CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... (http://www.cfd-online.com/Forums/openfoam-meshing-other/)
-   -   Highly skew faces in STAR-CCM+ meshes in OpenFOAM for boats (http://www.cfd-online.com/Forums/openfoam-meshing-other/101526-highly-skew-faces-star-ccm-meshes-openfoam-boats.html)

maxof May 6, 2012 21:54

Highly skew faces in STAR-CCM+ meshes in OpenFOAM for boats
 
Hi,

I am predictiong the calm water resistance of fast catamarans in OpenFOAM 2.1.0 with unstructured hex-meshes generated using STAR-CCM+ 6.04. Most of the times it is working very well, but sometimes there are some highly skew faces on (or very close to) the hull which may impair the results. For a skewness above 4.0 the simulation fails due to severe pressure discontinuities at those cells respectively. The highly skew faces usually occur in the bow region, where the sharp stem is of an angle of around 45 deg to the vertical axis.

Even though I am using prism layers on the hull and the convex angle has been reduced to 270 deg, the skew cells still occur where the prism layers do not wrap around the sharp edges. Furthermore, I am not applying a symmetry condition at the bow and refinements of those areas have not improved this behaviour.

Checking the mesh in STAR-CCM and checkMesh leads to different values of skewness, probably due to different definitions. My final question is if there a way to tell STAR-CCM to produce less skewed cells around sharp edges which are appropriate for OpenFOAM?

Any suggestions appreciated.
Thanks, Max

maxof May 13, 2012 22:20

Well, looks like this question is a bit special :-\
Anyway, is there anyone meshing with STAR-CCM+ and simulate using OF? Has anybody encountered any special issues of STAR-CCM+ meshes within OpenFOAM, especially on free surface flows?
Cheers, Max

hannes May 14, 2012 14:20

Hello,

I have tried once to mesh a hull in Star-CCM+ with the trimmed mesher and to use it in OpenFOAM. This failed because of a number of zero area faces.
Btw., StarCCM+ also failed to produce a stable solution on this mesh.
I have then created a mesh using snappyHexMesh. This worked fine with both solvers.
I also encountered problems with the prism layer cells in the polyhedral meshes from StarCCM+.

Regards, Hannes

Ros May 18, 2012 05:15

Hello,

I think a have a similar problem. In my case I have an internal flow through a pipe.
The interesting thing is that with a very simple geometry (pipe, elbow) OF accepts the mesh generated by StarCCM+, but with a more complex geometry I get this error:

Quote:


Create polyMesh for time = 0

Time = 0

Mesh stats
points: 231261
faces: 313837
internal faces: 300467
cells: 56589
boundary patches: 5
point zones: 0
face zones: 0
cell zones: 0

Overall number of cells of each type:
hexahedra: 2254
prisms: 85
wedges: 9
pyramids: 2
tet wedges: 11
tetrahedra: 5
polyhedra: 54223

Checking topology...
Boundary definition OK.
Cell to face addressing OK.
Point usage OK.
<<Found 24 neighbouring cells with multiple inbetween faces.
Upper triangular ordering OK.
<<Writing 52 unordered faces to set upperTriangularFace
Face vertices OK.
Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces ...
Patch Faces Points Surface topology
DOC_Wall 2352 4704 ok (non-closed singly connected)
Chan1_Wall 5944 9712 ok (non-closed singly connected)
inlet 371 636 ok (non-closed singly connected)
outlet 199 322 ok (non-closed singly connected)
Chan_2_Wall 4504 7392 ok (non-closed singly connected)

Checking geometry...
Overall domain bounding box (-0.0210004 -0.104821 -0.226609) (0.234912 0.0472684 0.0462122)
Mesh (non-empty, non-wedge) directions (1 1 1)
Mesh (non-empty) directions (1 1 1)
Boundary openness (-1.44097e-16 1.1794e-17 -4.36464e-17) OK.
Max cell openness = 4.1143e-16 OK.
Max aspect ratio = 26.1043 OK.
Minumum face area = 7.0189e-10. Maximum face area = 5.16457e-05. Face area magnitudes OK.
Min volume = 6.733e-12. Max volume = 5.28069e-07. Total volume = 0.0029788. Cell volumes OK.
Mesh non-orthogonality Max: 106.221 average: 20.8468
*Number of severely non-orthogonal faces: 1748.
***Number of non-orthogonality errors: 6.
<<Writing 1754 non-orthogonal faces to set nonOrthoFaces
***Error in face pyramids: 57 faces are incorrectly oriented.
<<Writing 55 faces with incorrect orientation to set wrongOrientedFaces
***Max skewness = 6.00451, 16 highly skew faces detected which may impair the quality of the results
<<Writing 16 skew faces to set skewFaces
Coupled point location match (average 0) OK.

