Thanks Mattijs, I post the pro
Thanks Mattijs, I post the problem here.
I have ran a case with two meshes, which are located in: -case/constant/region1/polyMesh and -case/constant/region2/polyMesh I tried to postprocess the results using foamToVTK: - foamToVTK . <casename> -mesh region1 Then the following ERROR apears: << Create mesh for time = constant --> FOAM FATAL ERROR : Cannot find file "points" in directory "constant/polyMesh" From function Time::findInstance(const word& dir, const word& name) in file db/Time/findInstance.C at line 133. FOAM exiting >> The point, is that the file "points" exist but in "constant/region1/polyMesh" and"constant/region2/polyMesh". I'm using OpenFOAM 1.4. I would appreciate any idea to solve the problem Thanks in advance. María. |
Bit of a regression bug. In po
Bit of a regression bug. In postProcessing/dataConversion/foamToVTK/foamToVTK.C
replace # include "createMesh.H" with Info<< "Create mesh for time = " << runTime.timeName() << nl << endl; fvMesh mesh ( IOobject ( meshName, runTime.timeName(), runTime, IOobject::MUST_READ ) ); and recompile (wclean; wmake) |
Hi!
Thanks Mattijs. We have
Hi!
Thanks Mattijs. We have changed what you recommend me with some modifications. Now it works. We replaced: # include "createMesh.H" with: Info<<"Create mesh for time="<< runTime.timeName()<<nl<<endl; fvMesh mesh ( IOobject ( meshName, meshDir, //runTime.timeName(), runTime, IOobject::MUST_READ ) ); Where meshDir is as follows: word meshDir = runTime.timeName(); if (args.options().found("mesh")) { meshName = args.options()["mesh"]; fvPath = fvPath/meshName; meshDir.append("/"); meshDir.append(meshName); } Thanks! María |
Hi Mattijs
Just as new user
Hi Mattijs
Just as new user of OpenFoam, would you please let me know, where should i go to find the postProcessing/dataConversion/foamToVTK/foamToVTK.C ? and provide changes? I have the same problem as: -> FOAM FATAL ERROR : Cannot find file "points" in directory "constant/polyMesh" From function Time::findInstance(const word& dir, const word& name) in file db/Time/findInstance.C at line 133. FOAM exiting I read your suggestion to solve this problem and i would please to ask you about that matter. Many Thanks |
>where should i go to find
>where should i go to find
cd $WM_PROJECT_INST_DIR find . -name foamToVTK.C Or http://foam.sourceforge.net/doc/Guides-a4/UserGuide.pdf section 3.6 This problem is fixed in 1.4.1. |
Dear Mattijs
Appreciat abou
Dear Mattijs
Appreciat about your answer. sorry for delay to send a feedback of your command . Many Thanks Armin |
All times are GMT -4. The time now is 20:52. |