
[Sponsors] 
chtMultiRegionSimpleFoam case crashes on first time step 

LinkBack  Thread Tools  Search this Thread  Display Modes 
September 27, 2017, 09:47 
chtMultiRegionSimpleFoam case crashes on first time step

#1 
Member
Marc
Join Date: May 2017
Posts: 39
Rep Power: 6 
Hi,
I'm trying to run a conjugate heat transfer case with the chtMultiRegionSimpleFoam solver in OpenFOAM 4.1. The geometry of the problem can be seen in the attached image. The red region corresponds to the solid (named schwarzP) and the blue region is the fluid (named boolean). The solid is hot and cold fluid flows through it, heating up in the process. After doing checkMesh, there appears too be no errors in the geometry. However, after running the solver, the output is the following: Code:
Time = 1 Solving for fluid region boolean #0 Foam::error::printStack(Foam::Ostream&) at ??:? #1 Foam::sigFpe::sigHandler(int) at ??:? #2 ? in "/lib/x86_64linuxgnu/libc.so.6" #3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) at ??:? #4 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::operator/<Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&, Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&) at ??:? #5 Foam::fluidThermo::nu() const at ??:? #6 Foam::laminar<Foam::ThermalDiffusivity<Foam::CompressibleTurbulenceModel<Foam::fluidThermo> > >::nuEff() const at ??:? #7 Foam::linearViscousStress<Foam::ThermalDiffusivity<Foam::CompressibleTurbulenceModel<Foam::fluidThermo> > >::divDevRhoReff(Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>&) const at ??:? #8 ? at ??:? #9 __libc_start_main in "/lib/x86_64linuxgnu/libc.so.6" #10 ? at ??:? Floating point exception (core dumped) In case any CFD/OpenFOAM hero would like to lend a hand, I have uploaded my case here (it is only 0.8Mb and runs in a minute by executing the runCase file). Thank you! 

September 27, 2017, 22:43 

#2 
New Member

I've tested the folder case, and I think the error comes from boundary or initial condition.
In my computer, I'm using OpenFOAM dev, it said: Code:
Time = 1 Solving for fluid region boolean > FOAM FATAL ERROR: PBiCG has failed to converge within the maximum number of iterations 1000 Please try the more robust PBiCGStab solver. From function virtual Foam::solverPerformance Foam::PBiCG::solve(Foam::scalarField&, const scalarField&, Foam::direction) const in file matrices/lduMatrix/solvers/PBiCG/PBiCG.C at line 214. FOAM exiting Code:
Time = 1 Solving for fluid region boolean DILUPBiCGStab: Solving for Ux, Initial residual = nan, Final residual = nan, No Iterations 1001 http://openfoamwiki.net/index.php/Ge...__planeWall2D 

September 28, 2017, 03:45 

#3 
Member
Marc
Join Date: May 2017
Posts: 39
Rep Power: 6 
It looks like the error in OpenFOAM dev gives more insight towards the source of the problem than the error output I posted.
I will check all my BC's specially for the velocity field and lower the tolerances to see if the solver starts running. Thank you for your advice, I will report back soon. On the other hand, I did try the planeWall2D (and many other cht tutorials I found) and used it as a template to build my case. However, this particular one did not run for me. I actually started a thread on this here but I got no replies as of yet. 

September 28, 2017, 07:21 

#4 
Super Moderator

Hi all,
the error messages you both get should be related to a nonsense setups. The iteration amount of 1001 (or crash  segmentation fault) is normally the sign of nonphysical boundary conditions and/or sometimes a bad mesh. Changing the matrix solver should not solve your problem. Only and only if, it is related to a very bad initial guess but I would bet that this is not the case and the solver will crash too ... however, I have the experience with the chtSolver, that this one was sill buggy in the previous versions (even in Dev). I made a case 4 days ago and run it @home  no problem. Then I sent it to my office to let it run on the cluster with the outcome of segmentation fault error. Unfortunately, I had no time to compare the Dev versions but the local on my home computer was one pulled 1 week ago while the one at my office was 2 month old. After updating foam the error was gone too. Therefore, keep in mind that the dev Repo always includes the latest bugfixes and features. It can happen that dev solves the equations differently or some model works differently and thus some problem you focus on does not exist anymore and the solver runs.
__________________
Keep foaming, Tobias Holzmann Last edited by Tobi; September 28, 2017 at 08:34. 

September 28, 2017, 08:23 

#5 
New Member

Here I attach sample case for chtMultiRegionSimpleFoam:
https://www.dropbox.com/s/mrw8c7ll96...dOnly.rar?dl=0 I've tested it in OpenFOAM dev and it works well. The simulation run heat conduction between two bodies with fixed temperature at two faces (hot and cold). I set the same thermophysical properties of the bodies, so can compare the result with laplacianFoam for further validation. Hope this help you troubleshooting the problem. 

