|April 20, 2010, 21:32||
settlingFoam fails with timeVarying conditions on U
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,907Rep Power: 27
settlingFoam fails when a timeVarying boundary condition is used for the U field, since Vdj inherits the boundaryField from U, leading the code to a segmentation fault when
I'm not sure why Vdj inherits the BC's from V, since it is computed explicitly. However a workaround could be to replace the declaration of Vdj in createFields.H with (I left the commented line).
volVectorField Vdj ( IOobject ( "Vdj", runTime.timeName(), mesh, IOobject::NO_READ, IOobject::AUTO_WRITE ), mesh, dimensionedVector("0.0", U.dimensions(), vector::zero) //,U.boundaryField().types() );
GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats.
OpenQBMM - An open-source implementation of quadrature-based moment methods.
To obtain more accurate answers, please specify the version of OpenFOAM you are using.
|April 21, 2010, 14:16||
Join Date: Sep 2009
Location: Buenos Aires
Posts: 36Rep Power: 9
The bug also exists for alpha BC, since Alpha inherits the boundaryField from alpha.
I tried a similar fix for this BC.
volScalarField Alpha ( IOobject ( "Alpha", runTime.timeName(), mesh, IOobject::NO_READ, IOobject::AUTO_WRITE ), alpha*rhod/rho //,alpha.boundaryField().types() );
But I get the next error message when trying to run the case:
volScalarField Alpha ( IOobject ( "Alpha", runTime.timeName(), mesh, IOobject::MUST_READ, IOobject::AUTO_WRITE ), mesh // alpha*rhod/rho //,alpha.boundaryField().types() );
It seems to work fine, but I had to manually calculate and create the Alpha bondaryField File in the 0 folder, and apply the timeVaryingUniformFixedValue to this BC instead of applying it to alpha.
P.S.: Note the difference between alpha and Alpha. Alpha= alpha*rhod/rho
Last edited by lfbarcelo; April 21, 2010 at 16:42. Reason: Found a solution
|Thread||Thread Starter||Forum||Replies||Last Post|
|Wind turbine simulation||Saturn||CFX||45||February 8, 2016 05:42|
|InterDyMFoam dynamic messing in parallel fails under nonquiescent conditions||adona058||OpenFOAM Running, Solving & CFD||5||August 19, 2010 11:47|
|InterDyMFoam dynamic meshing in parallel fails under nonquiescent conditions||adona058||OpenFOAM Bugs||7||November 18, 2008 15:58|
|Fluent accuracy and boundary conditions||Paolo Lampitella||FLUENT||0||June 12, 2008 06:25|
|A problem about setting boundary conditions||lyang||Main CFD Forum||0||September 19, 1999 18:29|