[eugene.katsevman]

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]

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

[Sylvain]

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]

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]

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]

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]

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]

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]

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]

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]

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]

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!

[xiaofishnus]

When I run simpleFoam, I notice that there are a lot of warnings like:
"no base point for face xxx - produces a valid tet decomposition".

What does this warning mean? Due to the mesh/decomposition problem?

I still can get the results if the warnings appear. However, will these affect the accuracy of the solution?

Thanks.

[Chrisi1984]

Hello,

this error can indicate that you have a so called "face tet eror".

You can check that by running the checkMesh command with the option "allGeometry".

command:
checkMesh -allGeometry

Kind regards
Chrisi

[luchen2408]

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

[Dosin]

Hey,

I want to simulate a cyclone separator and at the first step when I used snappyHexMesh to generate grids(meshes), I faced to many comments include this error:
"no base point for face xxx - produces a valid tet decomposition".

when I searched at the forums I could not find any idea how I can remove this problem.

any advice can be suitable for me.

[ThuliumC]

Hello

I have had a very similar issue when trying to use snappyHexMesh, where I got lot of warnings similar to the ones described and then a warning that further warnings would be suppressed.

By using checkMesh on the base mesh that I generated using blockMesh, I discovered that this base mesh was the issue ("Failed 5 mesh checks."). So I corrected the edges describing the boundary faces in constant/polyMesh/blockMeshDict and checkMesh reported a perfect mesh and snappyHexMesh ran perfectly.


Here is the code I used for running checkMesh. It checks the blockMesh generated mesh, completely, as recommended by Sylvain, and records the output on a text file checkMesh.log:

checkMesh -constant -allGeometry -allTopology | tee checkMesh.log

Here are the two last warnings by snappyHexMesh just before it was terminated:

--> FOAM Warning : 
    From function Foam::List<Foam::tetIndices> Foam::polyMeshTetDecomposition::faceTetIndices(const polyMesh&, label, label)
    in file meshes/polyMesh/polyMeshTetDecomposition/polyMeshTetDecomposition.C at line 570
    No base point for face 444410, 4(15 16 11025 11024), produces a valid tet decomposition.
--> FOAM Warning : Suppressing any further warnings.

Here is the part of the constant/polyMesh/blockMeshDict that describes the faces:

boundary
(
    allBoundary
    {
        type patch;
        faces
        (
            (3 7 6 2)
            (0 4 7 3)
            (2 6 5 1)
            (1 5 4 0)
            (0 3 2 1)
            (4 5 6 7)
        );
    }
);

Running OpenFOAM version 2.2.2

Túlio A. C.

[Chrisi1984]

Hi,

if you run the checkMesh utiity with the option -allGeometry (so checkMesh -allGeometry) you will see that you have some face tet errors. You need to improve your mesh to get rid of them and to ensure that particle tracking works fine.

Kind regards
Chrisi

[eemdee]

Hi,

This thread has been very helpful in identifying the error, however I have no idea how to fix it. Attached is my whole case directory. It should be a very simple rectangle. Block mesh runs fine, I can even see it in paraFoam and everything seems very simple. But when I use my all run utility (which I got from the dsmc tutorial wedge15Ma5) I get this "No base point for face blah blah, produces a valid tet decomposition." I ran the checkMesh -allGeometry tool and it told me that it failed 5 mesh checks. I don't see this error anywhere else, can anyone explain what I'm supposed to do here? This geometry seems to work for other solvers, just not dsmc?