CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   SonicFoam forwardStep Tutorial OF 14 (http://www.cfd-online.com/Forums/openfoam-solving/58909-sonicfoam-forwardstep-tutorial-14-a.html)

tutlhino June 9, 2007 12:51

Hey all, I wanted to run the
 
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:http://www.cfd-online.com/OpenFOAM_D...part/proud.gifstream&)
#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

msrinath80 June 9, 2007 13:45

Courant Number mean: 1.77239e+
 
Courant Number mean: 1.77239e+19 max: 1.46681e+23

That clearly indicates divergence.

tutlhino June 9, 2007 14:09

Thanks, that's what I also tho
 
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

tutlhino June 10, 2007 07:09

Is there nobody who has experi
 
Is there nobody who has experienced the same problem, or knows where to look?

msrinath80 June 10, 2007 07:20

Give it some time. There is a
 
Give it some time. There is a workshop in progress. Folks are busy. I'm sure someone will respond.

alberto June 10, 2007 11:15

I just checked and the issue c
 
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.

tutlhino June 10, 2007 11:28

Well I tried the same and with
 
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!

tutlhino June 10, 2007 11:38

Yes, I can confirm the result!
 
Yes, I can confirm the result! dt=0.003s solves the problem.

alberto June 10, 2007 12:37

Yes, I checked too. With dt =
 
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.

tutlhino June 10, 2007 12:39

At the beginning you had dt=0.
 
At the beginning you had dt=0.002s, so you have increased it! But nevertheless it should work also for higher dts..

tutlhino June 10, 2007 12:44

I tried the GAMG in that case,
 
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

alberto June 10, 2007 12:47

Exactly. It's not clear why we
 
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 June 10, 2007 14:45

I opened a bug-report, so that
 
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.

hjasak June 10, 2007 15:15

This is an error in case setup
 
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

hjasak June 10, 2007 15:17

Sorry, slight imprecision: the
 
Sorry, slight imprecision: the boundary condition on p should remain wave transmissive. It is only the inletOutlet stuff that's wrong.

Hrv

alberto June 10, 2007 15:38

Thanks! I attached the correct
 
Thanks! I attached the correct tutorial to the bug section.

Alberto

robbo May 1, 2008 16:09

I've experienced the same prob
 
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


All times are GMT -4. The time now is 08:38.