CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] ICEM-uncovered faces problem (http://www.cfd-online.com/Forums/ansys-meshing/71726-icem-uncovered-faces-problem.html)

saba_san January 13, 2010 05:44

ICEM-uncovered faces problem
 
4 Attachment(s)
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.

http://picasaweb.google.ch/lh/photo/...eat=directlinkwhen 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

PSYMN January 14, 2010 10:03

Uncovered faces...
 
1 Attachment(s)
When you do a refine, you get hanging nodes… This would be a problem for some solvers, but is not a problem for fluent. This is why the check is listed as a “possible problem”.

There are really two ways to “fix” these hanging nodes.

1)The default check fix doesn’t realize that they are this sort of refined hexa. It just sees hanging nodes and tells you about them. When you say fix, it prompts you to select a new part to put the new shells in. It uses these shells to cover all the hanging nodes and effectively walls off the problem. In some cases, this would be ideal. In your case it is not.

2)If you want 1 to 1 connection between the refined section and the rest of the mesh, you could use “resolve refinements” under edit mesh. This will connect everything up. The attached image should be an animated gif to illustrate... Just testing if it works. If not, you can find it on our ANSYS.com website under the ICEM CFD Product page.

But in your case, you are using Fluent and can simply look at the uncovered faces to make sure they are between hexa fluid regions and you will be fine. No need to fix. (On the other hand, if your inlet boundary was uncovered, you would want to fix and you would put the new shells in the part of INLET so you could apply a BOCO).

rackem February 11, 2010 12:04

PSYMN:
Where is this "resolve refinements" option under edit mesh in ICEM. I cannot find it and the uncovered faces issue is the only error I get in my 2d mesh when I try to export it to Fluent. For reference I am making a simple channel with a velocity inlet and a pressure outlet in between two walls. When I try to open this mesh in fluent I receive the error...
Error:
FLUENT received fatal signal (ACCESS_VIOLATION)
1. Note exact events leading to error.
2. Save case/data under new name.
3. Exit program and restart to continue.
4. Report error to your distributor.

Any help will be of use as I am new to ICEM/Fluent

thank you

PSYMN February 11, 2010 12:28

Make sure this is what you need...
 
Resolve refinments is under Edit Mesh => Merge Nodes => Merge Meshes => Resolve Refinements.

Just use the standard option.

This works with 3 to 1 hanging nodes.

With 2 to 1 hanging nodes, Fluent shouldn't care. Which is what I said last time... if you have 2 to 1 hanging nodes due to a hexa refinement, don't try to fix it. That is just a "possible problem". Fixing it actually makes it worse for Fluent because the fix is to cover them with elements.

saba_san March 15, 2010 05:19

"Uncovered faces" error again!
 
1 Attachment(s)
Hello and thanks for your response.
What you suggested about resolving the refinement does not work for me. I get an error of "uncoupling failed". My refinement is 2 to 1, although Fluent still have problem with it.
So I changed my case. I don't use any refinement. The geometry is made in Ansys workbench, and then meshed in ICEM using the "2D planar" blocking option. When I check the mesh, I get this error of "uncovered faces" again at all the cells at the perimeter, and when trying to import it to Fluent, I get an error. I dont understand why I get this error this time. I used no refinement. I appreciate if anyone can help me with this.
Attached is a shot of the mesh and where I get the error of the "uncovered faces"
Best,
Saba

saba_san March 15, 2010 09:21

I should add that I'm trying to make a 2D mesh. It seems that my problem is due to the fact that ICEM thinks its a 3D geometry, although in the workbench, I specified that it is 2D. Is there anyway I can create a simple 2D mesh in ICEM? or is it just to create 3D meshes?

PSYMN March 15, 2010 10:00

Unconvered edges...
 
Nope, ICEM CFD is perfectly good for 2D meshing...

In 3D, an uncovered face would mean that you don't have shells on the outside of your volume elements. The solver needs those shells to assign the bocos, so without them, you have a problem...

In 2D, you really have "uncovered edges" around your shells (notice it is highlighting only the perimeter). The result is the same, the solver has no where to put the boundary conditions and that is a problem.

