CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

SonicFoam forwardStep Tutorial OF 14

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   June 9, 2007, 13:51
Default Hey all, I wanted to run the
  #1
tutlhino
Guest
 
Posts: n/a
Hey all,
I wanted to run the tutorial case of sonicFoam - forwardStep and didn't change anything, but it didn't work in OF 1.4. But in OF 1.3 the tutorial case works. Do you know what the problem could be? So the simulation starts but after a while of computing it stops with the following error message:

Courant Number mean: 1.77239e+19 max: 1.46681e+23
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
#0 Foam::error::printStack(Foam:stream&)
#1 Foam::sigFpe::sigFpeHandler(int)
#2 Uninterpreted: [0xb7fa1420]
#3 Foam::DILUPreconditioner::DILUPreconditioner(Foam: :lduMatrix::solver const&, Foam::Istream&)
#4 Foam::lduMatrix::preconditioner::addasymMatrixCons tructorToTable<foam::dilupreco nditioner>::New(Foam::lduMatrix::solver const&, Foam::Istream&)
#5 Foam::lduMatrix::preconditioner::New(Foam::lduMatr ix::solver const&, Foam::Istream&)
#6 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const
#7 Foam::fvMatrix<foam::vector<double> >::solve(Foam::Istream&)
#8 Foam::lduMatrix::solverPerformance Foam::solve<foam::vector<double> >(Foam::tmp<foam::fvmatrix<foam::vector<double> > > const&)
#9 main
#10 __libc_start_main
#11 __gxx_personality_v0 at /usr/src/packages/BUILD/glibc-2.3/csu/../sysdeps/i386/elf/start.S:122
Gleitkomma-Ausnahme


Unfortunately I need the OF-Version 1.4 where I can take the GAMG-Solver. But at first I've got to make the tutorial case run...

Cheers
Florian
  Reply With Quote

Old   June 9, 2007, 14:45
Default Courant Number mean: 1.77239e+
  #2
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 697
Rep Power: 10
msrinath80 is on a distinguished road
Courant Number mean: 1.77239e+19 max: 1.46681e+23

That clearly indicates divergence.
msrinath80 is offline   Reply With Quote

Old   June 9, 2007, 15:09
Default Thanks, that's what I also tho
  #3
tutlhino
Guest
 
Posts: n/a
Thanks, that's what I also thought of. But as it is a tutorial case I thought that can't be. So if anyone experienced that problem as well and knows how to fix the problem...I'd appreciate it!


Cheers
Florian
  Reply With Quote

Old   June 10, 2007, 08:09
Default Is there nobody who has experi
  #4
tutlhino
Guest
 
Posts: n/a
Is there nobody who has experienced the same problem, or knows where to look?
  Reply With Quote

Old   June 10, 2007, 08:20
Default Give it some time. There is a
  #5
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 697
Rep Power: 10
msrinath80 is on a distinguished road
Give it some time. There is a workshop in progress. Folks are busy. I'm sure someone will respond.
msrinath80 is offline   Reply With Quote

Old   June 10, 2007, 12:15
Default I just checked and the issue c
  #6
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,890
Rep Power: 25
alberto will become famous soon enoughalberto will become famous soon enough
I just checked and the issue can be easily reproduced.

The problem is not reduced by using a smaller time step too.

With dt = 0.002 s, the divergens happens at 1.636s, while reducing dt = 0.002s it happens at 0.063s, and with dt = 0.0005s, I have divergence at 0.0645s.

Regards,
A.
__________________
Alberto

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
GeekoCFD 32bit - The 32bit edition of GeekoCFD.
GeekoCFD text mode - A smaller version of GeekoCFD, text-mode only, with only OpenFOAM. Available in a variety of virtual formats.
alberto is offline   Reply With Quote

Old   June 10, 2007, 12:28
Default Well I tried the same and with
  #7
tutlhino
Guest
 
Posts: n/a
Well I tried the same and with dt=0.003 s it worked, so there was no error-message! I'll try it again but I think this change will fix the problem!
  Reply With Quote

Old   June 10, 2007, 12:38
Default Yes, I can confirm the result!
  #8
tutlhino
Guest
 
Posts: n/a
Yes, I can confirm the result! dt=0.003s solves the problem.
  Reply With Quote

Old   June 10, 2007, 13:37
Default Yes, I checked too. With dt =
  #9
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,890
Rep Power: 25
alberto will become famous soon enoughalberto will become famous soon enough
Yes, I checked too. With dt = 0.003s it doesn't diverge. But this leaves some doubt. Why should it diverge with a smaller time step?

