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

[ICEM] Shadow walls in Fluent. ICEM meshes vs Workbench

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 18, 2011, 11:50
Default Shadow walls in Fluent. ICEM meshes vs Workbench
  #1
New Member
 
Adam Arvay
Join Date: Feb 2011
Posts: 21
Rep Power: 6
aarvay is on a distinguished road
I'm trying to understand how shadow walls are assigned when a mesh is imported into fluent from ICEM. My goal is to be able to model a fuel cell meshed with ICEM. My previous attempts at modeling using the workbench created meshes where shadow walls were generated only at the solid-liquid interfaces. As I understood the process, this was appropriate.

Now that I am making meshes with ICEM, the meshes that are imported into fluent seem to create shadow walls between everything and the solution isn't even coming close to converging. I'm quick to blame these new shadow walls since they are one very obvious difference between my two setups. However, I don't really understand shadow walls so my blame may be misplaced.

Do these shadow walls allow for gas transport through them? or do they behave like solid walls?
aarvay is offline   Reply With Quote

Old   February 18, 2011, 16:38
Default
  #2
New Member
 
Adam Arvay
Join Date: Feb 2011
Posts: 21
Rep Power: 6
aarvay is on a distinguished road
This is probably related. none of the cell zones have interiors that display on the mesh. Meshes brought into fluent through the workbench displayed green volumes for the interior zones. The meshes I am importing through ICEM via unstructured meshes don't feature any interiors. I'm not sure if thats a feature of using an unstructured mesh. but without it showing up on the mesh display control panel, i have no idea if these bodies have their volumes meshed. ICEM seems to be creating the volume elements but they don't seem to be carrying over, as far as i can tell.
aarvay is offline   Reply With Quote

Old   February 19, 2011, 14:17
Default
  #3
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Sorry, not sure what you are doing wrong. ICEM CFD can produce a mesh that is perfect for Fluent, and should pretty much do that by default, but without knowing your process or anything about what you did in ICEM CFD, I can't guess where you went wrong.
PSYMN is offline   Reply With Quote

Old   February 22, 2011, 11:41
Default
  #4
New Member
 
Adam Arvay
Join Date: Feb 2011
Posts: 21
Rep Power: 6
aarvay is on a distinguished road
I think I may have found my issue. I'm not sure how to resolve it yet, but I haven't fiddled around very much yet. Its probably very easy.

All of my surfaces are showing up in the boundary conditions as mixed/unknown. What do I need to do in order to have these surface parts to be categorized as one sided or two sided surfaces instead of mixed/unknown? its not as simple as dragging them on the BC screen, that would have been nice.

Thanks.
aarvay is offline   Reply With Quote

Old   February 22, 2011, 11:47
Default
  #5
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Mixed/Unknown means that you have multiple element types in a part...

For instance, it is quite common to have shell, line and point elements all in a single part. That part isn't just a shell part, so it puts it into "mixed/unknown".

For 3D fluent, bocos can be mixed shell, line, point. But for 2D, that would be a huge problem.

For 3D, it would be a huge problem if your mixed part included shell and volume parts.

The fix is to make sure you don't have shells and volumes (in 3D) in the same part, or to make sure you don't have shells and lines (for 2D) in the same part.

If you really want to make sure you never see this, you would need to make sure your lines, points, and surfaces were all in different parts, but that is more sorting than necessary for 3D Fluent.
PSYMN is offline   Reply With Quote

Old   February 22, 2011, 13:07
Default
  #6
New Member
 
Adam Arvay
Join Date: Feb 2011
Posts: 21
Rep Power: 6
aarvay is on a distinguished road
Thank you. That is very helpful.

I guess all my BC's are in good shape, according to what you described, they all seem to make sense to me.

I'll keep working on it. For some reason, the meshes I make in ICEM won't converge while the same geometry meshed with the workbench works okay. I still haven't found any important differences between the meshes so I don't know why one works and one doesn't but I'll keep searching.
aarvay is offline   Reply With Quote

Old   February 24, 2011, 12:39
Default
  #7
New Member
 
Adam Arvay
Join Date: Feb 2011
Posts: 21
Rep Power: 6
aarvay is on a distinguished road
I posted a new thread in the fluent forum. Its is related to this thread but more focused on the PEMFC module and fluent than the specifics of the meshing.

PEM Fuel cell module meshes. ICEM vs workbench
aarvay is offline   Reply With Quote

Old   March 14, 2011, 17:15
Default
  #8
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
If the mesh quality is similar between the two models, then this is quite the puzzle...
PSYMN is offline   Reply With Quote

Old   March 14, 2011, 18:21
Default
  #9
New Member
 
Adam Arvay
Join Date: Feb 2011
Posts: 21
Rep Power: 6
aarvay is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
If the mesh quality is similar between the two models, then this is quite the puzzle...

Yeah. The good news is, for me anyway, is that I seem to have figured everything out enough to get some working simulations.

As far as my shadow wall problem, I don't know what the deal is with that. When I use the workbench mesher then and bring the mesh into fluent, the mesh would have wall/shadow-wall pairs between the fluid/solid zones, as long as I assigned all of the parts to the same assembly. this seems to be the proper behavior for these types of simulations.

In ICEM, after i figured out how to use material points and generate decent quality mesh volumes, I was able to bring the mesh into fluent. But regardless of how the material properties were assigned in the bocos, wall/shadow-wall pairs are assigned at the interface between every geometrical part in the assembly. But like I said at the end of the other thread, I could fix this by reassigning the boundary conditions and changing unneeded walls into interiors.

I'm pretty sure I tried putting all the parts into an assembly in ICEM and it didn't change the shadow wall behavior. At this point it doesn't really matter, i found a method that works so I'll stick with it until I push it far enough that it breaks again.
aarvay is offline   Reply With Quote

Old   March 14, 2011, 19:22
Default
  #10
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Oh I understand now, ICEM is different when you create assemblies. If you want the mesh on both sides of a wall to be in the same fluid (so you get the wall and shadow between), you should use the same part for the material points... But then you must also make sure to mark that part as an internal wall under mesh => Params by parts or ICEM CFD will remove it for you.
PSYMN is offline   Reply With Quote

Old   February 5, 2014, 12:17
Default
  #11
New Member
 
John Black
Join Date: Feb 2014
Posts: 2
Rep Power: 0
Cube is on a distinguished road
A really simple solution would be to create a body (in ICEM) anywhere within the fluid (or domain of interest). After this step I exported my mesh using FLUENT and I did not have any problems with shadow walls.

I hope this helps.
Cube 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
[ICEM] domain interface in ICEM for fluent hsn ANSYS Meshing & Geometry 24 November 27, 2012 17:43
[ICEM] Meshing problem from ICEM CFD to Fluent cfdonlinederafa ANSYS Meshing & Geometry 2 September 21, 2010 16:16
Problem in IMPORT of ICEM input file in FLUENT csvirume FLUENT 2 September 9, 2009 01:08
Obtaining Shadow Walls ThinX FLUENT 0 April 22, 2009 14:38
Exporting ICEM Tetra Grid to Fluent with Hexa-Core Tim Main CFD Forum 4 August 28, 2007 04:05


All times are GMT -4. The time now is 18:18.