|
[Sponsors] |
Problem with running chtMultiRegionFoam after using setSet utility |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
November 19, 2009, 06:24 |
Problem with running chtMultiRegionFoam after using setSet utility
|
#1 |
New Member
Victor Fleischer
Join Date: Nov 2009
Posts: 21
Rep Power: 17 |
Hi at all,
as a Open-FOAM-beginner, i tried to use chtMultiregionFoam-solver as it is used in the HeatTransfer Tutorial Case. In my case,there is a part in the middle of the body that is cut out by the setSet utility in order to simulate a solid. After running blockMesh, setSet, setsToTones, splitMeshRegions without any errors the case allways stops,when running the chtMultiRegionFoam solver: /OpenFOAM-1.6/bin/tools/RunFunctions: line 38: 615 Aborted $APP_RUN $* > log.$APP_NAME 2>&1 the log-file: /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.6 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : 1.6-f802ff2d6c5a Exec : chtMultiRegionFoam Date : Nov 19 2009 Time : 10:34:59 Host : pag PID : 615 Case : /nfs/home/fleischer/OpenFOAM/fleischer-1.6/run/Tube1/Test2_4 nProcs : 1 SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create fluid mesh for region Fluid for time = 0.0001 Create solid mesh for region Stack for time = 0.0001 *** Reading fluid mesh thermophysical properties for region Fluid Adding to thermoFluid Selecting thermodynamics package hPsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>> Adding to rhoFluid Adding to KFluid Adding to UFluid Adding to phiFluid Adding to gFluid Adding to turbulence Selecting turbulence model type laminar Adding to DpDtFluid *** Reading solid mesh thermophysical properties for region Stack Adding to rhos Adding to cps Adding to Ks Adding to Ts Region: Fluid Courant Number mean: 6.9363e-05 max: 0.00600006 Region: Fluid Courant Number mean: 6.9363e-05 max: 0.00600006 request for objectRegistry region0 from objectRegistry Test2_4 failed available objects of type objectRegistry are 2 ( Stack Fluid ) #0 Foam::error:rintStack(Foam::Ostream&) in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so" #1 Foam::error::abort() in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so" #2 Foam::Ostream& Foam:perator<< <Foam::error>(Foam::Ostream&, Foam::errorManip<Foam::error>) in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/applications/bin/linux64GccDPOpt/chtMultiRegionFoam" #3 Foam:bjectRegistry const& Foam:bjectRegistry::lookupObject<Foam:bjectReg istry>(Foam::word const&) const in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so" #4 Foam::OutputFilterFunctionObject<Foam:robes>::st art() in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libsampling.so" #5 Foam::functionObjectList::read() in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so" #6 Foam::Time:perator++() in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so" #7 main in "/nfs/public/SI/Holzinger/OFTest/OpenFOAM/OpenFOAM-1.6/applications/bin/linux64GccDPOpt/chtMultiRegionFoam" #8 __libc_start_main in "/lib64/libc.so.6" #9 _start at /usr/src/packages/BUILD/glibc-2.9/csu/../sysdeps/x86_64/elf/start.S:116 From function objectRegistry::lookupObject<Type>(const word&) const in file db/objectRegistry/objectRegistryTemplates.C at line 140. FOAM aborting Does anybody know where this problem comes from? You'll find the packed Case in the attachment |
|
November 19, 2009, 07:40 |
|
#2 |
New Member
J H
Join Date: Mar 2009
Location: Germany
Posts: 20
Rep Power: 17 |
Hi Victor
I havent looked in your case but I would say there is something wrong with your coupled regions. Did you customize them? (for example in 0.001/T) |
|
November 19, 2009, 08:10 |
|
#3 |
New Member
J H
Join Date: Mar 2009
Location: Germany
Posts: 20
Rep Power: 17 |
no thats not
|
|
November 19, 2009, 08:22 |
|
#4 |
New Member
Victor Fleischer
Join Date: Nov 2009
Posts: 21
Rep Power: 17 |
Hi kawuppdich,
i have already looked at the boundary conditions for several times and cannot find any problem. And all log-files don't show any errors. So I don't know why there is a message "request for objectRegistry region0" in the chtMultiRegionFoam!? I searched for similar problems, but there are only problems like "request for uniformDimensionedVectorField g from objectRegistry region0 failed"!? |
|
November 19, 2009, 08:26 |
|
#5 |
New Member
J H
Join Date: Mar 2009
Location: Germany
Posts: 20
Rep Power: 17 |
the problem is there is no region0. normaly it should be fluid or Stack. I donīt know where it comes from. I had the same error and my problem was that iīve forgot to customize the boundary
|
|
November 19, 2009, 08:46 |
|
#6 |
New Member
J H
Join Date: Mar 2009
Location: Germany
Posts: 20
Rep Power: 17 |
all looks fine but same error here
|
|
November 19, 2009, 09:32 |
|
#7 |
New Member
Victor Fleischer
Join Date: Nov 2009
Posts: 21
Rep Power: 17 |
hmm, i don't find it either....