The fix is simple enough... When using ICEM CFD Hexa for 2D blocking ALWAYS associate the perimeter edges to the curves... When you do that, you will get the perimeter line elements that your solver needs.

SO just go back and make those associations now, then regenerate the unstructured mesh and you should be fine.

saba_san March 15, 2010 10:38

Thanks a lot for the clear explanation Simon. I tried it and it worked!

Saba

mars April 22, 2012 08:33

I'm a novice in ICEM, and could you kindly explain "shell" and "bocos" in your reply?
Thanks a lot!
Quote:

Originally Posted by PSYMN (Post 250056)
Nope, ICEM CFD is perfectly good for 2D meshing...

In 3D, an uncovered face would mean that you don't have shells on the outside of your volume elements. The solver needs those shells to assign the bocos, so without them, you have a problem...

In 2D, you really have "uncovered edges" around your shells (notice it is highlighting only the perimeter). The result is the same, the solver has no where to put the boundary conditions and that is a problem.

The fix is simple enough... When using ICEM CFD Hexa for 2D blocking ALWAYS associate the perimeter edges to the curves... When you do that, you will get the perimeter line elements that your solver needs.

SO just go back and make those associations now, then regenerate the unstructured mesh and you should be fine.


Adrian281 July 11, 2012 11:19

I similarly have problems with uncovered elements. I am generating a hybrid hex-tet grid around a slightly complicated 3D aircraft geometry. I'd like to be able to understand why this is happening. Is it something to do possibly with my edge criterion?

cesarcg December 3, 2012 14:41

18 uncovered faces when writing mesh for fluent!
 
hi all,

as i explained in a previous post, i'm meshing a 3d mesh using the blocking strategy. Far gave me some advices for improving the topology but now i'm having problems when writing the mesh for fluent.

ICEM prints a message that reads: "Warning: mesh has 18 uncovered faces" but when i run the 'check mesh' command it prints that everything is ok but 2 penetrating elements. i checked the surfaces, edges and vertices associations as suggested by Simon in previous posts and found that everything is ok.

please, any advice would be helpful. i uploaded the files to drop box in case you need to take a look at the problem. i hope this can be solved easily.

https://www.dropbox.com/sh/2bjnfo3mnn33w0p/-FgaEU82V6

kind regards,

Far January 7, 2013 02:52

Good work. Did you export the mesh to Fluent (It is too late to ask this question)! Any how how are the results ?

Again congratulation:) on meshing this complex model with Hexa

cesarcg January 7, 2013 12:29

Re
 
Quote:

Originally Posted by Far (Post 400415)
Good work. Did you export the mesh to Fluent (It is too late to ask this question)! Any how how are the results ?

Again congratulation:) on meshing this complex model with Hexa

Hi Far,

I exported the mesh after solving most of the issues I was having trouble with. It also came to mind how to improve a little bit more the topology in order to get a faster convergence. I'm trying this but now with the model including the fuselage.

I hope to get good results and I'll let you know when I succeed. If I get stuck again, I'll let you know asking for help.

Thanks for all your help and attention.

Regards.

Far January 7, 2013 12:34

I see the problem in the one of winglets, where quality is negative.

Lisandro Maders March 20, 2013 17:08

Uncovered faces - 3D How to Solve?
 
Quote:

Originally Posted by PSYMN (Post 250056)
Nope, ICEM CFD is perfectly good for 2D meshing...

In 3D, an uncovered face would mean that you don't have shells on the outside of your volume elements. The solver needs those shells to assign the bocos, so without them, you have a problem...

In 2D, you really have "uncovered edges" around your shells (notice it is highlighting only the perimeter). The result is the same, the solver has no where to put the boundary conditions and that is a problem.

The fix is simple enough... When using ICEM CFD Hexa for 2D blocking ALWAYS associate the perimeter edges to the curves... When you do that, you will get the perimeter line elements that your solver needs.

SO just go back and make those associations now, then regenerate the unstructured mesh and you should be fine.

I have the same problem, uncovered faces in a 3D strucutre... I understood what is an uncovered face, but how can I solve this problem??

