reply-To: References: <1281752463.260811283469234581.JavaMail.root@neo-mail-3> Message-ID: No only for the new binary format (.f????). Stefan On Fri, Sep 3, 2010 at 3:01 PM, wrote: > Hi Stefan, > > I have a question about the grid to grid interpolation. > > Does it work for both binary file formats, *.fld01 and *0.f00001? > > I use blah.fld* format more. > > Thanks, > > Harish. > > On Thu, 2 Sep 2010 nek5000-users at lists.mcs.anl.gov wrote: > > > > > > > Hi Stefan, > > > > > > > > I have a question about this routine. I haven't tried this yet, but I am > curious if the "overall domain" > > > > of the new mesh needs to be exactly the same as the old mesh? Or if you > can remove a portion of > > > > the domain completely, but still use g2gi to interpolate onto the new, > remaining mesh? > > > > > > > > Thanks for any info! > > > > > > > > - Michael > > > > > > ----- Original Message ----- > > From: nek5000-users at lists.mcs.anl.gov > > To: nek5000-users at lists.mcs.anl.gov > > Sent: Tuesday, August 24, 2010 1:45:24 AM GMT -06:00 US/Canada Central > > Subject: Re: [Nek5000-users] Grid to grid interpolation > > > > > > Shriram: > > > > The g2gi() routine can be used to interpolate an existing field file onto > a new mesh - so it will do exactly what you want to do. > > For more details: > http://nek5000.mcs.anl.gov/index.php/Data_processing_example > > > > > > > > Stefan > > > > > > > > On Tue, Aug 24, 2010 at 3:31 AM, < nek5000-users at lists.mcs.anl.gov > > wrote: > > > > > > > > Hi, > > > > > > Recently there was an updated routine in nek called grid-to-grid > interpolation (g2gi). I tried to understand it by grepping to source code, > but couldn't make much sense out of it. Could anyone brief what it is it for > ? > > > > > > I have a nek simulation in which I have got lots of data, but for some > comparisons, would like to do a grid refinement (quad/oct from prenek) and > restart from the existing field files if that is possible. I know that for > h-type refinement, usually the simulation has to be started afresh. But I > was wondering if g2gi would make it possible to restart from a previous > simulation. > > > > > > Thanks > > Shriram > > > > _______________________________________________ > > Nek5000-users mailing list > > Nek5000-users at lists.mcs.anl.gov > > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > > > > > > _______________________________________________ Nek5000-users mailing > list Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Fri Sep 3 16:01:00 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 3 Sep 2010 16:01:00 -0500 (CDT) Subject: [Nek5000-users] Grid to grid interpolation In-Reply-To: References: <1281752463.260811283469234581.JavaMail.root@neo-mail-3> Message-ID: Thanks Stefan!! Harish On Fri, 3 Sep 2010 nek5000-users at lists.mcs.anl.gov wrote: > No only for the new binary format (.f????). > Stefan > > On Fri, Sep 3, 2010 at 3:01 PM, wrote: > > > Hi Stefan, > > > > I have a question about the grid to grid interpolation. > > > > Does it work for both binary file formats, *.fld01 and *0.f00001? > > > > I use blah.fld* format more. > > > > Thanks, > > > > Harish. > > > > On Thu, 2 Sep 2010 nek5000-users at lists.mcs.anl.gov wrote: > > > > > > > > > > > Hi Stefan, > > > > > > > > > > > > I have a question about this routine. I haven't tried this yet, but I am > > curious if the "overall domain" > > > > > > of the new mesh needs to be exactly the same as the old mesh? Or if you > > can remove a portion of > > > > > > the domain completely, but still use g2gi to interpolate onto the new, > > remaining mesh? > > > > > > > > > > > > Thanks for any info! > > > > > > > > > > > > - Michael > > > > > > > > > ----- Original Message ----- > > > From: nek5000-users at lists.mcs.anl.gov > > > To: nek5000-users at lists.mcs.anl.gov > > > Sent: Tuesday, August 24, 2010 1:45:24 AM GMT -06:00 US/Canada Central > > > Subject: Re: [Nek5000-users] Grid to grid interpolation > > > > > > > > > Shriram: > > > > > > The g2gi() routine can be used to interpolate an existing field file onto > > a new mesh - so it will do exactly what you want to do. > > > For more details: > > http://nek5000.mcs.anl.gov/index.php/Data_processing_example > > > > > > > > > > > > Stefan > > > > > > > > > > > > On Tue, Aug 24, 2010 at 3:31 AM, < nek5000-users at lists.mcs.anl.gov > > > wrote: > > > > > > > > > > > > Hi, > > > > > > > > > Recently there was an updated routine in nek called grid-to-grid > > interpolation (g2gi). I tried to understand it by grepping to source code, > > but couldn't make much sense out of it. Could anyone brief what it is it for > > ? > > > > > > > > > I have a nek simulation in which I have got lots of data, but for some > > comparisons, would like to do a grid refinement (quad/oct from prenek) and > > restart from the existing field files if that is possible. I know that for > > h-type refinement, usually the simulation has to be started afresh. But I > > was wondering if g2gi would make it possible to restart from a previous > > simulation. > > > > > > > > > Thanks > > > Shriram > > > > > > _______________________________________________ > > > Nek5000-users mailing list > > > Nek5000-users at lists.mcs.anl.gov > > > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > > > > > > > > > > _______________________________________________ Nek5000-users mailing > > list Nek5000-users at lists.mcs.anl.gov > > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > > _______________________________________________ > > Nek5000-users mailing list > > Nek5000-users at lists.mcs.anl.gov > > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > > > From nek5000-users at lists.mcs.anl.gov Mon Sep 6 07:52:39 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 6 Sep 2010 07:52:39 -0500 Subject: [Nek5000-users] "byte swap" + grid to grid subroutine In-Reply-To: References: <1281752463.260811283469234581.JavaMail.root@neo-mail-3> Message-ID: Hello, I am testing subroutine g2gi() for a case of backward facing step (BFS) field file. After starting Nek5k in post-processing mode, the code stops in the subroutine g2gi() while reading the old field file. Nek5k is compiled with GNU compiler and OpenMPI. Here is the code snippet from the userchk() subroutine. *********************************************************************** subroutine userchk include 'SIZE' include 'TOTAL' character*132 newfld, oldfld, newgfld data newfld, oldfld, newgfld /'new0.f00001','bfs10.f00001', $ 'bfs20.f00001'/ call g2gi(newfld,oldfld,newgfld) ! grid2grid interpolation call exitt() *********************************************************************** Here is the part of the logfile which shows the point at which the simulation hangs and I have to kill the job after this point. *********************************************************************** nsteps=0 -> skip time loop running solver in post processing mode call userchk grid-to-grid interpolation set initial conditions Checking restart options: bfs10.f00001 Reading checkpoint data 1 OPEN: bfs10.f00001 byte swap: F 6.5432100 -2.93127722E+35 *********************************************************************** I am attaching the logfile for you reference. What is the solution to this problem? Thanks for all the help, Harish. -------------- next part -------------- A non-text attachment was scrubbed... Name: logfile Type: application/octet-stream Size: 6611 bytes Desc: not available URL: From nek5000-users at lists.mcs.anl.gov Mon Sep 6 08:33:39 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 6 Sep 2010 08:33:39 -0500 Subject: [Nek5000-users] "byte swap" + grid to grid subroutine In-Reply-To: References: <1281752463.260811283469234581.JavaMail.root@neo-mail-3> Message-ID: Harish, I will check into that. Stefan On Mon, Sep 6, 2010 at 7:52 AM, wrote: > Hello, > > I am testing subroutine g2gi() for a case of backward facing step (BFS) > field file. After starting Nek5k in post-processing mode, the code stops > in the subroutine g2gi() while reading the old field file. > > Nek5k is compiled with GNU compiler and OpenMPI. Here is the code snippet > from the userchk() subroutine. > *********************************************************************** > subroutine userchk > include 'SIZE' > include 'TOTAL' > > character*132 newfld, oldfld, newgfld > data newfld, oldfld, newgfld /'new0.f00001','bfs10.f00001', > $ 'bfs20.f00001'/ > > call g2gi(newfld,oldfld,newgfld) ! grid2grid interpolation > call exitt() > *********************************************************************** > > Here is the part of the logfile which shows the point at which the > simulation hangs and I have to kill the job after this point. > > *********************************************************************** > nsteps=0 -> skip time loop > running solver in post processing mode > > call userchk > grid-to-grid interpolation > set initial conditions > Checking restart options: bfs10.f00001 > > Reading checkpoint data > 1 OPEN: bfs10.f00001 > byte swap: F 6.5432100 -2.93127722E+35 > *********************************************************************** > > I am attaching the logfile for you reference. What is the solution to this > problem? > > Thanks for all the help, > > Harish. > _______________________________________________ > 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 Sep 6 08:39:42 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 6 Sep 2010 08:39:42 -0500 (CDT) Subject: [Nek5000-users] "byte swap" + grid to grid subroutine In-Reply-To: References: <1281752463.260811283469234581.JavaMail.root@neo-mail-3> Message-ID: Thanks Stefan!! Harish On Mon, 6 Sep 2010 nek5000-users at lists.mcs.anl.gov wrote: > Harish, > > I will check into that. > > Stefan > > On Mon, Sep 6, 2010 at 7:52 AM, wrote: > > > Hello, > > > > I am testing subroutine g2gi() for a case of backward facing step (BFS) > > field file. After starting Nek5k in post-processing mode, the code stops > > in the subroutine g2gi() while reading the old field file. > > > > Nek5k is compiled with GNU compiler and OpenMPI. Here is the code snippet > > from the userchk() subroutine. > > *********************************************************************** > > subroutine userchk > > include 'SIZE' > > include 'TOTAL' > > > > character*132 newfld, oldfld, newgfld > > data newfld, oldfld, newgfld /'new0.f00001','bfs10.f00001', > > $ 'bfs20.f00001'/ > > > > call g2gi(newfld,oldfld,newgfld) ! grid2grid interpolation > > call exitt() > > *********************************************************************** > > > > Here is the part of the logfile which shows the point at which the > > simulation hangs and I have to kill the job after this point. > > > > *********************************************************************** > > nsteps=0 -> skip time loop > > running solver in post processing mode > > > > call userchk > > grid-to-grid interpolation > > set initial conditions > > Checking restart options: bfs10.f00001 > > > > Reading checkpoint data > > 1 OPEN: bfs10.f00001 > > byte swap: F 6.5432100 -2.93127722E+35 > > *********************************************************************** > > > > I am attaching the logfile for you reference. What is the solution to this > > problem? > > > > Thanks for all the help, > > > > Harish. > > _______________________________________________ > > Nek5000-users mailing list > > Nek5000-users at lists.mcs.anl.gov > > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > > > From nek5000-users at lists.mcs.anl.gov Mon Sep 6 16:47:37 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 6 Sep 2010 16:47:37 -0500 Subject: [Nek5000-users] "byte swap" + grid to grid subroutine In-Reply-To: References: <1281752463.260811283469234581.JavaMail.root@neo-mail-3> Message-ID: Harish: Can you send me your case? I cannot reproduce your problem here. -Stefan On Mon, Sep 6, 2010 at 8:39 AM, wrote: > Thanks Stefan!! > > Harish > > On Mon, 6 Sep 2010 nek5000-users at lists.mcs.anl.gov wrote: > > > Harish, > > > > I will check into that. > > > > Stefan > > > > On Mon, Sep 6, 2010 at 7:52 AM, wrote: > > > > > Hello, > > > > > > I am testing subroutine g2gi() for a case of backward facing step (BFS) > > > field file. After starting Nek5k in post-processing mode, the code > stops > > > in the subroutine g2gi() while reading the old field file. > > > > > > Nek5k is compiled with GNU compiler and OpenMPI. Here is the code > snippet > > > from the userchk() subroutine. > > > *********************************************************************** > > > subroutine userchk > > > include 'SIZE' > > > include 'TOTAL' > > > > > > character*132 newfld, oldfld, newgfld > > > data newfld, oldfld, newgfld /'new0.f00001','bfs10.f00001', > > > $ 'bfs20.f00001'/ > > > > > > call g2gi(newfld,oldfld,newgfld) ! grid2grid interpolation > > > call exitt() > > > *********************************************************************** > > > > > > Here is the part of the logfile which shows the point at which the > > > simulation hangs and I have to kill the job after this point. > > > > > > *********************************************************************** > > > nsteps=0 -> skip time loop > > > running solver in post processing mode > > > > > > call userchk > > > grid-to-grid interpolation > > > set initial conditions > > > Checking restart options: bfs10.f00001 > > > > > > Reading checkpoint data > > > 1 OPEN: bfs10.f00001 > > > byte swap: F 6.5432100 -2.93127722E+35 > > > *********************************************************************** > > > > > > I am attaching the logfile for you reference. What is the solution to > this > > > problem? > > > > > > Thanks for all the help, > > > > > > Harish. > > > _______________________________________________ > > > 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 Sep 6 18:22:26 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 6 Sep 2010 18:22:26 -0500 Subject: [Nek5000-users] "byte swap" + grid to grid subroutine In-Reply-To: References: <1281752463.260811283469234581.JavaMail.root@neo-mail-3> Message-ID: <6801f02f734d7c93cea626945a75deac.squirrel@webmail.uic.edu> Hi Stefan, Thanks a lot for looking into this issue. Here is the link with bfs.tar file containing *.rea, *.usr, SIZE, old field file (bfs10.f00001) and new geometry file (bfs20.f00001). www2.uic.edu/~hkanch1/bfs.tar I actually converted a bfs1.fld20 file to bfs10.f00001. I use *.fld format because, my Visit 1.12.2 on Windows does not work with *.f???? format files. I can only see the mesh and not the velocity contours. Thanks, Harish. On Mon, September 6, 2010 4:47 pm, nek5000-users at lists.mcs.anl.gov wrote: > Harish: > > Can you send me your case? I cannot reproduce your problem here. > > -Stefan > > On Mon, Sep 6, 2010 at 8:39 AM, wrote: > >> Thanks Stefan!! >> >> Harish >> >> On Mon, 6 Sep 2010 nek5000-users at lists.mcs.anl.gov wrote: >> >> > Harish, >> > >> > I will check into that. >> > >> > Stefan >> > >> > On Mon, Sep 6, 2010 at 7:52 AM, >> wrote: >> > >> > > Hello, >> > > >> > > I am testing subroutine g2gi() for a case of backward facing step >> (BFS) >> > > field file. After starting Nek5k in post-processing mode, the code >> stops >> > > in the subroutine g2gi() while reading the old field file. >> > > >> > > Nek5k is compiled with GNU compiler and OpenMPI. Here is the code >> snippet >> > > from the userchk() subroutine. >> > > *********************************************************************** >> > > subroutine userchk >> > > include 'SIZE' >> > > include 'TOTAL' >> > > >> > > character*132 newfld, oldfld, newgfld >> > > data newfld, oldfld, newgfld /'new0.f00001','bfs10.f00001', >> > > $ 'bfs20.f00001'/ >> > > >> > > call g2gi(newfld,oldfld,newgfld) ! grid2grid interpolation >> > > call exitt() >> > > *********************************************************************** >> > > >> > > Here is the part of the logfile which shows the point at which the >> > > simulation hangs and I have to kill the job after this point. >> > > >> > > *********************************************************************** >> > > nsteps=0 -> skip time loop >> > > running solver in post processing mode >> > > >> > > call userchk >> > > grid-to-grid interpolation >> > > set initial conditions >> > > Checking restart options: bfs10.f00001 >> > > >> > > Reading checkpoint data >> > > 1 OPEN: bfs10.f00001 >> > > byte swap: F 6.5432100 -2.93127722E+35 >> > > *********************************************************************** >> > > >> > > I am attaching the logfile for you reference. What is the solution >> to >> this >> > > problem? >> > > >> > > Thanks for all the help, >> > > >> > > Harish. >> > > _______________________________________________ >> > > Nek5000-users mailing list >> > > Nek5000-users at lists.mcs.anl.gov >> > > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> > > >> > > >> > >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > From nek5000-users at lists.mcs.anl.gov Tue Sep 7 11:00:22 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 7 Sep 2010 10:00:22 -0600 (GMT-06:00) Subject: [Nek5000-users] "byte swap" + grid to grid subroutine In-Reply-To: <1742064787.423741283875022399.JavaMail.root@zimbra.anl.gov> Message-ID: <472313362.424031283875222081.JavaMail.root@zimbra.anl.gov> Harish: I think you mixed up the old field file (oldfld) and the fld file containing the new geometry (newgfld). call g2gi(newfld, oldfld, newgfld) ! grid2grid interpolation Note: You need to run your old case (oldfld.rea, oldfld.map) to interpolate oldfld onto the newgfld mesh. The output of this operation results in a new field file (newfld). hth, Stefan ----- Original Message ----- From: nek5000-users at lists.mcs.anl.gov To: nek5000-users at lists.mcs.anl.gov Sent: Monday, September 6, 2010 6:22:26 PM GMT -06:00 US/Canada Central Subject: Re: [Nek5000-users] "byte swap" + grid to grid subroutine Hi Stefan, Thanks a lot for looking into this issue. Here is the link with bfs.tar file containing *.rea, *.usr, SIZE, old field file (bfs10.f00001) and new geometry file (bfs20.f00001). www2.uic.edu/~hkanch1/bfs.tar I actually converted a bfs1.fld20 file to bfs10.f00001. I use *.fld format because, my Visit 1.12.2 on Windows does not work with *.f???? format files. I can only see the mesh and not the velocity contours. Thanks, Harish. On Mon, September 6, 2010 4:47 pm, nek5000-users at lists.mcs.anl.gov wrote: > Harish: > > Can you send me your case? I cannot reproduce your problem here. > > -Stefan > > On Mon, Sep 6, 2010 at 8:39 AM, wrote: > >> Thanks Stefan!! >> >> Harish >> >> On Mon, 6 Sep 2010 nek5000-users at lists.mcs.anl.gov wrote: >> >> > Harish, >> > >> > I will check into that. >> > >> > Stefan >> > >> > On Mon, Sep 6, 2010 at 7:52 AM, >> wrote: >> > >> > > Hello, >> > > >> > > I am testing subroutine g2gi() for a case of backward facing step >> (BFS) >> > > field file. After starting Nek5k in post-processing mode, the code >> stops >> > > in the subroutine g2gi() while reading the old field file. >> > > >> > > Nek5k is compiled with GNU compiler and OpenMPI. Here is the code >> snippet >> > > from the userchk() subroutine. >> > > *********************************************************************** >> > > subroutine userchk >> > > include 'SIZE' >> > > include 'TOTAL' >> > > >> > > character*132 newfld, oldfld, newgfld >> > > data newfld, oldfld, newgfld /'new0.f00001','bfs10.f00001', >> > > $ 'bfs20.f00001'/ >> > > >> > > call g2gi(newfld,oldfld,newgfld) ! grid2grid interpolation >> > > call exitt() >> > > *********************************************************************** >> > > >> > > Here is the part of the logfile which shows the point at which the >> > > simulation hangs and I have to kill the job after this point. >> > > >> > > *********************************************************************** >> > > nsteps=0 -> skip time loop >> > > running solver in post processing mode >> > > >> > > call userchk >> > > grid-to-grid interpolation >> > > set initial conditions >> > > Checking restart options: bfs10.f00001 >> > > >> > > Reading checkpoint data >> > > 1 OPEN: bfs10.f00001 >> > > byte swap: F 6.5432100 -2.93127722E+35 >> > > *********************************************************************** >> > > >> > > I am attaching the logfile for you reference. What is the solution >> to >> this >> > > problem? >> > > >> > > Thanks for all the help, >> > > >> > > Harish. >> > > _______________________________________________ >> > > Nek5000-users mailing list >> > > Nek5000-users at lists.mcs.anl.gov >> > > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> > > >> > > >> > >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Tue Sep 7 12:06:46 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 7 Sep 2010 12:06:46 -0500 (CDT) Subject: [Nek5000-users] "byte swap" + grid to grid subroutine In-Reply-To: <472313362.424031283875222081.JavaMail.root@zimbra.anl.gov> References: <472313362.424031283875222081.JavaMail.root@zimbra.anl.gov> Message-ID: Hi Stefan, Thanks for your help. I tested the grid to grid interpolation routine with the suggestions that you gave and it worked!! I guess I was confused about the last 2 statements from the Wiki page, # run nek using the new geometry (e.g. new_geom.f0000) # run nek using the old geometry and add this code snipplet to userchk() Now I see what these 2 statements mean. Regards, Harish. On Tue, 7 Sep 2010 nek5000-users at lists.mcs.anl.gov wrote: > Harish: > > I think you mixed up the old field file (oldfld) and the fld file containing the new geometry (newgfld). > > call g2gi(newfld, oldfld, newgfld) ! grid2grid interpolation > > Note: You need to run your old case (oldfld.rea, oldfld.map) to interpolate oldfld onto the newgfld mesh. > The output of this operation results in a new field file (newfld). > > hth, > Stefan > > ----- Original Message ----- > From: nek5000-users at lists.mcs.anl.gov > To: nek5000-users at lists.mcs.anl.gov > Sent: Monday, September 6, 2010 6:22:26 PM GMT -06:00 US/Canada Central > Subject: Re: [Nek5000-users] "byte swap" + grid to grid subroutine > > Hi Stefan, > > Thanks a lot for looking into this issue. > > Here is the link with bfs.tar file containing *.rea, *.usr, SIZE, old > field file (bfs10.f00001) and new geometry file (bfs20.f00001). > > www2.uic.edu/~hkanch1/bfs.tar > > I actually converted a bfs1.fld20 file to bfs10.f00001. I use *.fld format > because, my Visit 1.12.2 on Windows does not work with *.f???? format > files. I can only see the mesh and not the velocity contours. > > Thanks, > > Harish. > > > On Mon, September 6, 2010 4:47 pm, nek5000-users at lists.mcs.anl.gov wrote: > > Harish: > > > > Can you send me your case? I cannot reproduce your problem here. > > > > -Stefan > > > > On Mon, Sep 6, 2010 at 8:39 AM, wrote: > > > >> Thanks Stefan!! > >> > >> Harish > >> > >> On Mon, 6 Sep 2010 nek5000-users at lists.mcs.anl.gov wrote: > >> > >> > Harish, > >> > > >> > I will check into that. > >> > > >> > Stefan > >> > > >> > On Mon, Sep 6, 2010 at 7:52 AM, > >> wrote: > >> > > >> > > Hello, > >> > > > >> > > I am testing subroutine g2gi() for a case of backward facing step > >> (BFS) > >> > > field file. After starting Nek5k in post-processing mode, the code > >> stops > >> > > in the subroutine g2gi() while reading the old field file. > >> > > > >> > > Nek5k is compiled with GNU compiler and OpenMPI. Here is the code > >> snippet > >> > > from the userchk() subroutine. > >> > > *********************************************************************** > >> > > subroutine userchk > >> > > include 'SIZE' > >> > > include 'TOTAL' > >> > > > >> > > character*132 newfld, oldfld, newgfld > >> > > data newfld, oldfld, newgfld /'new0.f00001','bfs10.f00001', > >> > > $ 'bfs20.f00001'/ > >> > > > >> > > call g2gi(newfld,oldfld,newgfld) ! grid2grid interpolation > >> > > call exitt() > >> > > *********************************************************************** > >> > > > >> > > Here is the part of the logfile which shows the point at which the > >> > > simulation hangs and I have to kill the job after this point. > >> > > > >> > > *********************************************************************** > >> > > nsteps=0 -> skip time loop > >> > > running solver in post processing mode > >> > > > >> > > call userchk > >> > > grid-to-grid interpolation > >> > > set initial conditions > >> > > Checking restart options: bfs10.f00001 > >> > > > >> > > Reading checkpoint data > >> > > 1 OPEN: bfs10.f00001 > >> > > byte swap: F 6.5432100 -2.93127722E+35 > >> > > *********************************************************************** > >> > > > >> > > I am attaching the logfile for you reference. What is the solution > >> to > >> this > >> > > problem? > >> > > > >> > > Thanks for all the help, > >> > > > >> > > Harish. > >> > > _______________________________________________ > >> > > Nek5000-users mailing list > >> > > Nek5000-users at lists.mcs.anl.gov > >> > > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > >> > > > >> > > > >> > > >> _______________________________________________ > >> Nek5000-users mailing list > >> Nek5000-users at lists.mcs.anl.gov > >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > >> > > _______________________________________________ > > Nek5000-users mailing list > > Nek5000-users at lists.mcs.anl.gov > > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > > > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > From nek5000-users at lists.mcs.anl.gov Wed Sep 8 18:34:30 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 09 Sep 2010 01:34:30 +0200 Subject: [Nek5000-users] two phase flow Message-ID: <1283988870.19733.77.camel@localhost.localdomain> Hello all, Is there anyone out there solving two-phase flows? I am interested in understanding how to add a boundary condition at the interface that depends on the temperature gradient along the interface. Cheers, Frank -- Frank Herbert Muldoon, Ph.D. Mechanical Engineering Technische Universit?t Wien (Vienna Technical University) Inst. f. Str?mungsmechanik und W?rme?bertragung (Institute of Fluid Mechanics and Heat Transfer) Resselgasse 3 1040 Wien Tel: +4315880132232 Fax: +4315880132299 Cell:+436765203470 fmuldoo (skype) http://tetra.fluid.tuwien.ac.at/fmuldoo/public_html/webpage/frank-muldoon.html From nek5000-users at lists.mcs.anl.gov Thu Sep 9 19:03:23 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 9 Sep 2010 19:03:23 -0500 Subject: [Nek5000-users] Hpts output & lambda2 Message-ID: Hi, I am trying to compute lambda2 vortex just like how it is done in the turbchannel example. But it seems like that it messes up my output of hpts. The values of pressure are not written and I suppose instead of pressure the t(1,1,1,1,1) or t(1,1,1,1,2) is written. I tried setting the ifto and ifpsco value to false but it doesn't seem to work. Any thoughts on where I am going wrong ? if(mod(istep,iostep).eq.0 .and. istep.gt.0) then call lambda2(t(1,1,1,1,1)) ifto=.true. if(ldimt.gt.1) call comp_vort3(t(1,1,1,1,2),wo1,wo2,vx,vy,vz) ifpsco(1)=.true. endif ifto=.false. ifpo=.true. ifpsco(1)=.false. if(istep.gt.0) call hpts() Thanks Shriram -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Sep 9 19:27:59 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 9 Sep 2010 19:27:59 -0500 (CDT) Subject: [Nek5000-users] Hpts output & lambda2 In-Reply-To: References: Message-ID: Check ldimt/ldimt1 in SIZE ? Paul On Thu, 9 Sep 2010, nek5000-users at lists.mcs.anl.gov wrote: > Hi, > > I am trying to compute lambda2 vortex just like how it is done in the > turbchannel example. But it seems like that it messes up my output of hpts. > The values of pressure are not written and I suppose instead of pressure the > t(1,1,1,1,1) or t(1,1,1,1,2) is written. I tried setting the ifto and ifpsco > value to false but it doesn't seem to work. Any thoughts on where I am going > wrong ? > > if(mod(istep,iostep).eq.0 .and. istep.gt.0) then > call lambda2(t(1,1,1,1,1)) > ifto=.true. > if(ldimt.gt.1) call comp_vort3(t(1,1,1,1,2),wo1,wo2,vx,vy,vz) > ifpsco(1)=.true. > endif > > ifto=.false. > ifpo=.true. > ifpsco(1)=.false. > if(istep.gt.0) call hpts() > > Thanks > Shriram > From nek5000-users at lists.mcs.anl.gov Thu Sep 9 20:52:40 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 9 Sep 2010 20:52:40 -0500 Subject: [Nek5000-users] Hpts output & lambda2 In-Reply-To: References: Message-ID: Paul, My ldimt is 3 and the default values are used for the other parameters : ldimt1 = ldimt+1; ldimt3=ldimt+3 . . Regards Shriram -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Sep 9 21:07:12 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 9 Sep 2010 21:07:12 -0500 (CDT) Subject: [Nek5000-users] Hpts output & lambda2 In-Reply-To: References: Message-ID: Are wo1 and wo2 properly declared in the calling routine ? Paul On Thu, 9 Sep 2010, nek5000-users at lists.mcs.anl.gov wrote: > Hi, > > I am trying to compute lambda2 vortex just like how it is done in the > turbchannel example. But it seems like that it messes up my output of hpts. > The values of pressure are not written and I suppose instead of pressure the > t(1,1,1,1,1) or t(1,1,1,1,2) is written. I tried setting the ifto and ifpsco > value to false but it doesn't seem to work. Any thoughts on where I am going > wrong ? > > if(mod(istep,iostep).eq.0 .and. istep.gt.0) then > call lambda2(t(1,1,1,1,1)) > ifto=.true. > if(ldimt.gt.1) call comp_vort3(t(1,1,1,1,2),wo1,wo2,vx,vy,vz) > ifpsco(1)=.true. > endif > > ifto=.false. > ifpo=.true. > ifpsco(1)=.false. > if(istep.gt.0) call hpts() > > Thanks > Shriram > From nek5000-users at lists.mcs.anl.gov Fri Sep 10 09:59:35 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 10 Sep 2010 09:59:35 -0500 Subject: [Nek5000-users] Hpts output & lambda2 In-Reply-To: References: Message-ID: Hi Paul, Yes . .. This is how its declared. common /gaaa/ wo1(lx1,ly1,lz1,lelv) & , wo2(lx1,ly1,lz1,lelv) & , wo3(lx1,ly1,lz1,lelv) Regards Shriram -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Fri Sep 10 23:37:56 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 10 Sep 2010 23:37:56 -0500 Subject: [Nek5000-users] Hpts output & lambda2 In-Reply-To: References: Message-ID: Hi Paul, If I have it this way, the hpts.out has pressure data for istep=0 but after that my pressure values are not written. call hpts() ifpsco(1) = .true. ntot1 = nx1*ny1*nz1*nelv if(mod(istep,iostep).eq.0 .and. istep.gt.0) then call lambda2(t(1,1,1,1,1)) ifto=.true. if(ldimt.gt.1) call comp_vort3(t(1,1,1,1,2),wo1,wo2,vx,vy,vz) endif It looks like using the temperature field and passive scalar has messed up the o/p in hpts. I require the pressure values but not the passive scalars(however it would be nice to have it). Is there a way to force hpts not to o/p any passive scalar ? Regards Shriram -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Tue Sep 14 11:25:45 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 14 Sep 2010 10:25:45 -0600 Subject: [Nek5000-users] element order range Message-ID: Hello All. I am doing some tests of Nek5000 against a low-order code. Under "Performance tips", it is recommended to "design your resolution (mesh) for N=7 or N=9" Are there any limitations on the range of values for N? For example, what is the smallest N and largest N that the code can/has been run with? What are the limitations with running at, say, N = 16? Thanks. --Mike From