But thanks a lot for your helpkawuppdich!! |
|
November 23, 2009, 08:26 |
|
#8 |
New Member
Victor Fleischer
Join Date: Nov 2009
Posts: 21
Rep Power: 17 |
I have an idea where the problem could come from. After setting up a similar case with setSet, setsToZones,splitMeshRegions for the chtMultiregionFoam everything worked fine.
But when i tried to use the probes() function the problem we discussed above ocurred again. Does anybody know if this could be the reason? Or does anybody know an alternative for the probes() function without saving the whole data accumulated during the simulation? here the additional part of the controlDict-File: functions { probesTest { // Type of functionObject type probes; // Where to load it from (if not already in solver) functionObjectLibs ("libsampling.so"); outputControl timeStep; outputInterval 1; // Locations to be probed. runTime modifiable! probeLocations ( ( -0.05 0 0) ( -0.04 0 0) ( -0.03 0 0) ( -0.02 0 0) ( -0.01 0 0) ( 0.00 0 0) ( 0.01 0 0) ( 0.02 0 0) ( 0.03 0 0) ( 0.04 0 0) ( 0.05 0 0) ); // Fields to be probed. runTime modifiable! fields ( rho p U T ); } }; |
|
June 30, 2010, 09:36 |
|
#9 |
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 |
Just for information: Victor missed one keyword:
Code:
functions { probesTest { // Type of functionObject type probes; // Where to load it from (if not already in solver) functionObjectLibs ("libsampling.so"); outputControl timeStep; outputInterval 1; region heater; // Locations to be probed. runTime modifiable! probeLocations ( ( -0.05 0 0) ( -0.04 0 0) ( -0.03 0 0) ( -0.02 0 0) ( -0.01 0 0) ( 0.00 0 0) ( 0.01 0 0) ( 0.02 0 0) ( 0.03 0 0) ( 0.04 0 0) ( 0.05 0 0) ); // Fields to be probed. runTime modifiable! fields ( rho p U T ); } }; Hope this help someone, mad |
|
July 1, 2010, 08:30 |
|
#10 | |
Member
Robertas N.
Join Date: Mar 2009
Location: Kaunas, Lithuania
Posts: 53
Rep Power: 17 |
Quote:
Stack_to_Fluid { ... sampleRegion region0; samplePatch ... ... } Change these entries to be Stack_to_Fluid { ... sampleRegion Fluid; samplePatch Fluid_to_Stack; ... } Analogously, in 0.001/Fluid/polyMesh/boundary, there must be this entry: Fluid_to_Stack { ... sampleRegion Stack; samplePatch Stack_to_Fluid; ... } i.e., 'polyMesh/boundary' files of each region contain entries for neighbouring regions and neighbouring patches. |
||
September 10, 2012, 10:30 |
|
#11 | |
Senior Member
|
Quote:
I had the very same problem and it seems to be solved by now! (Testing the tool, but looking good!) Cheers, Bernhard |
||
March 22, 2023, 20:41 |
|
#12 |
Senior Member
Desh
Join Date: Mar 2021
Location: Sydney
Posts: 118
Rep Power: 5 |
Hi,
I am running into the same problem but trying to calculate 'wallHeatFlux' from the 'topSolid' region in the patch called ' maxZ'. OpenFOAM version is 10. my 'wallHeatFlux' function looks like Code:
/*--------------------------------*- C++ -*----------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 10 \\/ M anipulation | \*---------------------------------------------------------------------------*/ FoamFile { format ascii; class dictionary; location "system"; object sample; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // type surfaces; //sets; //surfaces functionObjectLibs ("libsampling.so"); region topSolid; //libs ("fieldFunctionObjects"); //region topSolid; writeControl writeTime; interpolationScheme cellPointFace; setFormat raw; //vtk fields ( wallHeatFlux ); //U p surfaces ( surfaces1 { type plane; patchName maxZ; } ); PHP Code:
Thanks, Dasith |
|
March 24, 2023, 01:01 |
|
#13 |
Senior Member
Desh
Join Date: Mar 2021
Location: Sydney
Posts: 118
Rep Power: 5 |
found the answer at
HTML Code:
https://www.cfd-online.com/Forums/openfoam-solving/248597-wallheatflux-openfoam-version-10-a.html |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
RSH problem for parallel running in CFX | Nicola | CFX | 5 | June 18, 2012 19:31 |
Problem setting with chtmultiregionFoam | Antonin | OpenFOAM | 10 | April 24, 2012 10:50 |
Problem running paraFoam on OpenFOAM 1.5 | sonny | OpenFOAM | 3 | June 6, 2009 21:24 |
Statically Compiling OpenFOAM Issues | herzfeldd | OpenFOAM Installation | 21 | January 6, 2009 10:38 |
problem in running FoamX in Open FOAM | Gaurav | Main CFD Forum | 3 | May 10, 2006 06:06 |