View Issue Details

Jump to NotesJump to History
IDProjectCategoryView StatusDate SubmittedLast Update
0003110OpenFOAMBugpublic2018-11-15 11:332018-11-15 13:16
Reportersdorof Assigned Towill  
PrioritynormalSeverityminorReproducibilityhave not tried
Status closedResolutionno change required 
Summary0003110: chtMultiRegionFoam crashes in SIMPLE mode
DescriptionAs said https://github.com/OpenFOAM/OpenFOAM-dev/commit/283f8b7dc8873e3c0352c23144cb6dfcb7ca26d9
since OF6, the chtMultiRegionFoam solver can operate in SIMPLE mode and chtMultiRegionSimpleFoam deprecated.

I attached a test-case which runs with OF5 chtMultRegoinSimpleFoam but crashes with OF6 chtMultiRegionFoam.
The case consists just single region with 1D solid rod with uniform temperature and zeroGradient BC. When runing with OF6 chtMultiRegionFoam, it crashes with negative temperature values:

--> FOAM FATAL ERROR:
Negative initial temperature T0: -1174.56

    From function Foam::scalar Foam::species::thermo<Thermo, Type>::T(Foam::scalar, Foam::scalar, Foam::scalar, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar) const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar) const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar) const) const [with Thermo = Foam::hConstThermo<Foam::rhoConst<Foam::specie> >; Type = Foam::sensibleEnthalpy; Foam::scalar = double; Foam::species::thermo<Thermo, Type> = Foam::species::thermo<Foam::hConstThermo<Foam::rhoConst<Foam::specie> >, Foam::sensibleEnthalpy>]
    in file /home/sdorof/OpenFOAM/OpenFOAM-6/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 54.

FOAM aborting

#0 Foam::error::printStack(Foam::Ostream&) at ??:?
#1 Foam::error::abort() at ??:?
#2 Foam::heSolidThermo<Foam::solidThermo, Foam::pureMixture<Foam::constIsoSolidTransport<Foam::species::thermo<Foam::hConstThermo<Foam::rhoConst<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() at ??:?
#3 Foam::heSolidThermo<Foam::solidThermo, Foam::pureMixture<Foam::constIsoSolidTransport<Foam::species::thermo<Foam::hConstThermo<Foam::rhoConst<Foam::specie> >, Foam::sensibleEnthalpy> > > >::correct() at ??:?
#4 ? at ??:?
#5 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#6 ? at ??:?


but with OF5 chtMultiRegionSimpleFoam its operates normally:

Time = 100


Solving for solid region solid
DICPCG: Solving for h, Initial residual = 0.29982, Final residual = 2.96367e-17, No Iterations 1
Min/max T:300 300

Regions not converged after 100 iterations
ExecutionTime = 0.03 s ClockTime = 0 s

End
TagsNo tags attached.

Activities

sdorof

2018-11-15 11:33

reporter  

test.zip (17,533 bytes)

will

2018-11-15 13:16

manager   ~0010186

That case has no meaning in steady state and only functions in 5.x because you are under-relaxing h. You are not under-relaxing in 6/dev. Note the commit message:

    In addition, additional "<variable>Final" solver
    and relaxation entries will be needed. For a steady case, adding a
    wildcard ending, ".*", to the variable names should be sufficient.

    ...

    relaxationFactors
    {
        fields
        {
            "p_rgh.*" 0.7;
        }
        equations
        {
            "U.*" 0.5;
            "(h|e).*" 0.3;
            "(k|epsilon).*" 0.2;
        }
    }

Issue History

Date Modified Username Field Change
2018-11-15 11:33 sdorof New Issue
2018-11-15 11:33 sdorof File Added: test.zip
2018-11-15 13:16 will Assigned To => will
2018-11-15 13:16 will Status new => closed
2018-11-15 13:16 will Resolution open => no change required
2018-11-15 13:16 will Note Added: 0010186