CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   [ICEM] Shadow walls in Fluent. ICEM meshes vs Workbench (

aarvay February 18, 2011 11:50

Shadow walls in Fluent. ICEM meshes vs Workbench
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 February 18, 2011 16:38

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.

PSYMN February 19, 2011 14:17

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.

aarvay February 22, 2011 11:41

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.


PSYMN February 22, 2011 11:47

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.

aarvay February 22, 2011 13:07

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 February 24, 2011 12:39

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.

PSYMN March 14, 2011 17:15

If the mesh quality is similar between the two models, then this is quite the puzzle...

aarvay March 14, 2011 18:21


Originally Posted by PSYMN (Post 299404)
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.

PSYMN March 14, 2011 19:22

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.

Cube February 5, 2014 12:17

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.

aravind vashista January 12, 2017 13:51

i have a similar issue, i have a wedge shaped internal body which has holes in it (the holes are inlet for fuel).I separately create 2 parts one for wedge and other for holes within wedge. no matter how i create block and mesh i will get either 2 sided or mixed/unknown surface for the holes. which fluent will not read. can u tell me how to rectify this?

All times are GMT -4. The time now is 08:12.