nek5000-users at lists.mcs.anl.gov Tue Sep 14 11:33:32 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 14 Sep 2010 11:33:32 -0500 (CDT) Subject: [Nek5000-users] element order range In-Reply-To: References: Message-ID: Hi Mike, I've run with N=120 in the past and just this past week was running w/ N=64. (I had to bump up a couple of parameters past the 40 or 50 mark to do so.) Stefan has run the Pn-Pn variant with N=1 (lx1=2). lx1=6-12 is the general sweet spot for the code because of the way the operators are evaluated... When comparing to a low-order code it's generally best to compare for an equal number of gridpoints - i.e., roughly the same resolution. The main reason for this is that higher order does not buy you increased resolution. (The Nyquist sampling theorem dictates at least 2*k points are required to resolve a signal of wavenumber k.) What the high-order method gains is improved accuracy for the modes that _are_ resolved. My goal is to try to ensure that the performance is comparable to a low-order code - i.e., that costs are not inordinate w/ N. What type of comparison did you have in mind ? You might be interested in: www.mcs.anl.gov/~fischer/users.pdf which is a work-in-progress. Paul On Tue, 14 Sep 2010, nek5000-users at lists.mcs.anl.gov wrote: > Hello All. > > I am doing some tests of Nek5000 against a low-order code. Under "Performance tips", it is recommended to "design your resolution (mesh) for N=7 or N=9" > > Are there any limitations on the range of values for N? For example, what is the smallest N and largest N that the code can/has been run with? What are the limitations with running at, say, N = 16? > > Thanks. > --Mike > > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > From nek5000-users at lists.mcs.anl.gov Tue Sep 14 12:31:40 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 14 Sep 2010 11:31:40 -0600 Subject: [Nek5000-users] element order range In-Reply-To: References: Message-ID: <623CB443-D204-4360-80A0-C879DE8C3328@nrel.gov> Paul, Thanks for that info and for the document. Both are very helpful. There's interest here in using OpenFOAM (second-order finite-volume), and I'm interested to see how Nek does in a head to head comparison. We're using turbulent planar Couette flow as our comparison test case with Re = 8000 (See, e.g. Sullivan et al. (JFM 404, 2000). We're looking at accuracy for a given number of grid points and scalability over 16-1024 cores. I'll let you know how things turn out with the comparison. --Mike On Sep 14, 2010, at 10:33 AM, wrote: > > Hi Mike, > > I've run with N=120 in the past and just this past > week was running w/ N=64. (I had to bump up a couple > of parameters past the 40 or 50 mark to do so.) > > Stefan has run the Pn-Pn variant with N=1 (lx1=2). > > lx1=6-12 is the general sweet spot for the code because > of the way the operators are evaluated... > > When comparing to a low-order code it's generally best > to compare for an equal number of gridpoints - i.e., > roughly the same resolution. The main reason for this is that > higher order does not buy you increased resolution. (The > Nyquist sampling theorem dictates at least 2*k points are > required to resolve a signal of wavenumber k.) What the > high-order method gains is improved accuracy for the modes > that _are_ resolved. My goal is to try to ensure that > the performance is comparable to a low-order code - i.e., > that costs are not inordinate w/ N. > > What type of comparison did you have in mind ? You might > be interested in: www.mcs.anl.gov/~fischer/users.pdf > which is a work-in-progress. > > Paul > > > > On Tue, 14 Sep 2010, nek5000-users at lists.mcs.anl.gov wrote: > >> Hello All. >> >> I am doing some tests of Nek5000 against a low-order code. Under "Performance tips", it is recommended to "design your resolution (mesh) for N=7 or N=9" >> >> Are there any limitations on the range of values for N? For example, what is the smallest N and largest N that the code can/has been run with? What are the limitations with running at, say, N = 16? >> >> Thanks. >> --Mike >> >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Tue Sep 14 12:37:49 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 14 Sep 2010 11:37:49 -0600 (GMT-06:00) Subject: [Nek5000-users] element order range In-Reply-To: <623CB443-D204-4360-80A0-C879DE8C3328@nrel.gov> Message-ID: <2068438727.882911284485869708.JavaMail.root@zimbra.anl.gov> Mike: If you're ready with the NEK case we're more than happy to have a look at it. Sometimes it can get a little bit tricky to find the right solver parameters to get the most out of it. We're very interested into comparisons like this! -Stefan ----- Original Message ----- From: nek5000-users at lists.mcs.anl.gov To: nek5000-users at lists.mcs.anl.gov Sent: Tuesday, September 14, 2010 12:31:40 PM GMT -06:00 US/Canada Central Subject: Re: [Nek5000-users] element order range Paul, Thanks for that info and for the document. Both are very helpful. There's interest here in using OpenFOAM (second-order finite-volume), and I'm interested to see how Nek does in a head to head comparison. We're using turbulent planar Couette flow as our comparison test case with Re = 8000 (See, e.g. Sullivan et al. (JFM 404, 2000). We're looking at accuracy for a given number of grid points and scalability over 16-1024 cores. I'll let you know how things turn out with the comparison. --Mike On Sep 14, 2010, at 10:33 AM, wrote: > > Hi Mike, > > I've run with N=120 in the past and just this past > week was running w/ N=64. (I had to bump up a couple > of parameters past the 40 or 50 mark to do so.) > > Stefan has run the Pn-Pn variant with N=1 (lx1=2). > > lx1=6-12 is the general sweet spot for the code because > of the way the operators are evaluated... > > When comparing to a low-order code it's generally best > to compare for an equal number of gridpoints - i.e., > roughly the same resolution. The main reason for this is that > higher order does not buy you increased resolution. (The > Nyquist sampling theorem dictates at least 2*k points are > required to resolve a signal of wavenumber k.) What the > high-order method gains is improved accuracy for the modes > that _are_ resolved. My goal is to try to ensure that > the performance is comparable to a low-order code - i.e., > that costs are not inordinate w/ N. > > What type of comparison did you have in mind ? You might > be interested in: www.mcs.anl.gov/~fischer/users.pdf > which is a work-in-progress. > > Paul > > > > On Tue, 14 Sep 2010, nek5000-users at lists.mcs.anl.gov wrote: > >> Hello All. >> >> I am doing some tests of Nek5000 against a low-order code. Under "Performance tips", it is recommended to "design your resolution (mesh) for N=7 or N=9" >> >> Are there any limitations on the range of values for N? For example, what is the smallest N and largest N that the code can/has been run with? What are the limitations with running at, say, N = 16? >> >> Thanks. >> --Mike >> >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Tue Sep 14 13:43:47 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 14 Sep 2010 12:43:47 -0600 Subject: [Nek5000-users] element order range In-Reply-To: <2068438727.882911284485869708.JavaMail.root@zimbra.anl.gov> References: <2068438727.882911284485869708.JavaMail.root@zimbra.anl.gov> Message-ID: Stefan, Thanks for the offer. If you'd like to look, I put the relevant files in a .tar.gz file at http://michaelasprague.com/couette_scale.tar.gz It's fairly simple. The dimensions are (Lx,Ly,Lz) = (6,5,1) with periodic BCs in x and y. At z = 0, (ux,uy,uz) = (0,0,0) and at z = 1, (ux,uy,uz)=(1,0,0). The domain is discretized as (Nx,Ny,Nz)=(24,16,16), and N = 13. Please let me know if you have any suggestions for parameter improvements and/or need more information. --Mike On Sep 14, 2010, at 11:37 AM, wrote: > Mike: > > If you're ready with the NEK case we're more than happy to have a look at it. > Sometimes it can get a little bit tricky to find the right solver parameters to get the most out of it. > > We're very interested into comparisons like this! > > -Stefan > > > ----- Original Message ----- > From: nek5000-users at lists.mcs.anl.gov > To: nek5000-users at lists.mcs.anl.gov > Sent: Tuesday, September 14, 2010 12:31:40 PM GMT -06:00 US/Canada Central > Subject: Re: [Nek5000-users] element order range > > Paul, > > Thanks for that info and for the document. Both are very helpful. > > There's interest here in using OpenFOAM (second-order finite-volume), and I'm interested to see how Nek does in a head to head comparison. We're using turbulent planar Couette flow as our comparison test case with Re = 8000 (See, e.g. Sullivan et al. (JFM 404, 2000). We're looking at accuracy for a given number of grid points and scalability over 16-1024 cores. > > I'll let you know how things turn out with the comparison. > > --Mike > > > On Sep 14, 2010, at 10:33 AM, wrote: > >> >> Hi Mike, >> >> I've run with N=120 in the past and just this past >> week was running w/ N=64. (I had to bump up a couple >> of parameters past the 40 or 50 mark to do so.) >> >> Stefan has run the Pn-Pn variant with N=1 (lx1=2). >> >> lx1=6-12 is the general sweet spot for the code because >> of the way the operators are evaluated... >> >> When comparing to a low-order code it's generally best >> to compare for an equal number of gridpoints - i.e., >> roughly the same resolution. The main reason for this is that >> higher order does not buy you increased resolution. (The >> Nyquist sampling theorem dictates at least 2*k points are >> required to resolve a signal of wavenumber k.) What the >> high-order method gains is improved accuracy for the modes >> that _are_ resolved. My goal is to try to ensure that >> the performance is comparable to a low-order code - i.e., >> that costs are not inordinate w/ N. >> >> What type of comparison did you have in mind ? You might >> be interested in: www.mcs.anl.gov/~fischer/users.pdf >> which is a work-in-progress. >> >> Paul >> >> >> >> On Tue, 14 Sep 2010, nek5000-users at lists.mcs.anl.gov wrote: >> >>> Hello All. >>> >>> I am doing some tests of Nek5000 against a low-order code. Under "Performance tips", it is recommended to "design your resolution (mesh) for N=7 or N=9" >>> >>> Are there any limitations on the range of values for N? For example, what is the smallest N and largest N that the code can/has been run with? What are the limitations with running at, say, N = 16? >>> >>> Thanks. >>> --Mike >>> >>> >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Fri Sep 17 12:51:47 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 17 Sep 2010 13:51:47 -0400 Subject: [Nek5000-users] heat transfer in a channel Message-ID: Hi, I'm running a DNS of fully developed heat transfer in a channel, the same as H. Kawamura et. al, International Journal of Heat and Fluid Flow, 1998. I use following subroutine to get rid of additional heat c----------------------------------------------------------------------- subroutine userq (ix,iy,iz,ieg) include 'SIZE' include 'TOTAL' include 'NEKUSE' ie = gllel(ieg) qvol = -vx(ix,iy,iz,ie) source = 0.0 return end c----------------------------------------------------------------------- Other procedures are similar to turbChannel example. But I find the mean temperature is not correct, there should not be negative value in my case. I attached my *.usr and *.rea and means.dat to this email. is there any one else did DNS of heat transfer in a channel ? Thank you very much zhicheng -------------- next part -------------- An HTML attachment was scrubbed... URL: -------------- next part -------------- A non-text attachment was scrubbed... Name: turbHeat.box Type: application/octet-stream Size: 510 bytes Desc: not available URL: -------------- next part -------------- A non-text attachment was scrubbed... Name: turbHeat.rea Type: application/octet-stream Size: 3512 bytes Desc: not available URL: -------------- next part -------------- A non-text attachment was scrubbed... Name: turbHeat.usr Type: application/octet-stream Size: 16611 bytes Desc: not available URL: -------------- next part -------------- A non-text attachment was scrubbed... Name: means.dat Type: application/x-ns-proxy-autoconfig Size: 2260 bytes Desc: not available URL: From nek5000-users at lists.mcs.anl.gov Fri Sep 17 13:25:32 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 17 Sep 2010 13:25:32 -0500 (CDT) Subject: [Nek5000-users] heat transfer in a channel In-Reply-To: References: Message-ID: Zhicheng, We've run under these conditions on a regular basis with this technique. Because temperature is determined only up to a constant there is no apriori reason to anticipate T > 0 everywhere. In general, for uniform heat flux boundary conditions, one writes T(X,t) = T'(X,t) + gamma x + C with X=(x,y,z) and T'(X,t) = T'(X+L,t) being the periodic part computed by nek. Here, C is an arbitrary constant and gamma is a constant determined by the mean temperature rise in the system. Gamma (in your case, gamma==1) should be chosen to balance the thermal enegy input at the boundaries with the flux advected by the mean flow. Note that if constant temperature bcs (as opposed to const. flux) are a bit trickier as that effectively amounts to solving an eigenvalue problem. (See, e.g., M. Greiner, G. Spencer, and P. Fischer, "Direct numerical simulation of three-dimensional flow and augmented heat transfer in a grooved channel" ASME J. of Heat Transfer 120 3 pp. 717-723 (1998). ). Paul On Fri, 17 Sep 2010, nek5000-users at lists.mcs.anl.gov wrote: > Hi, > > I'm running a DNS of fully developed heat transfer in a channel, the same as > H. Kawamura et. al, International Journal of Heat and Fluid Flow, 1998. > > I use following subroutine to get rid of additional heat > > c----------------------------------------------------------------------- > subroutine userq (ix,iy,iz,ieg) > include 'SIZE' > include 'TOTAL' > include 'NEKUSE' > ie = gllel(ieg) > qvol = -vx(ix,iy,iz,ie) > source = 0.0 > > return > end > c----------------------------------------------------------------------- > > Other procedures are similar to turbChannel example. > > But I find the mean temperature is not correct, there should not be > negative value in my case. > > I attached my *.usr and *.rea and means.dat to this email. > > is there any one else did DNS of heat transfer in a channel ? > > > Thank you very much > > > zhicheng > From nek5000-users at lists.mcs.anl.gov Fri Sep 17 16:16:24 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 17 Sep 2010 17:16:24 -0400 Subject: [Nek5000-users] Restarting from the last field file number - new filed file format .f0000* Message-ID: <1284758184.4c93daa850469@webmail.vt.edu> Hello, I am trying to restart my program form the last .f0000 (the new format. old field file format was .fld* as you know) file from the last run. But the old method of specifying the name of the last file in the rea file is not working. Please advise. Thank you, Himanshu From nek5000-users at lists.mcs.anl.gov Fri Sep 17 16:53:33 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 17 Sep 2010 16:53:33 -0500 (CDT) Subject: [Nek5000-users] Restarting from the last field file number - new filed file format .f0000* In-Reply-To: <1284758184.4c93daa850469@webmail.vt.edu> References: <1284758184.4c93daa850469@webmail.vt.edu> Message-ID: The usual think would be to set param(67)=4 in usrdat2() -- this would indicate that you are reading the "old" binary... Leaving p66 to be it's default value will result in the new being written. If you already have a new format, then you would want to make certain that you don't reassign p66 or p67 from their default values. Paul On Fri, 17 Sep 2010, nek5000-users at lists.mcs.anl.gov wrote: > > > Hello, > > I am trying to restart my program form the last .f0000 (the new format. old > field file format was .fld* as you know) file from the last run. But the old > method of specifying the name of the last file in the rea file is not working. > Please advise. > > Thank you, > Himanshu > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > From nek5000-users at lists.mcs.anl.gov Mon Sep 20 09:53:43 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 20 Sep 2010 08:53:43 -0600 Subject: [Nek5000-users] element order range In-Reply-To: References: <2068438727.882911284485869708.JavaMail.root@zimbra.anl.gov> Message-ID: Stefan, I'm about to start some comparison simulations on this problem. Are you still interested in looking over the input files for potential improvements? Thanks. --Mike On Sep 14, 2010, at 12:43 PM, wrote: > Stefan, > > Thanks for the offer. If you'd like to look, I put the relevant files in a .tar.gz file at > > http://michaelasprague.com/couette_scale.tar.gz > > It's fairly simple. The dimensions are (Lx,Ly,Lz) = (6,5,1) with periodic BCs in x and y. At z = 0, (ux,uy,uz) = (0,0,0) and at z = 1, (ux,uy,uz)=(1,0,0). > > The domain is discretized as (Nx,Ny,Nz)=(24,16,16), and N = 13. > > Please let me know if you have any suggestions for parameter improvements and/or need more information. > > --Mike > > On Sep 14, 2010, at 11:37 AM, wrote: > >> Mike: >> >> If you're ready with the NEK case we're more than happy to have a look at it. >> Sometimes it can get a little bit tricky to find the right solver parameters to get the most out of it. >> >> We're very interested into comparisons like this! >> >> -Stefan >> >> >> ----- Original Message ----- >> From: nek5000-users at lists.mcs.anl.gov >> To: nek5000-users at lists.mcs.anl.gov >> Sent: Tuesday, September 14, 2010 12:31:40 PM GMT -06:00 US/Canada Central >> Subject: Re: [Nek5000-users] element order range >> >> Paul, >> >> Thanks for that info and for the document. Both are very helpful. >> >> There's interest here in using OpenFOAM (second-order finite-volume), and I'm interested to see how Nek does in a head to head comparison. We're using turbulent planar Couette flow as our comparison test case with Re = 8000 (See, e.g. Sullivan et al. (JFM 404, 2000). We're looking at accuracy for a given number of grid points and scalability over 16-1024 cores. >> >> I'll let you know how things turn out with the comparison. >> >> --Mike >> >> >> On Sep 14, 2010, at 10:33 AM, wrote: >> >>> >>> Hi Mike, >>> >>> I've run with N=120 in the past and just this past >>> week was running w/ N=64. (I had to bump up a couple >>> of parameters past the 40 or 50 mark to do so.) >>> >>> Stefan has run the Pn-Pn variant with N=1 (lx1=2). >>> >>> lx1=6-12 is the general sweet spot for the code because >>> of the way the operators are evaluated... >>> >>> When comparing to a low-order code it's generally best >>> to compare for an equal number of gridpoints - i.e., >>> roughly the same resolution. The main reason for this is that >>> higher order does not buy you increased resolution. (The >>> Nyquist sampling theorem dictates at least 2*k points are >>> required to resolve a signal of wavenumber k.) What the >>> high-order method gains is improved accuracy for the modes >>> that _are_ resolved. My goal is to try to ensure that >>> the performance is comparable to a low-order code - i.e., >>> that costs are not inordinate w/ N. >>> >>> What type of comparison did you have in mind ? You might >>> be interested in: www.mcs.anl.gov/~fischer/users.pdf >>> which is a work-in-progress. >>> >>> Paul >>> >>> >>> >>> On Tue, 14 Sep 2010, nek5000-users at lists.mcs.anl.gov wrote: >>> >>>> Hello All. >>>> >>>> I am doing some tests of Nek5000 against a low-order code. Under "Performance tips", it is recommended to "design your resolution (mesh) for N=7 or N=9" >>>> >>>> Are there any limitations on the range of values for N? For example, what is the smallest N and largest N that the code can/has been run with? What are the limitations with running at, say, N = 16? >>>> >>>> Thanks. >>>> --Mike >>>> >>>> >>>> _______________________________________________ >>>> Nek5000-users mailing list >>>> Nek5000-users at lists.mcs.anl.gov >>>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>>> >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Mon Sep 20 11:07:31 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 20 Sep 2010 10:07:31 -0600 (GMT-06:00) Subject: [Nek5000-users] element order range In-Reply-To: Message-ID: <490643411.95891284998851886.JavaMail.root@zimbra.anl.gov> Let's discuss this off-list. -Stefan ----- Original Message ----- From: nek5000-users at lists.mcs.anl.gov To: nek5000-users at lists.mcs.anl.gov Sent: Monday, September 20, 2010 9:53:43 AM GMT -06:00 US/Canada Central Subject: Re: [Nek5000-users] element order range Stefan, I'm about to start some comparison simulations on this problem. Are you still interested in looking over the input files for potential improvements? Thanks. --Mike On Sep 14, 2010, at 12:43 PM, wrote: > Stefan, > > Thanks for the offer. If you'd like to look, I put the relevant files in a .tar.gz file at > > http://michaelasprague.com/couette_scale.tar.gz > > It's fairly simple. The dimensions are (Lx,Ly,Lz) = (6,5,1) with periodic BCs in x and y. At z = 0, (ux,uy,uz) = (0,0,0) and at z = 1, (ux,uy,uz)=(1,0,0). > > The domain is discretized as (Nx,Ny,Nz)=(24,16,16), and N = 13. > > Please let me know if you have any suggestions for parameter improvements and/or need more information. > > --Mike > > On Sep 14, 2010, at 11:37 AM, wrote: > >> Mike: >> >> If you're ready with the NEK case we're more than happy to have a look at it. >> Sometimes it can get a little bit tricky to find the right solver parameters to get the most out of it. >> >> We're very interested into comparisons like this! >> >> -Stefan >> >> >> ----- Original Message ----- >> From: nek5000-users at lists.mcs.anl.gov >> To: nek5000-users at lists.mcs.anl.gov >> Sent: Tuesday, September 14, 2010 12:31:40 PM GMT -06:00 US/Canada Central >> Subject: Re: [Nek5000-users] element order range >> >> Paul, >> >> Thanks for that info and for the document. Both are very helpful. >> >> There's interest here in using OpenFOAM (second-order finite-volume), and I'm interested to see how Nek does in a head to head comparison. We're using turbulent planar Couette flow as our comparison test case with Re = 8000 (See, e.g. Sullivan et al. (JFM 404, 2000). We're looking at accuracy for a given number of grid points and scalability over 16-1024 cores. >> >> I'll let you know how things turn out with the comparison. >> >> --Mike >> >> >> On Sep 14, 2010, at 10:33 AM, wrote: >> >>> >>> Hi Mike, >>> >>> I've run with N=120 in the past and just this past >>> week was running w/ N=64. (I had to bump up a couple >>> of parameters past the 40 or 50 mark to do so.) >>> >>> Stefan has run the Pn-Pn variant with N=1 (lx1=2). >>> >>> lx1=6-12 is the general sweet spot for the code because >>> of the way the operators are evaluated... >>> >>> When comparing to a low-order code it's generally best >>> to compare for an equal number of gridpoints - i.e., >>> roughly the same resolution. The main reason for this is that >>> higher order does not buy you increased resolution. (The >>> Nyquist sampling theorem dictates at least 2*k points are >>> required to resolve a signal of wavenumber k.) What the >>> high-order method gains is improved accuracy for the modes >>> that _are_ resolved. My goal is to try to ensure that >>> the performance is comparable to a low-order code - i.e., >>> that costs are not inordinate w/ N. >>> >>> What type of comparison did you have in mind ? You might >>> be interested in: www.mcs.anl.gov/~fischer/users.pdf >>> which is a work-in-progress. >>> >>> Paul >>> >>> >>> >>> On Tue, 14 Sep 2010, nek5000-users at lists.mcs.anl.gov wrote: >>> >>>> Hello All. >>>> >>>> I am doing some tests of Nek5000 against a low-order code. Under "Performance tips", it is recommended to "design your resolution (mesh) for N=7 or N=9" >>>> >>>> Are there any limitations on the range of values for N? For example, what is the smallest N and largest N that the code can/has been run with? What are the limitations with running at, say, N = 16? >>>> >>>> Thanks. >>>> --Mike >>>> >>>> >>>> _______________________________________________ >>>> Nek5000-users mailing list >>>> Nek5000-users at lists.mcs.anl.gov >>>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >>>> >>> _______________________________________________ >>> Nek5000-users mailing list >>> Nek5000-users at lists.mcs.anl.gov >>> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users >> _______________________________________________ >> Nek5000-users mailing list >> Nek5000-users at lists.mcs.anl.gov >> https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users > > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Wed Sep 22 22:35:09 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 22 Sep 2010 22:35:09 -0500 (CDT) Subject: [Nek5000-users] Grid 2 Grid Interpolation In-Reply-To: <86218368.515351285212807515.JavaMail.root@neo-mail-3> Message-ID: <2040683496.515811285212909088.JavaMail.root@neo-mail-3> Hi Stefan, I am having some difficulty using this routine and would like to check that I am setting things up correctly.? Do I set PPList = " MPIIO " in makenek ? Also, I have set lpart to 100000.? The issue I am having is that when I run nek to generate the newgfld it is not outputting any data into 'newg0.f00001'. It creates it, but nothing is written and then nek quits. Also, can I use existing fld files from each case, old and new, or does the new case need to be a "blank slate"? Thanks for help with this, and if you would like I can create a case file to send. - Michael -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Sep 23 10:42:57 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 23 Sep 2010 09:42:57 -0600 (GMT-06:00) Subject: [Nek5000-users] Grid 2 Grid Interpolation In-Reply-To: <2040683496.515811285212909088.JavaMail.root@neo-mail-3> Message-ID: <2120373201.141441285256577689.JavaMail.root@zimbra.anl.gov> Send over the case and I'll try to have a look at it. -Stefan ----- Original Message ----- From: nek5000-users at lists.mcs.anl.gov To: Nekton User List Sent: Wed, 22 Sep 2010 21:35:09 -0600 (GMT-06:00) Subject: [Nek5000-users] Grid 2 Grid Interpolation Hi Stefan, I am having some difficulty using this routine and would like to check that I am setting things up correctly.? Do I set PPList = " MPIIO " in makenek ? Also, I have set lpart to 100000.? The issue I am having is that when I run nek to generate the newgfld it is not outputting any data into 'newg0.f00001'. It creates it, but nothing is written and then nek quits. Also, can I use existing fld files from each case, old and new, or does the new case need to be a "blank slate"? Thanks for help with this, and if you would like I can create a case file to send. - Michael From nek5000-users at lists.mcs.anl.gov Thu Sep 23 11:41:04 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 23 Sep 2010 10:41:04 -0600 (GMT-06:00) Subject: [Nek5000-users] Grid 2 Grid Interpolation In-Reply-To: <2120373201.141441285256577689.JavaMail.root@zimbra.anl.gov> Message-ID: <2021243367.146011285260064804.JavaMail.root@zimbra.anl.gov> >I am having some difficulty using this routine and would like to check that I am setting things ?>up correctly.? Do I set PPList = " MPIIO " in makenek ? Yes, g2gi() will only work with enabled MPI-IO support. >Also, I have set lpart to 100000.? The issue I am having is that when I run nek to generate the >newgfld it is not outputting any data into 'newg0.f00001'. You need to adjust lpart such that the data fits on the given number of processors. Make sure your lpart is not too large otherwise the memory footprint will go through the roof. >It creates it, but nothing is written and then nek quits. Can you send me the logfile of this run. >Also, can I use existing fld files from each case, old and new, or does the new case need to be a >"blank slate"? Thanks for help with this, and if you would like I can create a case file to send. Any fld-file containing the new geometry will work. Stefan From nek5000-users at lists.mcs.anl.gov Fri Sep 24 10:53:35 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Fri, 24 Sep 2010 17:53:35 +0200 Subject: [Nek5000-users] Smooth Restart feature in Nek In-Reply-To: References: Message-ID: <4C9CC97F.2020804@lav.mavt.ethz.ch> Hi all. First, i have a comment that may save some time to some users. If i am correct, in Paul's comments rstx.fld03 and rstx.fld04 are the two fields after the x.fld92. Thus if x.fld92 is the field at time step NT=9200 , rstx.fld03 and rstx.fld04 are at NT=9201 and NT=9202. This means that if you want to restart a simulation from NT=10000, you need to run it at least until NT=10002 ( using Torder=3). Is that correct? Second, i have a problem. I think I am able to restart the velocity smoothly, but i may have a problem with the temperature. Attached there are two figures of the perturbation energy (e2=) and the temperature root mean square during the restart of an heated turbulent channel. The full restart clearly improves e2, while the temperature has the same behavior of the standard restart. Am I misled by the plots? Do i have to do anything particular for the restart of the scalars? Did anybody else have the same issue? Thank you for any help. francesco On 08/11/2010 03:03 PM, nek5000-users at lists.mcs.anl.gov wrote: > Shriram, > > Attached is a full-restart routine. You need to update the repo > to use it. It seems to work ok - hopefully the remarks in the attached > .usr file are clear. > > Paul > > On Mon, 9 Aug 2010, nek5000-users at lists.mcs.anl.gov wrote: > > >> Hi Paul, >> >> Thanks a lot. That would be very helpful. >> >> Regards >> Shriram >> >> -------------- next part -------------- A non-text attachment was scrubbed... Name: t_rms.eps Type: image/x-eps Size: 35040 bytes Desc: not available URL: -------------- next part -------------- A non-text attachment was scrubbed... Name: e2.eps Type: image/x-eps Size: 35581 bytes Desc: not available URL: From nek5000-users at lists.mcs.anl.gov Mon Sep 27 09:01:24 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Mon, 27 Sep 2010 10:01:24 -0400 Subject: [Nek5000-users] Restarting from the last field file number - new filed file format .f0000* Message-ID: <1285596084.4ca0a3b431da0@webmail.vt.edu> Hello Paul, The p66 and p67 in usrdat2() were commented out as per Stefan's recommendation. I uncommented them and tried to restart the program from the last field file number, but it was unable to read from the last file. In the rea file p66=4 and p67=-4 (I am setting this to -4 to get the output in ascii format). Thank you for your help. Himanshu from nek5000-users at lists.mcs.anl.gov reply-to nek5000-users at lists.mcs.anl.gov to nek5000-users at lists.mcs.anl.gov date Fri, Sep 17, 2010 at 5:53 PM subject Re: [Nek5000-users] Restarting from the last field file number - new filed file format .f0000* mailing list Filter messages from this mailing list unsubscribe Unsubscribe from this mailing-list hide details Sep 17 (9 days ago) The usual think would be to set param(67)=4 in usrdat2() -- this would indicate that you are reading the "old" binary... Leaving p66 to be it's default value will result in the new being written. If you already have a new format, then you would want to make certain that you don't reassign p66 or p67 from their default values. Paul From nek5000-users at lists.mcs.anl.gov Tue Sep 28 10:01:33 