[jsing232]

Originally Posted by saba_san

Hello,
I have created a mesh for a street canyon using ICEM as below. I have refined the mesh in the canyon and the small area on top of it using the refinement option in ICEM.

when I run check the mesh, it tells me that I have "uncovered faces" at the boarder of this area where I have refined the mesh. I say "fix" and apparently it fixed the problem.

When I save the mesh and open it in fluent and run a simulation, it does not recognize this area (refined) as my domain.. the entire domain is supposed to be air. If I look at the velocity vectors after running the simulations, it shows there is no flow in this refined mesh area which is a mistake. So this boundary that is created for fixing the "uncovered faces" apparently causes this problem.

So what I need to understand is:
1. why is this uncovered faces occur in ICEM?
2. How can I solve the problem I have now in fluent?


I appreciate your help,
Best,
Saba

Dear
When u are trying to save mesh file for fluent just check 3d and check-----ignore coupling.....then u can read mesh in fluent

[arohr]

Hello,

I'm hoping to bring this thread back to life because I'm having some serious difficulty with the uncovered faces error.
I am attempting a hybrid grid to look at flow around a cylinder which I am using as a test case before I move up to a sphere.
I have a blocking structure for the near-surface geometry, with an O-grid for the cylinder and a normal block for the wake region.
Then I have an interface surface which separates this volume from unstructured cells which I mesh normally propagating further towards the far field. (see picture)
I want to use the blocking refinement to save cell count in the structured cell zone by refining in the span-wise direction. Since I am using an O-grid, if I don't have different levels of refinement, the cell size from my surface will propagate all the way to my interface surface, and cause for a very large cell count (because I need very small cells near the surface to capture Boundary Layer).

I have attempted to use resolve refinements, but ICEM spits out the "This mesh has no couplings" error.
When I do the built-in mesh error fix for uncovered faces, all it does is assign the faces to a part. Exporting this mesh to fluent causes the flow to see these faces as a One-sided surface, which I DON'T intend them to be since they are internal to the flow.
The other attempt I made was to just leave them as is, but I get an error when I attempt to read the mesh into fluent of "cell is missing face..." which means that the uncovered faces are being noticed by fluent.
I even attempted the latest idea of checking the "ignore coupling" option on mesh output to fluent, but because icem doesn't detect coupling in the mesh, there is no coupling to ignore. I tried anyways, fluent error'ed out.

Basically, I am attempting to simply refine different sections of my blocking mesh. Then output them as part of my overall mesh. I couldn't believe it was this difficult to get it working, but I have run out of ideas. Any and all help is welcome!

P.S. If anything doesn't make sense I can include more pictures!

Thanks,

Allen

[Far]

this problem comes after hybrid mesh or in just hexa mesh?

[arohr]

Originally Posted by Far

this problem comes after hybrid mesh or in just hexa mesh?

Not sure what you mean by your question, but I'll try and explain my process more clearly.
First, I created all of my geometry. Then, I used blocking for the inner section (if you look at the picture of my overall mesh, you can see the smaller sort of rectangle section). When I completed my blocking, I used the mesh refinement for the blocks closest to my body surface. Then, I hid the inner blocking area, and did a tetra mesh for the outer area (where you see the unstructured cells).
Next, I used "load from blocking" for the blocking structured mesh and merged with the tetra unstructured mesh. After that, I merged the interface surface nodes at my "dummy" interface surface. Then I performed my check mesh and that's where it displays my uncovered faces error.
So the problem with uncovered faces comes when I converted my blocking to unstructured mesh.

Please let me know if there's anything else I can clear up! Hope we can solve my problem!

-Allen

[Far]

Does ICEM CFD show uncovered faces at interface of tetra and hexa mesh?? I guess yes...

or it may be due to mesh refinement with any ratio other than 2:1.


Ok. Here is step by step procedure.

1. First create the hexa blocking. Convert to unstructured mesh and save this mesh as, lets say, hexa.uns (from file>mesh>save mesh as). name the interface walls as wall1_hexa, wall2_hexa etc.

Note : a. You must limit your refinement to 2:1 in one layer, and do it successively to reduce mesh count. Fluent will not accept 3:1 or other refinement levels.

b. You can get rid of this problem by using option resolve refinements in ICEM CFD (Edit mesh tab)



2. Create Tetra mesh in the outer part as you have already described. and save it also (just to make things safe ) . name the same interface as now, wall1_tetra, wall2_tetra etc. note that wall1_hexa and wall1_tetra are the boundaries at the same goemetric location and are exact copy to each other.

3. Open hexa mesh , file > mesh > open mesh. when prompted, select merge option. But wait, mesh is still not merged

4. Now go to edit mesh tab, merge nodes > merge meshes and select the common surfaces (e.g. wall1_hexa, wall1_tetra etc).

5. After merging you will have both meshes merged and tetra mesh will adjust itself according to hexa mesh. But note that, there should almost same no of nodes on both sides. it may slightly be different, like you have 100 nodes on hexa side and 90 to 110 nodes on tetra side. that will be taken care by ICEM CFD.

