[skuznet]

Hello!

Can any one tell me what does this message mean:

--> FOAM FATAL ERROR: 
cell 15802 of level 0 does not seem to have 8 points of equal or lower level
cellPoints:5(17411 17412 17432 17433 17640)
pointLevels:5{0}


From function hexRef8::setRefinement(const labelList&, polyTopoChange&)
in file polyTopoChange/polyTopoChange/hexRef8.C at line 3770.

I how do I fix this problem?

Thank you!

[seaspray]

It is a mesh topology error. I would suggest looking at the mesh refinement settings used or at the way the base mesh is first obtained. Surface-based refinement in particular is prone to introducing step changes in refinement levels close to the surface that can sometimes lead to further problems. Exceeding 2:1 refinement ratios is also asking for trouble and often leads to such errors with SHM.

SHM runs with the least issues when there is a nice consistent uniform body of hexahedral cells all around the surface(s). Look into distance-based refinement before snapping, trying to further refine hexes around features is not always such a good idea, etc.

It is usually not too hard to get good snapping around geometry with the latest version (OF2.3.0), the same can't be said about growing consistent layers from the surface in the next step unfortunately!!!

[GabGar]

Maybe you didn't erase the data from the last simulation, I mean, in 0 folder.

[mhsadafi]

That is a great point! It worked for me

[Ahyar]

Originally Posted by mhsadafi

That is a great point! It worked for me

which one do you say is a great point? i seem have a similar problem here

[CfdUser5855]

For anyone else who finds this issue, re running block mesh and then SHM got rid of the same error

[zyfsoton]

Originally Posted by CfdUser5855

For anyone else who finds this issue, re running block mesh and then SHM got rid of the same error

HI, I had the same problem, could you please provide more details how you resolve this?

Many thanks,
Tony

[Yann]

Hi Tony,

This issue usually happens when trying to re-run snappyHexMesh on an existing mesh. snappy uses the previous mesh as initial mesh and throw this error because some cells are not hexahedric and it does not know how to split these cells to refine it.

In order to solve this issue you have to delete the previous mesh and recreate the initial mesh so snappy can start over on a clean initial mesh.

Regards,
Yann

[zyfsoton]

Originally Posted by Yann

Hi Tony,

This issue usually happens when trying to re-run snappyHexMesh on an existing mesh. snappy uses the previous mesh as initial mesh and throw this error because some cells are not hexahedric and it does not know how to split these cells to refine it.

In order to solve this issue you have to delete the previous mesh and recreate the initial mesh so snappy can start over on a clean initial mesh.

Regards,
Yann

Dear Yann,

Many thanks for your reply.

I have done some mesh refinement before executing snappyHexMesh, but I am not too sure about what you suggested about delete the previous mesh and recreate the initial mesh. Could you please provide more details about what means for previous mesh and how to create new initial mesh?

Many thanks and best regards,
Tony

[Yann]

Better doing it the other way around: can you describe all the steps you are doing before getting to the point when snappy gives your this error?

Yann

[zyfsoton]

Originally Posted by Yann

Better doing it the other way around: can you describe all the steps you are doing before getting to the point when snappy gives your this error?

Yann

Sure, I am simulating the hull and the rudder. The basic step is to import hull and rudder stl files and then use blockMesh to generate the computation domain. Then refine the mesh around the hull. After mesh refinement, I use snappyhexmesh, then this error reported. I have tried to lower the nCellsBetweenLevels from 4 to 1, but it doesn't work.

Many thanks
Tony

[Yann]

What do you mean by refine the mesh around the hull? How do you do it?

Yann

[zyfsoton]

Originally Posted by Yann

What do you mean by refine the mesh around the hull? How do you do it?

Yann

Mesh refinement is the process of using refineMeshDict and topoSetDict, which you can find more details in OpenFOAM tutorial e.g. DTCHull.

[Yann]

OK then refineMesh should not be the issue. Do you clean your case between 2 meshing attempts?

Try running an Allclean script, or manually delete the processor* directories (if running in parallel) or the constant/polyMesh directory (if running in serial). And then start over the process (blockMesh, refineMesh and then snappyHexMesh)

Regards,
Yann

[zyfsoton]

Originally Posted by Yann

OK then refineMesh should not be the issue. Do you clean your case between 2 meshing attempts?

Try running an Allclean script, or manually delete the processor* directories (if running in parallel) or the constant/polyMesh directory (if running in serial). And then start over the process (blockMesh, refineMesh and then snappyHexMesh)

Regards,
Yann

Yes, every time if there is an error reported, I will delete all folders and then rerun all the processes, but there is still an error. Let me check again, I think the stl scale is not correct, which may be the source of error. I will figure it out and keep you updated.

Many thanks for your suggestion anyway!
Tony

[Yann]

Ok then let us know if proper scaling solves the issue.
If not, you can still post your case here so we can try running it and see if someone can spot where does the error come from.

Regards,
Yann

[MS321@]

Hai All
I am new to openFoam
My case if to study flow around DTMB 5415
I run into an error as "cell 226430 of level 0 uses more than 8 points of equal or lower level" when i execute snappyhexmesh.
I did blockmesh then surfaceFeatureExtract then toposet(1 to 5) and refinemeshdict for each toposet then when i execute snappyHexMesh i run into same error as listed above.
I am using v2206 version 2.0
If anyone know how to solve this error please give me some suggestions
Hope i receives a positive reply soon ,Thank you,
Regards

[zyfsoton]

Originally Posted by MS321@

Hai All
I am new to openFoam
My case if to study flow around DTMB 5415
I run into an error as "cell 226430 of level 0 uses more than 8 points of equal or lower level" when i execute snappyhexmesh.
I did blockmesh then surfaceFeatureExtract then toposet(1 to 5) and refinemeshdict for each toposet then when i execute snappyHexMesh i run into same error as listed above.
I am using v2206 version 2.0
If anyone know how to solve this error please give me some suggestions
Hope i receives a positive reply soon ,Thank you,
Regards

HI, not sure the exact error source but from my point of view, it is better to do checkMesh after each mesh step, e.g blockMesh and refinementmesh. These two steps may have mesh problem, then if you run SHM, it will report the error for sure. But it also maybe the setting of your SHM is not sensible. Only from the information you provide, it is hard to figure it out. Also, it is necessary to do OF tutorials like DTCHull, DTCHullMoving and DTCHullWave, which would give you more insights of how mesher works in OF. I am using openfoam.org instead of your version openfoam.com, I think there is some differecne also between them, so be careful of it.

Tony

[MS321@]

I am facing an issue -feature and surface refinement are getting stopped by saying "Stopping refining since too few cells selected".
Can someone please give me a suggestion to solve this problem.

[MS321@]

I am attaching my snappy log file below please have a look into it , it is giving a message as meshing was done ok, but the problem is feature and surface refinement is not happening it is getting stopped.