[bany]

Hello,everyone:
i am meshing a cylinder.In order to refine the regions near the center of the cylinder,i used the order called refinement.But when checking mesh,there was a warning:Mesh has uncovered faces. Fluent needs a complete boundary (shells in 3D) or it will give a variety of errors and not read in the mesh!All edges have been associated.
Anymore,before refinement,there is no warning!
How can i resolve this problem?
Thanks.

[bany]

Oh,i think i should add something.
To explain my problem further,when i refine the local area at the top right-hand of the cube,it occurred something wrong.
To more details ,please see the following picture.

[bluebase]

How can i resolve this problem?

What did the search in this forum yield? Where there any solutions proposed that didn't work for you?

so called "Hanging nodes" is what you experience.

[bany]

Originally Posted by bluebase

What did the search in this forum yield? Where there any solutions proposed that didn't work for you?

so called "Hanging nodes" is what you experience.

Thanks for your reply.

Of course,there are several questions like mine in this forum yield.
But there is no explain why uncovered faces happened when refining a local area and how to solve it.
Can you help me？Thanks a lot!

[bluebase]

You might read these threads briefly:

Mesh refinement causing problems
ICEM-uncovered faces problem

The source of uncovered faces after refinement, that there are faces which are not associated to any (boundary) geometry, or a similar entity. ICEM does not have a specific element type to deal with the interface layer.

Depending on your solver, this will require specific treatment, or none at all.
If you use Fluent, and if you limit the refinement to 1to2 only, fluent will read the mesh just fine, without any treatment. Just ignore the uncovered faces at the refinement's jump.
Other solvers might need additional boundary faces at the refinement's edge.

[bany]

The source of uncovered faces after refinement, that there are faces which are not associated to any (boundary) geometry, or a similar entity. ICEM does not have a specific element type to deal with the interface layer.

Depending on your solver, this will require specific treatment, or none at all.
If you use Fluent, and if you limit the refinement to 1to2 only, fluent will read the mesh just fine, without any treatment. Just ignore the uncovered faces at the refinement's jump.
Other solvers might need additional boundary faces at the refinement's edge.[/QUOTE]

First,thanks for your help.
From your answers,I know that the mesh that have uncovered faces causing by the refinement to 1to2 can be used in fluent,but it cannot be used in openFoam.
So when someone wants to refine his model which will be computed in openFoam in ICEM,he should avoid the hanging nodes.

Thank you once again.

[bluebase]

Originally Posted by bany

So when someone wants to refine his model which will be computed in openFoam in ICEM,he should avoid the hanging nodes.

Are you sure? Have you tried fluent3dmeshtofoam? I am pretty sure this tool can deal with hanging nodes. It will convert the hexas to polyhedral in the transition layer.

As far as i remember the normal fluentmeshtofoam couldn't deal with hanging nodes. However, i haven't used openfoam extensively for a few years, so i am not informed on the latest changes.

[bany]

Originally Posted by bluebase

Are you sure? Have you tried fluent3dmeshtofoam? I am pretty sure this tool can deal with hanging nodes. It will convert the hexas to polyhedral in the transition layer.

As far as i remember the normal fluentmeshtofoam couldn't deal with hanging nodes. However, i haven't used openfoam extensively for a few years, so i am not informed on the latest changes.

Oh,when i tried fluent3dmeshtofoam to convert the fluent.msh and checkMesh,there is no warning or error.But when i run my case,there are errors.Please see the picture.Can you tell me what is wrong?

Thank you very much!

[bluebase]

I just ran a minimal test case and did not encounter any errors.
Openfoam 4.1, inflowoutflow template, simplefoam, and a simple box done in icem which has been splitted in halve and one side refined.

ftf.tar.gz, icem.tar.gz

Have you tried to do the node merging to resolve refinements on your unstructured mesh? I think this is not necessary and will likely cause problems.

You might need to explain your case in more detail, better in the openfoam subforum for mesh conversions?

[bany]

You might need to explain your case in more detail, better in the openfoam subforum for mesh conversions?[/QUOTE]

Thanks a lot. Now,I explain my case in detail.
My computational domain is a cylinder, and in the center of it,there is a jet flow .So I want to refine the center of the cylinder,just see the attachments.

In icem,I used the nested O-block,when I did the refinement ->pre mesh->convert to unstruct mesh->check mesh（there are more uncovered faces )->output fluent.msh->fluent3DMeshToFoam->checkMesh(mesh OK)->reactingFoam,then errors which said cannot find faces came.

Best wishes!

[bany]

Thanks a lot. Now,I explain my case in detail.
[/QUOTE]
I think i should attach my geometric model.

[bluebase]

Hi bany,

i saw in the project file that you are using ICEM v14.0.

there has been some issue with refinements till version 14.5
See Mesh Refinement Problem

Though i have no idea, whether this intersects with the openfoam issue.

Anyway, update to a later version.

[bany]

Though i have no idea, whether this intersects with the openfoam issue.

Anyway, update to a later version.[/QUOTE]

I will have a try.
Anyway,thanks for your continuous and high quality help and support.

[bany]

I think i am late to pose my test about my questions.
I test the case uploaded by Sebastian Engel and it does work well. When i check my mesh again using ICEM of higher version, the problem about uncovered faces occurs again. And then, i find that the error which says 'cannot find faces using edges......' does not come from the calculating process. Because i find the 'FATAL ERRORS' is in meshTool.C. That is ,when i use the functionObjects which involves meshTool.C in controlDict, the errors come. And when closing the functionObjects in controlDict, i find the errors disappear and the calculation can continue. So i think the solvers in OpenFOAM can deal with the hanging nodes, just like FLUENT which can deal with the 1=>2 ratio refinement.
But until now, i cannot find the reason why the mesh with hanging nodes which created in ICEM and converted into OpenFOAM by fluent3dmeshtofoam cannot be identified by meshTool.C or how can i do to solve this problem.
Finally, thanks to Sebastian.
Any advice is appreciating.
Best wishes.

[bany]

I think this post "can not find faces using edges.."when using the ICEM mesh can finish this post.
Best wishes to all who helped me.