September 28, 2017, 08:37 

#6 
Super Moderator

Hi all,
I changed my reply a bit and want to refer to this bug report: https://bugs.openfoam.org/view.php?id=2663 and the related commit: https://github.com/OpenFOAM/OpenFOAM...9a73241ba3a832 which caused my problem.
__________________
Keep foaming, Tobias Holzmann 

October 4, 2017, 04:13 

#7 
Member
Marc
Join Date: May 2017
Posts: 39
Rep Power: 6 
Thank you Ali and Tobias,
The problem was indeed an initial condition issue: I changed the velocity at fluidsolid interphase to noSlip and pressure conditions' fixed values to nozero constants (for instance 1 atm) and now the case runs smoothly. Nevertheless, I would like to ask you about the latter. It was my understanding that pressure was nonphysical (i.e. only pressure differences matter) and therefore I could define any constant value for the initial condition. However, in testing this problem I found that changing the initial condition from say p=1 to p=100000 changed the solution completely. How can I go about understanding this? Thank you 

October 4, 2017, 04:31 

#8 
Super Moderator

Hi,
you have to distinguish between incompressible and compressible solvers. In incompressible solvers, the density is a constant value. Thus we can put it out of the derivatives and the pressure becomes the units p/rho. However, you see that we do not evaluate the density in that case (we do not need e.g. the ideal gas law or something similar). For compressible treatments, rho is not a constant and we have to calculate it (e.g. using the ideal gas law). The pressure in the compressible solvers have the normal units [Pa]. If you now model the compressible case by your assumption that only the pressure gradient is of interest and you set your pressure to 1 Pa, you can imagine how the density of your fluid is evaluated. If the setup is too unphysical, the solver cannot handle it and blow up; I guess in your case the density should get very large. Further information of the mathematical point of view is given here: https://www.cfdonline.com/Forums/op...openfoam.html I hope I explained it in an appropriate way. Otherwise just let me know. An additional hint: you are using chtMultiRegionSimpleFoam which is a compressible solver. You can check it out if you have a transportProperties file (in general for incompressible solvers) or a thermodynamicProperties file (for compressible solvers).
__________________
Keep foaming, Tobias Holzmann 

October 4, 2017, 04:52 

#9 
Member
Marc
Join Date: May 2017
Posts: 39
Rep Power: 6 
Thanks for the quick reply!
I was so used to working with incompressible solvers that I didn't think about it, now it is really obvious. But, if the solver computes the density, how can I extract it for postprocessing? By the way I used your book a couple of times and it is pretty amazing, you did a great contribution to the OpenFOAM community. 

October 4, 2017, 06:10 

#10 
Super Moderator

The density field is calculated in the thermodynamic library. E.g. rhoThermo.C. However, the write option in the thermodynamic classes are in general set toIOobject::NO_WRITE and thus the field is not written. Maybe there is a function library you can use with the program postProcess. The way I would do it out of the box is to build a new field in the solver and save it. E.g. buoyantPimpleFoam:
Code:
// CreateFields.H volScalarField myRho ( IOobject ( "rho" . . IOobject::NO_READ, IOobject::AUTO_WRITE ), mesh ); . . . // After updating the thermodynamic (pEqn.H) myRho = thermo>rho(); I guess there are easier ways e.g. functionObjects but out of the box I cannot give you an example. Another solution could be: Code:
volScalarField& myRho = thermo>rho() // Changing the write option of the object somehow myRho.foobar // Or write the object manuelly if (runTime.write()) { myRho.write(); }
__________________
Keep foaming, Tobias Holzmann 

May 6, 2021, 10:48 

#11 
New Member
WY
Join Date: Mar 2020
Posts: 11
Rep Power: 3 
Hi Tobias, I have the same error "PBiCG has failed to converge within the maximum number of iterations 1000. Please try the more robust PBiCGStab solver." when using pisoFoam to solve an unsteady and incompressible case (3D flow over cylinder). The question is that the case can run smoothly when using icoFoam, but it crashed after running 180000 steps when using pisoFoam with same settings except for adding the standard kepsilon turbulence model. So I suppose the initial condition, the boundary condition and also the mesh are Ok because it can run with icoFoam. But I don't know why pisoFocam failed to solve it. I would be very appreciated if you can give me some help!


Tags 
chtmultiregionsimpefoam, heat and mass transfer, openfoam 4.1 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
[DesignModeler] DesignModeler Scripting: How to get Full Command Access  ANT  ANSYS Meshing & Geometry  53  February 16, 2020 15:13 
courant number increases to rather large values  6863523  OpenFOAM Running, Solving & CFD  21  November 10, 2019 10:14 
Extrusion with OpenFoam problem No. Iterations 0  Lord Kelvin  OpenFOAM Running, Solving & CFD  8  March 28, 2016 11:08 
Star cd esice solver error  ernarasimman  STARCD  2  September 12, 2014 00:01 
Micro Scale Pore, icoFoam  gooya_kabir  OpenFOAM Running, Solving & CFD  2  November 2, 2013 13:58 