Thank you

ok___ko April 28, 2013 07:53

after refinement, it shows uncovered faces
 
Quote:

Originally Posted by PSYMN (Post 242597)
When you do a refine, you get hanging nodes… This would be a problem for some solvers, but is not a problem for fluent. This is why the check is listed as a “possible problem”.

There are really two ways to “fix” these hanging nodes.

1)The default check fix doesn’t realize that they are this sort of refined hexa. It just sees hanging nodes and tells you about them. When you say fix, it prompts you to select a new part to put the new shells in. It uses these shells to cover all the hanging nodes and effectively walls off the problem. In some cases, this would be ideal. In your case it is not.

2)If you want 1 to 1 connection between the refined section and the rest of the mesh, you could use “resolve refinements” under edit mesh. This will connect everything up. The attached image should be an animated gif to illustrate... Just testing if it works. If not, you can find it on our ANSYS.com website under the ICEM CFD Product page.

But in your case, you are using Fluent and can simply look at the uncovered faces to make sure they are between hexa fluid regions and you will be fine. No need to fix. (On the other hand, if your inlet boundary was uncovered, you would want to fix and you would put the new shells in the part of INLET so you could apply a BOCO).

Hi.

I have the same problem with saba, which also shows 'WARNING: Mesh has uncovered edges. Fluent needs a complete boundary (lines in 2D) or it will give a variety of errors and not read in the mesh! If this was 2D Hexa, perhaps your edges are not associated with perimeter curves' after the refinement.
And I have already tried the way that you said to 'resolve refinement', but it said 'This mesh has no couplings.' So, it still cannot work. Could you help me except re-do a new mesh.

I am looking forward to your reply. Thanks

Daniel_Khazaei October 17, 2013 08:13

Quote:

Originally Posted by PSYMN (Post 250056)
Nope, ICEM CFD is perfectly good for 2D meshing...

In 3D, an uncovered face would mean that you don't have shells on the outside of your volume elements. The solver needs those shells to assign the bocos, so without them, you have a problem...

In 2D, you really have "uncovered edges" around your shells (notice it is highlighting only the perimeter). The result is the same, the solver has no where to put the boundary conditions and that is a problem.

The fix is simple enough... When using ICEM CFD Hexa for 2D blocking ALWAYS associate the perimeter edges to the curves... When you do that, you will get the perimeter line elements that your solver needs.

SO just go back and make those associations now, then regenerate the unstructured mesh and you should be fine.


thanks for the great explanation, that just solved my problem.:)

kozalp January 9, 2014 11:03

uncovered face error (overlapped shell elements)
 
5 Attachment(s)
Hey guys,

I have a very similar case like this one: http://www.cfd-online.com/Forums/ans...ary-layer.html

My images are below:

Attachment 27841 Attachment 27842 Attachment 27843 Attachment 27844

I did my BL by 2d planar blocking and then I meshed my outer geometry.

After I checked mesh, I got the error of uncovered faces. So I did what psymn said and created a subset of uncovered faces. Then I added layers to the subset of uncovered faces and visualized the entire uncovered faces and believe me they were many. So I deleted all the shell elements under the subset. That solved my problem, but I wonder why it happened, what did I do wrong?

Uncovered faces were starting from the boundaries of the refinement curves and reach to the wall of my base geometry. This pic will make you realize better:

Attachment 27845

The red curve in the middle is my geo and the inner c-grid is my refinement zone.

Hope you can find an answer guys.

zdunol October 12, 2014 10:01

solution
 
Hi, i have found this to help with uncovered faces:
in icem go to edit mesh-->check mesh--> check and fix uncovered faces

it helped me - fluent managed to read the mesh.
I have to say that before doing this i have associated all the edges to the curves manually and it didnt help.

I wouldn't be surprised if fixing stuff this way may be dangerous, like for example when you use "speed up your computer" programs which delete your register files and in general, to some extent, work in brute force manner, but that's just my guts maybe some specialists in here? :P

p3vdim May 18, 2015 12:28

Hi,
I am new to ANSYS... and I want to use design modeler to draw 2D street canyon... like how you have design in your study. Can you please send me the steps how you have created this geometry in design modeler of ANSYS please?


All times are GMT -4. The time now is 03:34.