|
[Sponsors] |
April 4, 2014, 11:46 |
InterFoam problems adjusting Mesh
|
#1 | |
New Member
Benjamin
Join Date: Apr 2014
Location: Zürich
Posts: 27
Rep Power: 12 |
Hey everyone!
I'm sorry if this has been asked before (I haven't found it so far), but I got Problems with the interFoam solver. You might remember the dam breaking tutorial from the OpenFoam User Guide. I completed it and then decided to extend it to a 3D case (I also had and still have to). I changed the original blockMesh to a longer rectangular volume, put a water column in one edge and started it. It worked well, but when I try to run it now (I don't think I have made any changes), the following error message appears: Quote:
Cheers, Benji PS: If you wish, I could also post some more Code.... Last edited by Benji; April 7, 2014 at 04:57. |
||
April 7, 2014, 05:02 |
|
#2 | |
New Member
Benjamin
Join Date: Apr 2014
Location: Zürich
Posts: 27
Rep Power: 12 |
Sorry for being annoying (I'm very new to OpenFoam), but I'm still having problems and don't see why... I went back to the original dambreak model, and just replaced the given geometry by another (simpler!) one. I'll post the code here:
Quote:
Cheers Benji |
||
April 7, 2014, 05:10 |
|
#3 |
Senior Member
|
Hi,
your post looks like "I've taken tutorial case, have done something to it, and now I'm not able to run it." There can be anything (though as error appears in interface properties call, I guess, you've just modified geometry but not setFieldsDict). Can you post your case files? This is the shortest path to solution of your problem. Otherwise it will be more-or-less: maybe the problem is there - no it is not - then maybe it is there - and so on. |
|
April 7, 2014, 05:32 |
|
#4 |
New Member
Benjamin
Join Date: Apr 2014
Location: Zürich
Posts: 27
Rep Power: 12 |
Thanks for the reply alexeym. And you're right, it is pretty much what you said, I'm not able to run it I just don't get why, I've done other cases with altered volumes/geometries etc. and didn't have problems...
I will add the files in the attachment, and yes, I have change the SetFieldsDict, too (although I'm not sure if correctly ) |
|
April 7, 2014, 05:54 |
|
#5 |
Senior Member
|
Well,
In the error, you've posted, there were two keywords: Code:
#4 pow in "/lib64/libm.so.6" #5 Foam::pow(Foam::dimensioned<double> const&, Foam::dimensioned<double> const&) at ??:? #6 Foam::interfaceProperties::interfaceProperties(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::IOdictionary const&) at ??:? Here is the relevant part of the constructor: Code:
Foam::interfaceProperties::interfaceProperties ( const volScalarField& alpha1, const volVectorField& U, const IOdictionary& dict ) : ... deltaN_ ( "deltaN", 1e-8/pow(average(alpha1.mesh().V()), 1.0/3.0) ), ... So I've rerun blockMesh and got the following output (relevant part is below): Code:
Creating block mesh topology --> FOAM Warning : From function cellModel::mag(const labelList&, const pointField&) in file meshes/meshShapes/cellModel/cellModel.C at line 128 zero or negative pyramid volume: -1666.67 for face 0 --> FOAM Warning : From function cellModel::mag(const labelList&, const pointField&) in file meshes/meshShapes/cellModel/cellModel.C at line 128 zero or negative pyramid volume: -2500 for face 1 --> FOAM Warning : From function cellModel::mag(const labelList&, const pointField&) in file meshes/meshShapes/cellModel/cellModel.C at line 128 zero or negative pyramid volume: -2083.33 for face 2 --> FOAM Warning : From function cellModel::mag(const labelList&, const pointField&) in file meshes/meshShapes/cellModel/cellModel.C at line 128 zero or negative pyramid volume: -2083.33 for face 3 --> FOAM Warning : From function cellModel::mag(const labelList&, const pointField&) in file meshes/meshShapes/cellModel/cellModel.C at line 128 zero or negative pyramid volume: -2083.33 for face 4 --> FOAM Warning : From function cellModel::mag(const labelList&, const pointField&) in file meshes/meshShapes/cellModel/cellModel.C at line 128 zero or negative pyramid volume: -2083.33 for face 5 --> FOAM Warning : From function blockMesh::createTopology(IOdictionary&) in file blockMesh/blockMeshTopology.C at line 255 negative volume block : 0, probably defined inside-out Code:
Checking geometry... Overall domain bounding box (0 -5 0) (100 10 10) Mesh (non-empty, non-wedge) directions (1 1 1) Mesh (non-empty) directions (1 1 1) Boundary openness (9.57111e-17 0 3.81162e-16) OK. ***High aspect ratio cells found, Max aspect ratio: 2.19333e+200, number of cells 5000 <<Writing 5000 cells with high aspect ratio to set highAspectRatioCells Minimum face area = 1. Maximum face area = 2.99. Face area magnitudes OK. ***Zero or negative cell volume detected. Minimum negative volume: -2.99, Number of negative volume cells: 5000 <<Writing 5000 zero volume cells to set zeroVolumeCells Mesh non-orthogonality Max: 180 average: 178.658 ***Number of non-orthogonality errors: 13900. <<Writing 13900 non-orthogonal faces to set nonOrthoFaces ***Error in face pyramids: 30000 faces are incorrectly oriented. <<Writing 16100 faces with incorrect orientation to set wrongOrientedFaces Max skewness = 0.0951575 OK. Coupled point location match (average 0) OK. Failed 4 mesh checks. |
|
April 7, 2014, 06:07 |
|
#6 |
New Member
Benjamin
Join Date: Apr 2014
Location: Zürich
Posts: 27
Rep Power: 12 |
Thanks for looking at it and sorry for being an idiot xD took 1 minute to fix it, got the the net as it was and just trusted it to be right (cuz it looked right in paraView)... I'll now allways check it before, sorry again...
|
|
Thread Tools | Search this Thread |
Display Modes | |
|
|