SonicFoam forwardStep Tutorial OF 14

June 9, 2007, 13:51

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

msrinath80 · June 9, 2007, 14:45

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

That clearly indicates divergence.

June 9, 2007, 15:09

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

June 10, 2007, 08:09

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

msrinath80 · June 10, 2007, 08:20

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

alberto · June 10, 2007, 12:15

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.

June 10, 2007, 12:28

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!

June 10, 2007, 12:38

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

alberto · June 10, 2007, 13:37

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.

June 10, 2007, 13:39

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

June 10, 2007, 13:44

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, 13:47

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, 15:45

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, 16:15

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, 16:17

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, 16:38

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

Alberto

robbo · May 1, 2008, 17:09

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

June 9, 2007, 13:51	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

June 10, 2007, 12:15	I just checked and the issue c	#6
alberto Senior Member Alberto Passalacqua Join Date: Mar 2009 Location: Ames, Iowa, United States Posts: 1,912 Rep Power: 36	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 Passalacqua GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM - An open-source implementation of quadrature-based moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using.

June 10, 2007, 13:37	Yes, I checked too. With dt =	#9
alberto Senior Member Alberto Passalacqua Join Date: Mar 2009 Location: Ames, Iowa, United States Posts: 1,912 Rep Power: 36	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 Passalacqua GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM - An open-source implementation of quadrature-based moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using.

June 10, 2007, 13:47	Exactly. It's not clear why we	#12
alberto Senior Member Alberto Passalacqua Join Date: Mar 2009 Location: Ames, Iowa, United States Posts: 1,912 Rep Power: 36	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 Passalacqua GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM - An open-source implementation of quadrature-based moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using.

June 10, 2007, 15:45	I opened a bug-report, so that	#13
alberto Senior Member Alberto Passalacqua Join Date: Mar 2009 Location: Ames, Iowa, United States Posts: 1,912 Rep Power: 36	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 Passalacqua GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM - An open-source implementation of quadrature-based moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using.

June 9, 2007, 14:45	Courant Number mean: 1.77239e+	#2
msrinath80 Senior Member Srinath Madhavan (a.k.a pUl\|) Join Date: Mar 2009 Location: Edmonton, AB, Canada Posts: 703 Rep Power: 21	Courant Number mean: 1.77239e+19 max: 1.46681e+23 That clearly indicates divergence.

June 9, 2007, 15:09	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

June 10, 2007, 08:09	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?

June 10, 2007, 08:20	Give it some time. There is a	#5
msrinath80 Senior Member Srinath Madhavan (a.k.a pUl\|) Join Date: Mar 2009 Location: Edmonton, AB, Canada Posts: 703 Rep Power: 21	Give it some time. There is a workshop in progress. Folks are busy. I'm sure someone will respond.

June 10, 2007, 12:28	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!

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

June 10, 2007, 13:39	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..

June 10, 2007, 13:44	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

June 10, 2007, 16:15	This is an error in case setup	#14
hjasak Senior Member Hrvoje Jasak Join Date: Mar 2009 Location: London, England Posts: 1,907 Rep Power: 33	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

June 10, 2007, 16:17	Sorry, slight imprecision: the	#15
hjasak Senior Member Hrvoje Jasak Join Date: Mar 2009 Location: London, England Posts: 1,907 Rep Power: 33	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

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

June 10, 2007, 16:38	Thanks! I attached the correct	#16
alberto Senior Member Alberto Passalacqua Join Date: Mar 2009 Location: Ames, Iowa, United States Posts: 1,912 Rep Power: 36	Thanks! I attached the correct tutorial to the bug section. Alberto __________________ Alberto Passalacqua GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM - An open-source implementation of quadrature-based moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using.

May 1, 2008, 17:09	I've experienced the same prob	#17
robbo New Member Roberto Join Date: Mar 2009 Posts: 17 Rep Power: 17	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