|
[Sponsors] |
April 22, 2013, 03:57 |
simpleFoam error
|
#1 |
New Member
Nik
Join Date: May 2012
Posts: 5
Rep Power: 13 |
Hi all,
I am beginner in OpenFoam and have been through some tutorials. I have been also looking at the user guide but I am unable to understand the error OpenFoam has been throwing at me. Few details of my problem setup: Openfoam 2.0.v4 and 2.1.0 Solver simpleFoam using in serial mode its a flow around a block case. I believe it is something like "My guess is that this is (again) the old "I set k/epsilon/omega to 0 in the initial conditions (or on a boundary) and the turbulence model divides by it"-problem" linked at http://www.cfd-online.com/Forums/ope...-parallel.html I have added the error below: /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.1.0 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : 2.1.0-bd7367f93311 Exec : simpleFoam Date : Apr 22 2013 Time : 15:53:37 Host : "hpclogin1" PID : 9930 Case : /gpfs/home/ngarg/ngarg/OpenFOAM/buildings/building_simple nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Disallowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 Reading field p Reading field U #0 Foam::error:rintStack(Foam::Ostream&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 __restore_rt at sigaction.c:0 #3 __ieee754_log at interp.c:0 #4 log in "/lib64/libm.so.6" #5 Foam::incompressible::atmBoundaryLayerInletVelocit yFvPatchVectorField::updateCoeffs() in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so" #6 Foam::incompressible::atmBoundaryLayerInletVelocit yFvPatchVectorField::atmBoundaryLayerInletVelocity FvPatchVectorField(Foam::fvPatch const&, Foam:imensionedField<Foam::Vector<double>, Foam::volMesh> const&, Foam::dictionary const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so" #7 Foam::fvPatchField<Foam::Vector<double> >::adddictionaryConstructorToTable<Foam::incompres sible::atmBoundaryLayerInletVelocityFvPatchVectorF ield>::New(Foam::fvPatch const&, Foam:imensionedField<Foam::Vector<double>, Foam::volMesh> const&, Foam::dictionary const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so" #8 Foam::fvPatchField<Foam::Vector<double> >::New(Foam::fvPatch const&, Foam:imensionedField<Foam::Vector<double>, Foam::volMesh> const&, Foam::dictionary const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/simpleFoam" #9 Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::GeometricB oundaryField(Foam::fvBoundaryMesh const&, Foam:imensionedField<Foam::Vector<double>, Foam::volMesh> const&, Foam::dictionary const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/simpleFoam" #10 Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>::readField(Foam::dictionary const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/simpleFoam" #11 Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>::readField(Foam::Istream&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/simpleFoam" #12 Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>::GeometricField(Foam::IOobject const&, Foam::fvMesh const&) in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/simpleFoam" #13 main in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/simpleFoam" #14 __libc_start_main in "/lib64/libc.so.6" #15 Foam::regIOobject::writeObject(Foam::IOstream::str eamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/usr/local/OpenFOAM/OpenFOAM-2.1.0/platforms/linux64GccDPOpt/bin/simpleFoam" Floating point exception I would appreciate if someone can help me with this. It seems to me that my boundary conditions are not correctly set. Cheers Nikhil Last edited by nikkuoa; April 22, 2013 at 10:43. |
|
April 22, 2013, 13:21 |
|
#2 |
Senior Member
Lieven
Join Date: Dec 2011
Location: Leuven, Belgium
Posts: 299
Rep Power: 22 |
Hi Nikhil,
The problem is due to a division by 0 in the atmBoundaryLayerInletVelocity boundary condition. Can you post the content of the 0/U file? Then we can check your settings. Cheers, L |
|
April 22, 2013, 23:16 |
|
#3 |
New Member
Nik
Join Date: May 2012
Posts: 5
Rep Power: 13 |
Hi L,
Thanks for your reply. I have posted the contents of 0/U here: /*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.0.0 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volVectorField; location "0"; object U; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // #include "include/ABLConditions" dimensions [0 1 -1 0 0 0 0]; internalField uniform (5 0 0); boundaryField { inlet { type atmBoundaryLayerInletVelocity; Uref $Uref; Href $Href; n $windDirection; z $zDirection; z0 $z0; value $internalField; zGround $zGround; } outlet { type inletOutlet; inletValue uniform (0 0 0); value $internalField; } "buildings" { type fixedValue; value uniform (0 0 0); } bottom { type fixedValue; value uniform (0 0 0); } #include "include/sideAndTopPatches" } // ************************************************** *********************** // Also, I have encountered some interesting things. I managed to run the same case with uniform input velocity but when i try to run with atmBoundaryLayerVelocity i ran into some different error. /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.1.0 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : 2.1.0-bd7367f93311 Exec : potentialFoam -noFunctionObjects -writep Date : Apr 23 2013 Time : 10:59:13 Host : "hpclogin1" PID : 24801 Case : /gpfs/home/ngarg/ngarg/OpenFOAM/buildings/building_simple nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Disallowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 Reading field p Reading field U --> FOAM FATAL IO ERROR: Unknown patchField type atmBoundaryLayerInletVelocity for patch type patch Valid patchField types are : 59 ( SRFFreestreamVelocity SRFVelocity activeBaffleVelocity activePressureForceBaffleVelocity advective calculated codedFixedValue codedMixed cyclic cyclicAMI cyclicSlip cylindricalInletVelocity directionMixed empty fixedGradient fixedInternalValue fixedNormalSlip fixedValue flowRateInletVelocity fluxCorrectedVelocity freestream inletOutlet mapped mappedField mappedFixedInternalValue mappedFixedPushedInternalValue mappedFlowRate mappedVelocityFlux mixed movingWallVelocity nonuniformTransformCyclic oscillatingFixedValue outletInlet outletMappedUniformInlet partialSlip pressureDirectedInletOutletVelocity pressureDirectedInletVelocity pressureInletOutletParSlipVelocity pressureInletOutletVelocity pressureInletUniformVelocity pressureInletVelocity pressureNormalInletOutletVelocity processor processorCyclic rotatingPressureInletOutletVelocity rotatingWallVelocity sliced slip supersonicFreestream surfaceNormalFixedValue swirlFlowRateInletVelocity symmetryPlane timeVaryingMappedFixedValue translatingWallVelocity turbulentInlet uniformFixedValue waveTransmissive wedge zeroGradient ) file: /gpfs/home/ngarg/ngarg/OpenFOAM/buildings/building_simple/0/U::boundaryField::inlet from line 28 to line 16. From function fvPatchField<Type>::New(const fvPatch&, const DimensionedField<Type, volMesh>&, const dictionary&) in file /usr/local/OpenFOAM/OpenFOAM-2.1.0/src/finiteVolume/lnInclude/fvPatchFieldNew.C at line 135. FOAM exiting |
|
April 22, 2013, 23:37 |
problem with atmBoundaryLayerVelocity conditions in inlet
|
#4 |
New Member
Nik
Join Date: May 2012
Posts: 5
Rep Power: 13 |
Hi everyone,
As posted previously, I removed the atmBoundaryLayerVelocity from inlet and then the simulation worked, so I am thinking that this conditions is stopping the simulation from working. I am still trying to figure out how to sort this matter. If anyone has experience, i would really appreciate help Cheers nikhil |
|
April 23, 2013, 03:02 |
|
#5 |
Senior Member
Lieven
Join Date: Dec 2011
Location: Leuven, Belgium
Posts: 299
Rep Power: 22 |
Ok, can you also post the "include/ABLConditions" file?
The second error is easy to explain, potentialFoam does not know turbulence models and the atmBoundaryLayerInletVelocity is provided by the RAS models. So in short, potentialFoam will complain that he doesn't know the condition (and then he prints out what he prints out the ones he does know). Cheers, L |
|
April 23, 2013, 03:07 |
ABLConditions file
|
#6 |
New Member
Nik
Join Date: May 2012
Posts: 5
Rep Power: 13 |
I have provided the ABLconditions file
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.0.0 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Ustar 0.82; Uref 10.0; Href 20; z0 0.1; turbulentKE 1.3; windDirection (1 0 0); zDirection (0 0 1); zGround uniform 935.0; // ************************************************** *********************** // Thanks Nikhil |
|
April 23, 2013, 04:06 |
|
#7 |
Senior Member
Lieven
Join Date: Dec 2011
Location: Leuven, Belgium
Posts: 299
Rep Power: 22 |
Why do you set zGround to 935 m? Is the z-coordinate of you bottom plane (the wall) really about 935 m?
If not, set it to 0.0 and try again... Cheers, L |
|
April 23, 2013, 12:56 |
|
#8 |
New Member
Nik
Join Date: May 2012
Posts: 5
Rep Power: 13 |
Thanks for your help. The solution worked, i feel so stupid as kept on thinking it to be geostrophic height.
Cheers Nikhil |
|
August 14, 2013, 04:12 |
|
#9 |
Senior Member
izna O'connor
Join Date: Jun 2013
Posts: 143
Rep Power: 12 |
hello Nik
Have you been able to run the case with the atmBoundaryLayerInletVelocity? I have exact error as you. |
|
June 22, 2018, 04:16 |
|
#10 |
Member
Join Date: Nov 2009
Posts: 43
Rep Power: 16 |
I'm using v2.4.0 and seem to be running into the same issue: potentialFoam does not recognize the atmBoundaryLayerInletVelocity boundary condition.
Has anyone gotten this to work? |
|
June 23, 2018, 07:07 |
|
#11 |
Senior Member
|
Hi,
potentialFoam (inviscid) can not sustain the atmospheric boundary layer, so it makes no sense to use it, probably also why it is not recognised by the solver. Furthermore it has to do with near surface turbulence as well, which is also not possible with potentialFoam. Regards, Tom |
|
June 25, 2018, 05:22 |
|
#12 |
Member
Join Date: Nov 2009
Posts: 43
Rep Power: 16 |
Thanks for the reply.
Yes, certainly. Inviscid flow is not useful for applications where ABLs are present. The idea here was just to initialise the flow field with a +- realistic field (hence trying potentialFoam). Also I thought that someone in the thread got it to work, hence my question. Cheers |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
c++ libraries and solver compiling | vaina74 | OpenFOAM Installation | 13 | February 3, 2012 17:43 |
[swak4Foam] groovyBC: problems compiling: "flex: not found" and "undefined reference to ..." | sega | OpenFOAM Community Contributions | 12 | February 17, 2010 09:30 |
Installation OF1.5-dev | ttdtud | OpenFOAM Installation | 46 | May 5, 2009 02:32 |
Problem with compile the setParabolicInlet | ivanyao | OpenFOAM Running, Solving & CFD | 6 | September 5, 2008 20:50 |
user defined function | cfduser | CFX | 0 | April 29, 2006 10:58 |