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 28 Sep 2010 09:01:33 -0600 (GMT-06:00) Subject: [Nek5000-users] Smooth Restart feature in Nek In-Reply-To: <4C9CC97F.2020804@lav.mavt.ethz.ch> Message-ID: <459448884.344521285686093527.JavaMail.root@zimbra.anl.gov> Is this with CVODE? -Stefan ----- Original Message ----- From: nek5000-users at lists.mcs.anl.gov To: nek5000-users at lists.mcs.anl.gov Sent: Fri, 24 Sep 2010 09:53:35 -0600 (GMT-06:00) Subject: Re: [Nek5000-users] Smooth Restart feature in Nek Hi all. First, i have a comment that may save some time to some users. If i am correct, in Paul's comments rstx.fld03 and rstx.fld04 are the two fields after the x.fld92. Thus if x.fld92 is the field at time step NT=9200 , rstx.fld03 and rstx.fld04 are at NT=9201 and NT=9202. This means that if you want to restart a simulation from NT=10000, you need to run it at least until NT=10002 ( using Torder=3). Is that correct? Second, i have a problem. I think I am able to restart the velocity smoothly, but i may have a problem with the temperature. Attached there are two figures of the perturbation energy (e2=) and the temperature root mean square during the restart of an heated turbulent channel. The full restart clearly improves e2, while the temperature has the same behavior of the standard restart. Am I misled by the plots? Do i have to do anything particular for the restart of the scalars? Did anybody else have the same issue? Thank you for any help. francesco On 08/11/2010 03:03 PM, nek5000-users at lists.mcs.anl.gov wrote: > Shriram, > > Attached is a full-restart routine. You need to update the repo > to use it. It seems to work ok - hopefully the remarks in the attached > .usr file are clear. > > Paul > > On Mon, 9 Aug 2010, nek5000-users at lists.mcs.anl.gov wrote: > > >> Hi Paul, >> >> Thanks a lot. That would be very helpful. >> >> Regards >> Shriram >> >> From nek5000-users at lists.mcs.anl.gov Tue Sep 28 10:21:59 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 28 Sep 2010 17:21:59 +0200 Subject: [Nek5000-users] Smooth Restart feature in Nek In-Reply-To: <459448884.344521285686093527.JavaMail.root@zimbra.anl.gov> References: <459448884.344521285686093527.JavaMail.root@zimbra.anl.gov> Message-ID: <4CA20817.7000606@gmail.com> Hi Nek's :-) , Francesco, I also encounter this problem and I was on the edge of writing such an email when the mail-list forwarded yours. I work on stenotic flows (non-linear evolution of infinitesimal perturbations), and because of the long-time dynamics we wanna observe, restarting the simulations from previous time steps is not an option. I set various probes within the flow to plot the velocity. Just like you, I have no problem so far: the velocity restarts smoothly. However, I compute the total energy in usrchk as being the square of the L2-norm and I indeed also get a jump at the restart timestep when plotting this energy. Help (or at least a few hints on how to solve this) would be highly appreciated. Sincerely yours, JC From nek5000-users at lists.mcs.anl.gov Tue Sep 28 12:19:01 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 28 Sep 2010 19:19:01 +0200 Subject: [Nek5000-users] Smooth Restart feature in Nek In-Reply-To: <4CA20817.7000606@gmail.com> References: <459448884.344521285686093527.JavaMail.root@zimbra.anl.gov> <4CA20817.7000606@gmail.com> Message-ID: <4CA22385.4020108@lav.mavt.ethz.ch> Hi Stefan, yes, the test was done with CVODE. @ JC , i have the jump in energy only with a standard restart. The energy restarts smoothly ( see e2.eps of the previous email ) if I use the subroutine "my_full_restart_load" that Paul posted here on 8/11/2010. Thanks everybody francesco On 09/28/2010 05:21 PM, nek5000-users at lists.mcs.anl.gov wrote: > Hi Nek's :-) , > > Francesco, I also encounter this problem and I was on the edge of > writing such an email when the mail-list forwarded yours. I work on > stenotic flows (non-linear evolution of infinitesimal perturbations), > and because of the long-time dynamics we wanna observe, restarting the > simulations from previous time steps is not an option. > > I set various probes within the flow to plot the velocity. Just like > you, I have no problem so far: the velocity restarts smoothly. > However, I compute the total energy in usrchk as being the square of > the L2-norm and I indeed also get a jump at the restart timestep when > plotting this energy. > > Help (or at least a few hints on how to solve this) would be highly > appreciated. > Sincerely yours, > > JC > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Tue Sep 28 12:43:58 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 28 Sep 2010 11:43:58 -0600 (GMT-06:00) Subject: [Nek5000-users] Smooth Restart feature in Nek In-Reply-To: <4CA22385.4020108@lav.mavt.ethz.ch> Message-ID: <978727370.378771285695838239.JavaMail.root@zimbra.anl.gov> You cannot do an accurate (taking the full BDF history) restart if you use CVODE. Stefan ----- Original Message ----- From: nek5000-users at lists.mcs.anl.gov To: nek5000-users at lists.mcs.anl.gov Sent: Tue, 28 Sep 2010 11:19:01 -0600 (GMT-06:00) Subject: Re: [Nek5000-users] Smooth Restart feature in Nek Hi Stefan, yes, the test was done with CVODE. @ JC , i have the jump in energy only with a standard restart. The energy restarts smoothly ( see e2.eps of the previous email ) if I use the subroutine "my_full_restart_load" that Paul posted here on 8/11/2010. Thanks everybody francesco On 09/28/2010 05:21 PM, nek5000-users at lists.mcs.anl.gov wrote: > Hi Nek's :-) , > > Francesco, I also encounter this problem and I was on the edge of > writing such an email when the mail-list forwarded yours. I work on > stenotic flows (non-linear evolution of infinitesimal perturbations), > and because of the long-time dynamics we wanna observe, restarting the > simulations from previous time steps is not an option. > > I set various probes within the flow to plot the velocity. Just like > you, I have no problem so far: the velocity restarts smoothly. > However, I compute the total energy in usrchk as being the square of > the L2-norm and I indeed also get a jump at the restart timestep when > plotting this energy. > > Help (or at least a few hints on how to solve this) would be highly > appreciated. > Sincerely yours, > > JC > _______________________________________________ > Nek5000-users mailing list > Nek5000-users at lists.mcs.anl.gov > https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users _______________________________________________ Nek5000-users mailing list Nek5000-users at lists.mcs.anl.gov https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users From nek5000-users at lists.mcs.anl.gov Tue Sep 28 15:10:00 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Tue, 28 Sep 2010 15:10:00 -0500 Subject: [Nek5000-users] conjugate heat and low mach Message-ID: <21B5B5BD-4915-4977-A6E4-E21545038C17@exosent.com> Hi NEKs I'm trying to get a low mach number with conjugate heat going, but the solution is diverging on iteration 1 and then the pressure blows up really quick on iteration 2. Anybody got this combination working? The geometry right now is really simple, just a solid annulus with constant temperature inner radius and surrounded by air. Thanks, Andrew From nek5000-users at lists.mcs.anl.gov Wed Sep 29 03:42:40 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 29 Sep 2010 10:42:40 +0200 Subject: [Nek5000-users] Smooth Restart feature in Nek In-Reply-To: <978727370.378771285695838239.JavaMail.root@zimbra.anl.gov> References: <978727370.378771285695838239.JavaMail.root@zimbra.anl.gov> Message-ID: <4CA2FC00.4000406@lav.mavt.ethz.ch> thank you francesco On 09/28/2010 07:43 PM, nek5000-users at lists.mcs.anl.gov wrote: > You cannot do an accurate (taking the full BDF history) restart if you use CVODE. > Stefan > > > ----- Original Message ----- > From: nek5000-users at lists.mcs.anl.gov > To: nek5000-users at lists.mcs.anl.gov > Sent: Tue, 28 Sep 2010 11:19:01 -0600 (GMT-06:00) > Subject: Re: [Nek5000-users] Smooth Restart feature in Nek > > Hi Stefan, > > yes, the test was done with CVODE. > > @ JC > , i have the jump in energy only with a standard restart. The energy > restarts smoothly > ( see e2.eps of the previous email ) if I use the subroutine > "my_full_restart_load" that Paul posted here on 8/11/2010. > > > Thanks everybody > > francesco > > > > > On 09/28/2010 05:21 PM, nek5000-users at lists.mcs.anl.gov wrote: > >> Hi Nek's :-) , >> >> Francesco, I also encounter this problem and I was on the edge of >> writing such an email when the mail-list forwarded yours. I work on >> stenotic flows (non-linear evolution of infinitesimal perturbations), >> and because of the long-time dynamics we wanna observe, restarting the >> simulations from previous time steps is not an option. >> >> I set various probes within the flow to plot the velocity. Just like >> you, I have no problem so far: the velocity restarts smoothly. >> However, I compute the total energy in usrchk as being the square of >> the L2-norm and I indeed also get a jump at the restart timestep when >> plotting this energy. >> >> Help (or at least a few hints on how to solve this) would be highly >> appreciated. >> Sincerely yours, >> >> JC >> _______________________________________________ >> 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 Sep 29 08:36:20 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 29 Sep 2010 07:36:20 -0600 (GMT-06:00) Subject: [Nek5000-users] conjugate heat and low mach In-Reply-To: <21B5B5BD-4915-4977-A6E4-E21545038C17@exosent.com> Message-ID: <1110432097.432791285767380943.JavaMail.root@zimbra.anl.gov> Andrew: We have another user reporting similar problems with the Low Mach number formulation and CHT. I'll try to have a look at it. -Stefan ----- Original Message ----- From: nek5000-users at lists.mcs.anl.gov To: nek5000-users at lists.mcs.anl.gov Sent: Tue, 28 Sep 2010 14:10:00 -0600 (GMT-06:00) Subject: [Nek5000-users] conjugate heat and low mach Hi NEKs I'm trying to get a low mach number with conjugate heat going, but the solution is diverging on iteration 1 and then the pressure blows up really quick on iteration 2. Anybody got this combination working? The geometry right now is really simple, just a solid annulus with constant temperature inner radius and surrounded by air. Thanks, Andrew _______________________________________________ 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 Sep 29 23:09:38 