Failed 3 mesh checks.

End



Does anyone has any suggestions how to repair the mesh?
Thanks,Ros

wyldckat May 18, 2012 11:04

Greetings Ros and welcome to the forum!

I've seen these errors occur in the past with converting Star-CCM+ meshes to OpenFOAM, as well as snappyHexMesh generating some damaged meshes... and came to a few conclusions:
  • The converter might be already too outdated, or at least doesn't take into account certain cell/face shapes that Star-CCM+ can use.
  • Also ended up having to generate meshes with snappyHexMesh and then convert to Fluent mesh to import in Star-CCM+.
  • Some errors might be fixable with OpenFOAM's utility modifyMesh. The problem is that even after looking at the code to understand how it can be used, there aren't any real examples of how to use it. Additionally, not all situations are contemplated by modifyMesh, at least not directly.
In the end, if the mesh is bad after its generated/converted, the usual solution is just do another mesh, with adjusted parameters, including placing the geometry placed closer to the origin of the simulation space in snappyHexMesh.

Best regards,
Bruno

Ros May 18, 2012 11:55

Hello Bruno,

Thank you very much for your quick and detailed answer!
  • I am going to try to modify some of the parameters in Star-CCM+ because I think that the problem has also something to do with the fact that I am generating an unstructured mesh.
  • modifyMesh seems to be very interesting and I'll give it a try
Regards. Ros

prasanth July 10, 2012 06:35

Hello Ros,

Did you tried with modifyMesh utility? It requires modifyMeshDict file right? In that dictionary, there are several options like point move, split edges etc. Which one is preferrable. In Icem and all other commercial pre processors, split edge is preferrable. Is it like in OpenFOAM also the same thing. Paraview is the only option to identify those skew faces? or Is there any other option. Please reply, If you have done with this utility.

Regards
Prasanth.

Ros July 10, 2012 07:12

Hello prasanth,

I am sorry, but I stillt haven't tried it. I switched to snappyHexMesh and it produces actually very satisfying results even with complex geometries.
But if you are going to try it, please post here your results. It would be very interesting to see if there is a stable solution to this problem.

Regards, Ros

prasanth July 13, 2012 04:20

Hello Ros,

I am trying with simplecase. If it works, I will post the results.

Regards
Prasanth.

Sniper August 19, 2013 08:51

hi Ros, Prasanth,

Any luck with your meshes, I am facing similar issues after converting mesh from StarCCm to OpenFOAM. Your inputs will be helpful

Thanks,

Vimal.

KateEisenhower June 8, 2015 05:53

Quote:

Originally Posted by wyldckat (Post 361871)
Greetings Ros and welcome to the forum!

I've seen these errors occur in the past with converting Star-CCM+ meshes to OpenFOAM, as well as snappyHexMesh generating some damaged meshes... and came to a few conclusions:
  • The converter might be already too outdated, or at least doesn't take into account certain cell/face shapes that Star-CCM+ can use.
  • Also ended up having to generate meshes with snappyHexMesh and then convert to Fluent mesh to import in Star-CCM+.
  • Some errors might be fixable with OpenFOAM's utility modifyMesh. The problem is that even after looking at the code to understand how it can be used, there aren't any real examples of how to use it. Additionally, not all situations are contemplated by modifyMesh, at least not directly.
In the end, if the mesh is bad after its generated/converted, the usual solution is just do another mesh, with adjusted parameters, including placing the geometry placed closer to the origin of the simulation space in snappyHexMesh.

Best regards,
Bruno

Hi Bruno,

what do you mean with placing the geometry closer to the origin of the simulation space? And why does it change the outcome?

Best regards,

Kate

wyldckat June 10, 2015 15:40

Quote:

Originally Posted by KateEisenhower (Post 549300)
what do you mean with placing the geometry closer to the origin of the simulation space? And why does it change the outcome?

Quick answer: For example, having a geometry placed at 4000km from the origin of the world will not have the same numerical precision during meshing as placing the geometry near the origin.
If you play around with a 32 or 64-bit calculator, you'll see what I mean; e.g. try adding 4000000000 with various values of 0.00000153452353 or something like that :).


All times are GMT -4. The time now is 05:29.