6. You will notice that interface surfaces are now converted into one surface with quad elements.

7. Now you have option to declare it as interior boundary in ICEM CFD or just go to left panel and from part delete those surfaces.

Thats all...

[arohr]

Originally Posted by Far

Does ICEM CFD shows uncovered faces at interface of tetra and hexa mesh?? I guess yes...

or it may be due to mesh refinement with any ratio other than 2:1.


Ok. Here is step by step procedure.

1. First create the hexa blocking. Convert to unstructured mesh and save this mesh as, lets say, hexa.uns (from file>mesh>save mesh as). name the interface walls as wall1_hexa, wall2_hexa etc.

Note : 1. You must limit your refinement to 2:1 in one layer, and do it successively to reduce mesh count. Fluent will not accept 3:1 or other refinement levels.

2. You can get rid of this problem by using option resolve refinements in ICEM CFD (Edit mesh tab)



2. Create Tetra mesh in the outer part as you have already described. and save it also (just to make things safe ) . name the same interface as now, wall1_tetra, wall2_tetra etc. note that wall1_hexa and wall1_tetra are the boundaries at the same goemetric location and are exact copy to each other.

3. Open hexa mesh , file > mesh > open mesh. when prompted, select merge option. But wait, mesh is still not merged

4. Now go to edit mesh tab, merge nodes > merge meshes and select the common surfaces (e.g. wall1_hexa, wall1_tetra etc).

5. After merging you will have both meshes merged and tetra mesh will adjust itself according to hexa mesh. But note that, there should almost same no of nodes on both sides. it may slightly be different, like you have 100 nodes on hexa side and 90 to 110 nodes on tetra side. that will be taken care by ICEM CFD.

6. You will notice that interface surfaces are now converted into one surface with quad elements.

7. Now you have option to declare it as interior boundary in ICEM CFD or just go to left panel and from part delete those surfaces.

Thats all...

Hey Far,

So just to clear up, the issue of resolving the refinement is not occurring between my tetra and hexa mesh merging. That I thankfully figured out on my own!
The issue is occurring after I've converted the Hexa to an Unstructured mesh.

Referring to what you wrote in Step 2, I would like to use the resolve refinements option in "edit mesh", but icem doesn't see that there are couplings, so it doesn't allow the resolve refinements function to run at all. The output I receive when I attempt to run Resolve Refinements is "The mesh has no couplings".
The only error I receive regarding my problem is that there are uncovered faces between the hexa cells that I have going from a ratio of 2:1. (see the second picture in my original reply).

Let me know if you'd like me to include any more explanation or images. I can also include files if it would help!

Thanks,

Allen

[Far]

yes attach files...

What if you have only hexa mesh. The same issues occurs. Actually what i am trying to figure it out, is that either this problem is due to hybrid mesh or due to issue in resolve refinements (specific to hexa mesh only).

So first thing you can do is that convert hexa mesh, after mesh refinement, into unstructured mesh and see if there is any problem. If not then we can converge our attention towards interface region between hexa and tetra mesh. But you can not use the resolve refinements option at the hybrid mesh interface...

[arohr]

Far,

Here is a folder with the project file:
https://drive.google.com/drive/folde...DA?usp=sharing
It is at the point where I have already converted the blocking to unstructured cells and merged with the unstructured mesh. I also have already merged the surface nodes on my dummy interface surface named "int_surf". I used the check errors in the edit mesh menu and saved the uncovered faces to a separate part "uncovered_faces". Let me know if you have any questions about it.

Thanks again for your help!

[arohr]

Originally Posted by Far

yes attach files...

What if you have only hexa mesh. The same issues occurs. Actually what i am trying to figure it out, is that either this problem is due to hybrid mesh or due to issue in resolve refinements (specific to hexa mesh only).

So first thing you can do is that convert hexa mesh, after mesh refinement, into unstructured mesh and see if there is any problem. If not then we can converge our attention towards interface region between hexa and tetra mesh. But you can not use the resolve refinements option at the hybrid mesh interface...

I have included a link in my previous reply, but I wanted to respond to what you wrote here.

The problems I am having are not in my interface region between the hexa and tetra, it is simply in the hexa which I converted to an unstructured grid. Those cells are not being recognized to have hanging nodes so I can't make use of the resolve refinements feature where I have the 2:1 ratio between cells.

[arohr]

Hi Far,

Any luck with my issue?
I have tried using the "Resolve Refinements" tool in the Edit Mesh tab after just converting my structured mesh to unstructured and when I used "Allow unstable patterns" I got the error: illegal non-symmetric refinement.

Any thoughts on this?

Thanks,

Allen

[vish161095]

thanks man...it worked well

[sidharthm18]

Hi .
I am new to Icem. I have a doubt. I want to make some of my blocks free. as i make them free they are becoming o grid automatically. due to which i am getting uncovered faces instead of edge curve association..




Thanks