CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Pre-Processing (http://www.cfd-online.com/Forums/openfoam-pre-processing/)
-   -   no base point for face xxx (http://www.cfd-online.com/Forums/openfoam-pre-processing/89883-no-base-point-face-xxx.html)

eugene.katsevman June 24, 2011 12:57

no base point for face xxx
 
Hello!
I'm pretty new to OpenFOAM. Now I'm trying to use dsmc solver. Now I'm getting a bunch of dsmcInitialize warnings like that:

--> FOAM Warning :
From function Foam::List<Foam::FixedList<Foam::label, 4> >Foam::Cloud<ParticleType>::faceTetIndices(label fI, label cI) const
in file meshes/polyMesh/polyMeshTetDecomposition/polyMeshTetDecomposition.C at line 561
No base point for face 25085, 3(3298 2596 2567), produces a valid tet decomposition.


I've tried to google it, but have no success. Where should I look and what's wrong exactly?

Thanks in advance.

johnsmith332 February 27, 2012 01:54

I've been having the same problem trying to run dsmc with snappyHexMesh. Has anyone figured this out?

Sylvain February 27, 2012 11:09

Hi everybody

Same here with the uncoupledKinematicparcelFoam. I found out that it was very sensitive to the mesh quality at the surface.
I succeed in avoiding the problem with basic meshes. But if your mesh is a bit complex it crashes every time a particle enter a cell whose shape is not so nice. So I don't know what to do.
The problem is that it is crashing the whole calculation, ,not only the individual particle.

Sylvain

Sylvain February 27, 2012 12:47

I tried to comment the part of the code that makes the code crash in the src/lagrangian/basic.particleI.H

As a result, the calculation doesn't crash any longer, but the code seemed to be caught in infinite loop and the calculation is stuck to one time step.

Means that this piece of code as a purpose after all!!!

Anyone as a solution?

Sylvain

Sylvain February 28, 2012 03:35

Hello John,

I'm trying to figure out why some of my meshes are working well, and why some others not.

I have tried 3 meshes generated with harpoon:

-1 with BL => it crashes, checkMesh told me that there was few cell with skewness but not a big deal
-1 whithout BL but with zero-thickness surfaces => it crashes => checkMesh told me about non-manifold points
-1 wihtout BL and whithout zero-thicknesse => it works => chekmesh reports few celles with skewness

I never had any problem with meshes generated with snappy before. Now I thinking about the zero-thicknesses surfaces which might be a problem (the particles don't know if it hits the above or below of the face?)

Do your mesh contains such surfaces, baffles, or weird BLs

johnsmith332 February 28, 2012 16:59

The geometry I used was pretty simple: a 3 inch bolt with no thread, so just an extruded hexagon and a cylinder. I've tried changing the mergeTolerance in snappyHexMesh, but nothing happened. I have no idea which tolerance the error is referring to. The only thing I really wrote myself was the snappyHexMeshdict, but then your having the same problem without snappy..

Sylvain February 29, 2012 03:35

hello John,

Thank you for your message. What did checkMesh say when you ran it on your mesh?

I'm pretty convinced that it has something to do with the mesh.
Yesterday I tried to get rid of all the non manifold points on may baffles using mergeOrSplitBaffle utility. But it only delayed the problem to another face.

So I don't know why it is working fine sometimes and not I other cases.

i'm going on with my investigations.

Sylvain February 29, 2012 12:12

Ok, last update!
i ran a calculation on a mesh made by a colleague with snappy. the mesh is far more than ugly, but well, it's working without any problem. So I don't understand.

johnsmith332 March 2, 2012 14:40

When I run checkMesh is gives me a bunch of ok's with no errors or warnings. However, in the final mesh, checkMesh lists the number of cells of each type, and there are a bunch of each type except tetrahedral, of which there is only 1 which seems strange. Also, in the source code where the error is, it mentions variables like tetFacel_ and tetBasePtI which I assume refers to tetrahedral cells, so perhaps this 1 cell is causing problems.

Sylvain March 7, 2012 13:00

Hello John,

i got the problem again today. something weird: the face which makes the run crash belongs to perfect hexa cell located far away from the particles.

I'm puzzled. For all my experiments, the problem arises with meshes from harpoon. Would be my conclusion except from the fact you have problem with snappy also... still I'm not yet confident with meshes from harpoon to OF



Anyone else had this issue before?

ybapat June 12, 2012 00:22

Helllo,

I also got same error mentioned in first post.

OpenFOAM release notes for 2.0.0 mention that polymesh used must pass test
checkMesh -allGeometry by giving message "Face tets OK" to run the particle case.

You can try running this check on your mesh and check if it fails.

Regards,
-Yogesh


Sylvain June 12, 2012 01:57

Thanks Yogesh for your message!

I have checked this morning on my previous case mentioned above. The "Face tets OK" indeed failed on the mesh which was not working. The test is good on the mesh which works.

Conclusion: adding this -allGeometry option allows to anticipate if your Mesh going to crash on Lagrangian simulations.

Thank you very much again Yogesh!

luchen2408 June 14, 2015 23:21

hello, sylvain, your conclusion for lagrangian simulation is :
checkMesh -allGeometry before start the simulation, right?
but how can I solve the problem if the fact tets failed? is there any optimization? Thanks


All times are GMT -4. The time now is 19:36.