CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[ICEM] ICEM-uncovered faces problem

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree4Likes
  • 4 Post By PSYMN

Reply
 
LinkBack Thread Tools Display Modes
Old   January 13, 2010, 05:44
Default ICEM-uncovered faces problem
  #1
New Member
 
Saba Saneinejad
Join Date: Jan 2010
Posts: 4
Rep Power: 7
saba_san is on a distinguished road
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
Attached Images
File Type: jpg mesh.jpg (54.4 KB, 443 views)
File Type: jpg mesh2.jpg (81.6 KB, 393 views)
File Type: jpg mesh3.jpg (95.4 KB, 373 views)
File Type: jpg mesh4.jpg (63.8 KB, 350 views)
saba_san is offline   Reply With Quote

Old   January 14, 2010, 10:03
Default Uncovered faces...
  #2
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
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).
Attached Images
File Type: gif hanganim.gif (50.9 KB, 353 views)
PSYMN is offline   Reply With Quote

Old   February 11, 2010, 12:04
Default
  #3
New Member
 
Join Date: Feb 2010
Posts: 7
Rep Power: 7
rackem is on a distinguished road
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
rackem is offline   Reply With Quote

Old   February 11, 2010, 12:28
Default Make sure this is what you need...
  #4
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
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.
PSYMN is offline   Reply With Quote

Old   March 15, 2010, 05:19
Default "Uncovered faces" error again!
  #5
New Member
 
Saba Saneinejad
Join Date: Jan 2010
Posts: 4
Rep Power: 7
saba_san is on a distinguished road
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
Attached Images
File Type: jpg uncoverd faces.jpg (64.0 KB, 255 views)
saba_san is offline   Reply With Quote

Old   March 15, 2010, 09:21
Default
  #6
New Member
 
Saba Saneinejad
Join Date: Jan 2010
Posts: 4
Rep Power: 7
saba_san is on a distinguished road
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?
saba_san is offline   Reply With Quote

Old   March 15, 2010, 10:00
Default Unconvered edges...
  #7
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
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.
Far, DungPham, ahmadreza and 1 others like this.
PSYMN is offline   Reply With Quote

Old   March 15, 2010, 10:38
Default
  #8
New Member
 
Saba Saneinejad
Join Date: Jan 2010
Posts: 4
Rep Power: 7
saba_san is on a distinguished road
Thanks a lot for the clear explanation Simon. I tried it and it worked!

Saba
saba_san is offline   Reply With Quote

Old   April 22, 2012, 08:33
Default
  #9
New Member
 
Ma Shao-jun
Join Date: Sep 2011
Posts: 1
Rep Power: 0
mars is on a distinguished road
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 View Post
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.
mars is offline   Reply With Quote

Old   July 11, 2012, 11:19
Default
  #10
New Member
 
Adrian
Join Date: Mar 2012
Posts: 8
Rep Power: 5
Adrian281 is on a distinguished road
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?
Adrian281 is offline   Reply With Quote

Old   December 3, 2012, 14:41
Default 18 uncovered faces when writing mesh for fluent!
  #11
Member
 
Cesar
Join Date: Nov 2012
Location: Guanajuato, México
Posts: 78
Rep Power: 6
cesarcg is on a distinguished road
Send a message via Skype™ to cesarcg
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,

Last edited by cesarcg; December 3, 2012 at 19:02. Reason: providing the link of the geometry files uploaded
cesarcg is offline   Reply With Quote

Old   January 7, 2013, 02:52
Default
  #12
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
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
Far is offline   Reply With Quote

Old   January 7, 2013, 12:29
Default Re
  #13
Member
 
Cesar
Join Date: Nov 2012
Location: Guanajuato, México
Posts: 78
Rep Power: 6
cesarcg is on a distinguished road
Send a message via Skype™ to cesarcg
Quote:
Originally Posted by Far View Post
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.
cesarcg is offline   Reply With Quote

Old   January 7, 2013, 12:34
Default
  #14
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
I see the problem in the one of winglets, where quality is negative.
Far is offline   Reply With Quote

Old   March 20, 2013, 17:08
Default Uncovered faces - 3D How to Solve?
  #15
Member
 
Lisandro Maders
Join Date: Feb 2013
Posts: 31
Rep Power: 4
Lisandro Maders is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
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
Lisandro Maders is offline   Reply With Quote

Old   April 28, 2013, 07:53
Default after refinement, it shows uncovered faces
  #16
New Member
 
tita
Join Date: Apr 2013
Posts: 27
Rep Power: 4
ok___ko is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
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
ok___ko is offline   Reply With Quote

Old   October 17, 2013, 08:13
Default
  #17
Senior Member
 
Daniel
Join Date: Mar 2013
Posts: 177
Rep Power: 9
Daniel_Khazaei will become famous soon enough
Quote:
Originally Posted by PSYMN View Post
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.
Daniel_Khazaei is offline   Reply With Quote

Old   January 9, 2014, 11:03
Default uncovered face error (overlapped shell elements)
  #18
New Member
 
Join Date: Jun 2013
Posts: 16
Rep Power: 4
kozalp is on a distinguished road
Hey guys,

I have a very similar case like this one: Hybrid mesh for 2D boundary layer

My images are below:

entire geometry.jpg boundary.jpg leading edge.jpg trailing edge.jpg

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:

curves.jpg

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.

Last edited by kozalp; January 9, 2014 at 11:09. Reason: added pictures
kozalp is offline   Reply With Quote

Old   October 12, 2014, 10:01
Default solution
  #19
New Member
 
Paweł
Join Date: Dec 2013
Location: Warsaw, Poland
Posts: 29
Rep Power: 3
zdunol is on a distinguished road
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
zdunol is offline   Reply With Quote

Old   May 18, 2015, 12:28
Default
  #20
New Member
 
Purvi
Join Date: Oct 2014
Posts: 4
Rep Power: 2
p3vdim is on a distinguished road
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?
p3vdim is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
problem with surface creation in ICEM from multiple curves dialolema ANSYS Meshing & Geometry 2 October 27, 2014 14:14
[ICEM] Multiple fluide zone in ICEM Hexa Block problem ddqp ANSYS Meshing & Geometry 4 October 9, 2013 10:57
[Other] Mesh Importing Problem cuteapathy ANSYS Meshing & Geometry 1 June 7, 2012 13:39
cyclicGgi - uncovered faces in parallel seami OpenFOAM Running, Solving & CFD 1 July 5, 2011 09:36
[gambit] problem connecting faces on 2 volumes joe_star ANSYS Meshing & Geometry 1 December 16, 2009 03:38


All times are GMT -4. The time now is 12:44.