Regards,
A.
__________________
Alberto

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
GeekoCFD 32bit - The 32bit edition of GeekoCFD.
GeekoCFD text mode - A smaller version of GeekoCFD, text-mode only, with only OpenFOAM. Available in a variety of virtual formats.
alberto is offline   Reply With Quote

Old   June 10, 2007, 13:39
Default At the beginning you had dt=0.
  #10
tutlhino
Guest
 
Posts: n/a
At the beginning you had dt=0.002s, so you have increased it! But nevertheless it should work also for higher dts..
  Reply With Quote

Old   June 10, 2007, 13:44
Default I tried the GAMG in that case,
  #11
tutlhino
Guest
 
Posts: n/a
I tried the GAMG in that case, but it took 5 seconds more than with the standard sovers, although I took the same values for the residuum...!? Any ideas why that can be?

By the way, thanks for helping me to find the source of the error in the simplefoam tutorial.

Regards
Florian
  Reply With Quote

Old   June 10, 2007, 13:47
Default Exactly. It's not clear why we
  #12
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,890
Rep Power: 25
alberto will become famous soon enoughalberto will become famous soon enough
Exactly. It's not clear why we obtain a stable solution with a higher time step, while it diverges with a smaller one.

The Courant number should be lower with the smallest time step and, as a consequence, you should not notice instabilities. By increasing it you're probably loosing some oscillation which were the cause of the divergence.

Regards,
A.
__________________
Alberto

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
GeekoCFD 32bit - The 32bit edition of GeekoCFD.
GeekoCFD text mode - A smaller version of GeekoCFD, text-mode only, with only OpenFOAM. Available in a variety of virtual formats.
alberto is offline   Reply With Quote

Old   June 10, 2007, 15:45
Default I opened a bug-report, so that
  #13
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,890
Rep Power: 25
alberto will become famous soon enoughalberto will become famous soon enough
I opened a bug-report, so that Henry and OpenCFD guys can read it more easily.

http://www.cfd-online.com/OpenFOAM_D...tml?1181501044

Regards,
A.
__________________
Alberto

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
GeekoCFD 32bit - The 32bit edition of GeekoCFD.
GeekoCFD text mode - A smaller version of GeekoCFD, text-mode only, with only OpenFOAM. Available in a variety of virtual formats.
alberto is offline   Reply With Quote

Old   June 10, 2007, 16:15
Default This is an error in case setup
  #14
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,748
Rep Power: 20
hjasak will become famous soon enough
This is an error in case setup: wrong outlet boundary conditions on U, p and T in the tutorial..

Change them to zeroGradient (currently, they are inletOutlet) and all works fine.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   June 10, 2007, 16:17
Default Sorry, slight imprecision: the
  #15
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,748
Rep Power: 20
hjasak will become famous soon enough
Sorry, slight imprecision: the boundary condition on p should remain wave transmissive. It is only the inletOutlet stuff that's wrong.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   June 10, 2007, 16:38
Default Thanks! I attached the correct
  #16
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,890
Rep Power: 25
alberto will become famous soon enoughalberto will become famous soon enough
Thanks! I attached the correct tutorial to the bug section.

Alberto
__________________
Alberto

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
GeekoCFD 32bit - The 32bit edition of GeekoCFD.
GeekoCFD text mode - A smaller version of GeekoCFD, text-mode only, with only OpenFOAM. Available in a variety of virtual formats.
alberto is offline   Reply With Quote

Old   May 1, 2008, 17:09
Default I've experienced the same prob
  #17
New Member
 
Roberto
Join Date: Mar 2009
Posts: 17
Rep Power: 7
robbo is on a distinguished road
I've experienced the same problem but I don't understand how to change the boundary conditions at outlet.
I'm using foamX and in the patches menu i select for the outlet "pressure transmissive outlet". In this case i don't manage to change the entries for pressure, velocity and temperature. how to do this?
I've also noted one thing. In the programmer's guide is indicated to specify belong the thermodynamic properties also the thermal conductivity (wich i think is used in the energy equation). Unfortunately i've not found any place to insert it... is this superfluous? I don't think so but i've found no place to specify it.

thanks

Roberto
robbo is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
SonicFoam stvtiegh OpenFOAM Running, Solving & CFD 1 June 26, 2008 10:30
SonicFoam 141dev changes what do they mean mike_jaworski OpenFOAM Running, Solving & CFD 0 December 30, 2007 16:55
SonicFoam divphiU dimi OpenFOAM Running, Solving & CFD 3 June 25, 2007 06:47
Help me with sonicFoam marcelo OpenFOAM Running, Solving & CFD 6 December 10, 2005 03:57
ForwardStep tutorial didomenico OpenFOAM Running, Solving & CFD 1 November 2, 2005 12:57


All times are GMT -4. The time now is 19:14.