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 29 Sep 2010 23:09:38 -0500 (CDT) Subject: [Nek5000-users] Boundary Condtions not being read after restart In-Reply-To: <723563374.2464671285819637025.JavaMail.root@neo-mail-3> Message-ID: <1321422007.2465641285819778930.JavaMail.root@neo-mail-3> Hi, I am having an issue with a restart in which I want to change the boundary condition for the inlet.?Simply put the issue is that the boundary condition is not being used.? For the old runs I had? ux = const ?? and uy = uz = 0. For the new runs I still have ux = const ? but now I want to use Walsh solution in uy and uz .? However uy and uz are still? = 0 , and the ux is not even the constant that is specified (close but too low).? Any thoughts as to why? Thanks, Michael -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Wed Sep 29 23:12:17 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Wed, 29 Sep 2010 23:12:17 -0500 Subject: [Nek5000-users] Visualizing lambda2 vortices Message-ID: Hi, I was looking at Paul's pretty picture ( http://www.mcs.anl.gov/~fischer/cfd/hairpin_split.html) which I assume is iso-surfaces of vorticity and had a question regarding visualizing lambda2 vortices. I have the lambda2 vortices calculated and stored as a passive scalar in the field files but cant figure out a way to visualize them. How do you generally visualize the dominant structures in the flow, say for eg, the hairpin vortices in the same animation ? Regards Shriram -------------- next part -------------- An HTML attachment was scrubbed... URL: From nek5000-users at lists.mcs.anl.gov Thu Sep 30 05:24:21 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 30 Sep 2010 05:24:21 -0500 (CDT) Subject: [Nek5000-users] Visualizing lambda2 vortices In-Reply-To: References: Message-ID: Those are lambda2s, with pressure mapped onto the isosurface. Here is another - www.mcs.anl.gov/~fischer/hemi/hemi_0700.gif These are isosurfaces of lambda2 (probably lambda2 = -.1 or something --- usually a slight negative bias is required). In VisIt, you can select an isosurface of scalar A and then map scalar value B onto that surface as a pseudocolor plot. The plate and hemisphere are visualized by setting A to be velocity magnitude=.0001 (say) with B=pressure. The lambda2 vortices are visualized by setting A to be temperature (which is where lambda2 is stored in my case) and B to be velocity magnitude. (Choosing B to be pressure for both the walls and the vortices did not yield high contrast...) Paul On Wed, 29 Sep 2010, nek5000-users at lists.mcs.anl.gov wrote: > Hi, > > I was looking at Paul's pretty picture ( > http://www.mcs.anl.gov/~fischer/cfd/hairpin_split.html) which I assume is > iso-surfaces of vorticity and had a question regarding visualizing lambda2 > vortices. I have the lambda2 vortices calculated and stored as a passive > scalar in the field files but cant figure out a way to visualize them. How > do you generally visualize the dominant structures in the flow, say for eg, > the hairpin vortices in the same animation ? > > Regards > Shriram > From nek5000-users at lists.mcs.anl.gov Thu Sep 30 05:44:42 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 30 Sep 2010 05:44:42 -0500 (CDT) Subject: [Nek5000-users] Boundary Condtions not being read after restart In-Reply-To: <1321422007.2465641285819778930.JavaMail.root@neo-mail-3> References: <1321422007.2465641285819778930.JavaMail.root@neo-mail-3> Message-ID: Hi Michael, if you send me your .usr file off-list we can take a look here. Thanks, Paul On Wed, 29 Sep 2010, nek5000-users at lists.mcs.anl.gov wrote: > > > Hi, > > > > I am having an issue with a restart in which I want to change the boundary condition for the inlet.??Simply put the issue is that the boundary condition > > is not being used.?? > > > > For the old runs I had?? ux = const ???? and uy = uz = 0. > > For the new runs I still have ux = const ?? but now I want to use Walsh solution in uy and uz .?? > > > > However uy and uz are still?? = 0 , and the ux is not even the constant that is specified (close but too low).?? Any thoughts as to why? > > > > Thanks, > > Michael > From nek5000-users at lists.mcs.anl.gov Thu Sep 30 08:37:52 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 30 Sep 2010 15:37:52 +0200 Subject: [Nek5000-users] Smooth Restart feature in Nek In-Reply-To: <4CA2FC00.4000406@lav.mavt.ethz.ch> References: <978727370.378771285695838239.JavaMail.root@zimbra.anl.gov> <4CA2FC00.4000406@lav.mavt.ethz.ch> Message-ID: <4CA492B0.4060607@gmail.com> Hi Nek's :-) , I have a problem when using the full_restart routine with the .f???? format: a few iterations after the restart the simulation crashes. Attached are the .usr file I've been using + the logfiles before and after restart. Note however that when using the old .fld format, everything works fine. Best regards, JC -------------- next part -------------- An embedded and charset-unspecified text was scrubbed... Name: After_Logfile URL: -------------- next part -------------- An embedded and charset-unspecified text was scrubbed... Name: stenosis.usr URL: From nek5000-users at lists.mcs.anl.gov Thu Sep 30 09:08:37 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 30 Sep 2010 16:08:37 +0200 Subject: [Nek5000-users] Smooth Restart feature in Nek In-Reply-To: <4CA492B0.4060607@gmail.com> References: <978727370.378771285695838239.JavaMail.root@zimbra.anl.gov> <4CA2FC00.4000406@lav.mavt.ethz.ch> <4CA492B0.4060607@gmail.com> Message-ID: <4CA499E5.3090803@lav.mavt.ethz.ch> JC, I think you have loaded the wrong rst* files. I think your my_old_run0.f00004 is the field at t=4.00000E-02 while 'rststenosis0.f00001' and rststenosis0.f00002 are the fields at 3.0100E-02 and 3.0200E-02. francesco On 09/30/2010 03:37 PM, nek5000-users at lists.mcs.anl.gov wrote: > Hi Nek's :-) , > > I have a problem when using the full_restart routine with the .f???? > format: a few iterations after the restart the simulation crashes. > Attached are the .usr file I've been using + the logfiles before and > after restart. Note however that when using the old .fld format, > everything works fine. > > Best regards, > JC > > > _______________________________________________ > 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 Sep 30 09:43:36 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 30 Sep 2010 09:43:36 -0500 (CDT) Subject: [Nek5000-users] Nek5000 Workshop at ANL, December 9 & 10, 2010. Message-ID: Dear Nek5000 Users: We are pleased to invite you to attend the first Nek5000 Workshop, to be held at Argonne National Laboratory on December 9-10, 2010. The intent is to bring developers and users of Nek5000 together to promote collaborative activities, exchange information, and share experiences in areas of common interest. The schedule is under development, but we currently are planning to have technical sessions on Dec. 9 and Dec. 10, including hands-on sessions in the use of Nek5000, VisIt, and Cubit. One objective of the workshop is to assist users in defining their simulation problems and to address technical issues that they may face. Attendees are invited to contribute short (15 min.) presentations on their applications of Nek5000. Contributions should consist of an abstract (1-2 pages) and presentation slides. Please note that, as this is the first users meeting, we are uncertain of anticipated interest and may therefore cancel the meeting if we do not meet a critical attendance limit. It is therefore important to register by the deadline if you plan to come, so that suitable arrangements may be made at ANL. REGISTRATION DEADLINE: October 15. To register, please visit https://nek5000.mcs.anl.gov/index.php/usermeeting2010 We look forward to your attendance! Sincerely, Nek5000 Development Team From nek5000-users at lists.mcs.anl.gov Thu Sep 30 10:11:14 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 30 Sep 2010 17:11:14 +0200 Subject: [Nek5000-users] Smooth Restart feature in Nek In-Reply-To: <4CA499E5.3090803@lav.mavt.ethz.ch> References: <978727370.378771285695838239.JavaMail.root@zimbra.anl.gov> <4CA2FC00.4000406@lav.mavt.ethz.ch> <4CA492B0.4060607@gmail.com> <4CA499E5.3090803@lav.mavt.ethz.ch> Message-ID: <4CA4A892.20904@gmail.com> Yes indeed, the rst* files specified in the .usr attached to my previous mail are not the correct ones. However, I have also tried with the correct restart pair and it did not change anything. The simulation still crashes after a few time steps. JC From nek5000-users at lists.mcs.anl.gov Thu Sep 30 11:02:44 2010 From: nek5000-users at lists.mcs.anl.gov (nek5000-users at lists.mcs.anl.gov) Date: Thu, 30 Sep 2010 11:02:44 -0500 Subject: [Nek5000-users] Visualizing lambda2 vortices In-Reply-To: References: Message-ID: Hi Paul, The animations are very impressive ! I can now spot the hairpin structures in my flow but it required a much higher value of lambda2- about -200 or so. A=temperature and B=velocity worked really well. Thanks. Regards Shriram On 30 September 2010 05:24, wrote: > > Those are lambda2s, with pressure mapped onto the isosurface. > > Here is another - www.mcs.anl.gov/~fischer/hemi/hemi_0700.gif > > These are isosurfaces of lambda2 (probably lambda2 = -.1 or something > --- usually a slight negative bias is required). > > In VisIt, you can select an isosurface of scalar A and then map > scalar value B onto that surface as a pseudocolor plot. > > The plate and hemisphere are visualized by setting A to > be velocity magnitude=.0001 (say) with B=pressure. > > The lambda2 vortices are visualized by setting A to be temperature > (which is where lambda2 is stored in my case) and B to be velocity > magnitude. > > (Choosing B to be pressure for both the walls and the vortices > did not yield high contrast...) > > Paul > > > > > On Wed, 29 Sep 2010, nek5000-users at lists.mcs.anl.gov wrote: > > Hi, >> >> I was looking at Paul's pretty picture ( >> http://www.mcs.anl.gov/~fischer/cfd/hairpin_split.html) which I assume is >> iso-surfaces of vorticity and had a question regarding visualizing lambda2 >> vortices. I have the lambda2 vortices calculated and stored as a passive >> scalar in the field files but cant figure out a way to visualize them. How >> do you generally visualize the dominant structures in the flow, say for >> eg, >> the hairpin vortices in the same animation ? >> >> Regards >> Shriram >> >> _______________________________________________ > 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: