CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM

no base point for face xxx

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   June 24, 2011, 13:57
Default no base point for face xxx
  #1
New Member
 
Eugene Katsevman
Join Date: Jun 2011
Posts: 1
Rep Power: 0
eugene.katsevman is on a distinguished road
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.
eugene.katsevman is offline   Reply With Quote

Old   February 27, 2012, 01:54
Default
  #2
New Member
 
John Smith
Join Date: Feb 2012
Posts: 4
Rep Power: 4
johnsmith332 is on a distinguished road
I've been having the same problem trying to run dsmc with snappyHexMesh. Has anyone figured this out?
johnsmith332 is offline   Reply With Quote

Old   February 27, 2012, 11:09
Default
  #3
Member
 
Sylvain Aguinaga
Join Date: Feb 2010
Posts: 32
Rep Power: 6
Sylvain is on a distinguished road
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 is offline   Reply With Quote

Old   February 27, 2012, 12:47
Default
  #4
Member
 
Sylvain Aguinaga
Join Date: Feb 2010
Posts: 32
Rep Power: 6
Sylvain is on a distinguished road
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 is offline   Reply With Quote

Old   February 28, 2012, 03:35
Default
  #5
Member
 
Sylvain Aguinaga
Join Date: Feb 2010
Posts: 32
Rep Power: 6
Sylvain is on a distinguished road
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
Sylvain is offline   Reply With Quote

Old   February 28, 2012, 16:59
Default
  #6
New Member
 
John Smith
Join Date: Feb 2012
Posts: 4
Rep Power: 4
johnsmith332 is on a distinguished road
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..
johnsmith332 is offline   Reply With Quote

Old   February 29, 2012, 03:35
Default
  #7
Member
 
Sylvain Aguinaga
Join Date: Feb 2010
Posts: 32
Rep Power: 6
Sylvain is on a distinguished road
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 is offline   Reply With Quote

Old   February 29, 2012, 12:12
Default
  #8
Member
 
Sylvain Aguinaga
Join Date: Feb 2010
Posts: 32
Rep Power: 6
Sylvain is on a distinguished road
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.
Sylvain is offline   Reply With Quote

Old   March 2, 2012, 14:40
Default
  #9
New Member
 
John Smith
Join Date: Feb 2012
Posts: 4
Rep Power: 4
johnsmith332 is on a distinguished road
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.
johnsmith332 is offline   Reply With Quote

Old   March 7, 2012, 13:00
Default
  #10
Member
 
Sylvain Aguinaga
Join Date: Feb 2010
Posts: 32
Rep Power: 6
Sylvain is on a distinguished road
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?
Sylvain is offline   Reply With Quote

Old   June 12, 2012, 01:22
Default
  #11
Member
 
Yogesh Bapat
Join Date: Oct 2010
Posts: 33
Rep Power: 6
ybapat is on a distinguished road
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

ybapat is offline   Reply With Quote

Old   June 12, 2012, 02:57
Default
  #12
Member
 
Sylvain Aguinaga
Join Date: Feb 2010
Posts: 32
Rep Power: 6
Sylvain is on a distinguished road
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!
Sylvain is offline   Reply With Quote

Reply

Tags
base point, dsmc, dsmcinitialize, model

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
matching variable data with grid point data anfho OpenFOAM Programming & Development 0 May 6, 2011 16:28
CFX Post: Problems with moving point cloud for changing time steps spatialtime CFX 0 December 7, 2009 05:56
BlockMeshmergePatchPairs hjasak OpenFOAM Native Meshers: blockMesh 11 August 15, 2008 08:36
Gmsh and samplesurface touf Open Source Meshers: Gmsh, Netgen, CGNS, ... 2 December 10, 2007 03:27
CFX4.3 -build analysis form Chie Min CFX 5 July 13, 2001 00:19


All times are GMT -4. The time now is 20:19.