[MMRC]

Hi community,

I tried on OpenFOAM ESI 2012 run a RAS simulation using the set-up of A local time step (LTS) incompressible pimpleFoam solver, with localEuler in ddtSchemes and rDelta* numerics in fvSolution. The simulation prompt the error while trying tro finish 1st iteration of:

--> FOAM FATAL ERROR: (openfoam-2012)

    request for volScalarField rDeltaT from objectRegistry region0 failed
    available objects of type volScalarField are
7(nut fp pPrevIter k nu p epsilon)

    From const Type& Foam::objectRegistry::lookupObject(const Foam::word&, bool) const [with Type = Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>]
    in file /home/mmros/OpenFOAMv2012/OpenFOAM-v2012/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 463.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::exitOrAbort(int, bool) at ??:?
#2  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const& Foam::objectRegistry::lookupObject<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> >(Foam::word const&, bool) const at ??:?
#3  Foam::fv::localEulerDdtScheme<Foam::Vector<double> >::fvmDdt(Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
#4  ? in ~/OpenFOAMv2012/OpenFOAM-v2012/platforms/linux64GccDPInt32Opt/bin/pimpleFoam
#5  ? in ~/OpenFOAMv2012/OpenFOAM-v2012/platforms/linux64GccDPInt32Opt/bin/pimpleFoam
#6  ? in /lib/x86_64-linux-gnu/libc.so.6
#7  __libc_start_main in /lib/x86_64-linux-gnu/libc.so.6
#8  ? in ~/OpenFOAMv2012/OpenFOAM-v2012/platforms/linux64GccDPInt32Opt/bin/pimpleFoam
Aborted (core dumped)

I checked how tutorials of LTS where set-up for this version, and none for incompressible-pimpleFoam solver was built, you can find for reactingFoam, rhoPimpleFoam and interFoam.



In comparison, OpenFOAM foundation does have tutorial for a incompressible pimplefoam case with LTS.



Can it be that these versions of OpenFOAM ESI (2012 and 2306) do not support LTS on incompressible pimpleFoam?

[Tobermory]

There must be something wrong with your set up.

1. Look in pimpleFoam.C, and on line 84 you will see:

#include "localEulerDdtScheme.H"

... so it is coded up in pimpleFoam.

2. Try copying the pitzDaily tutorial case, and change fvSchemes.ddtSchemes to localEuler - it runs just fine, with LTS.

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2112 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : _14aeaf8dab-20211220 OPENFOAM=2112 version=v2112
Arch : "LSB;label=32;scalar=64"
Exec : pimpleFoam
Date : Sep 08 2024
Time : 16:42:44
Host : Eddy
PID : 293898
I/O : uncollated
Case : /home/ian/OpenFOAM/ian-v2112/run/tmpLTS
nProcs : 1
trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20)
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0


PIMPLE: Operating solver in PISO mode

Using LTS
Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model type RAS
Selecting RAS turbulence model kEpsilon
RAS
{
RASModel kEpsilon;
turbulence on;
printCoeffs on;
Cmu 0.09;
C1 1.44;
C2 1.92;
C3 0;
sigmak 1;
sigmaEps 1.3;
}

No MRF models present

No finite volume options present
Courant Number mean: 0.000874894 max: 0.315889

Starting time loop

Flow time scale min/max = 0.000253254, 1e+15
Smoothed flow time scale min/max = 0.000253254, 0.0350751
Time = 0.0001

PIMPLE: iteration 1
smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 7.8432e-06, No Iterations 9
smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 6.42733e-06, No Iterations 11
GAMG: Solving for p, Initial residual = 1, Final residual = 0.00703477, No Iterations 13
time step continuity errors : sum local = 1.23849e-05, global = 2.79833e-06, cumulative = 2.79833e-06
GAMG: Solving for p, Initial residual = 0.0405227, Final residual = 6.93139e-08, No Iterations 27
time step continuity errors : sum local = 1.07654e-08, global = -2.63219e-09, cumulative = 2.7957e-06
smoothSolver: Solving for epsilon, Initial residual = 0.20423, Final residual = 8.56121e-06, No Iterations 48
smoothSolver: Solving for k, Initial residual = 1, Final residual = 8.83069e-06, No Iterations 44
ExecutionTime = 0.22 s ClockTime = 0 s

Flow time scale min/max = 1.28354e-05, 0.00614002
Smoothed flow time scale min/max = 1.28354e-05, 0.000460444
Time = 0.0002

[MMRC]

Originally Posted by Tobermory

There must be something wrong with your set up.

1. Look in pimpleFoam.C, and on line 84 you will see:

#include "localEulerDdtScheme.H"

... so it is coded up in pimpleFoam.

2. Try copying the pitzDaily tutorial case, and change fvSchemes.ddtSchemes to localEuler - it runs just fine, with LTS.

Big thanks Tobermory. I follow your recommendation and run pitzDaily. I found that the error keeps prompting when running OpenFOAM ESI 2012, whereas for V2306 it does not happen so pimpleFoam in this 'compressible tutorial' runs fine in LTS mode.

[MMRC]

I found that at pimpleFoam.C from OFV2012 there is no #include "localEulerDdtScheme.H" which is a header file found in path OpenFOAM-v2012/src/finiteVolume/finiteVolume/ddtSchemes/localEulerDdtScheme.
Another lack is the bool operation to check if case is LTS and then read the header file of setRDeltaT.H which is also no included in pimpleFoam/. So for this version, to enable incompressible LTS by pimpleFoam looks like there the source code has to be modified.

[Tobermory]

Originally Posted by MMRC

I found that at pimpleFoam.C from OFV2012 there is no #include "localEulerDdtScheme.H"

Aaah - my mistake, apologies - I read that as V2112!

As a shortcut, you could try to compile the version from v2112 as a local user solver in v2012, if you are stuck with running under v2012, and see if that compiles ...