[pmtgt]

Dear Community,

This is my first post and I'm relatively new to CFD. I am working through a problem that was originally designed to be meshed in GAMBIT but I am trying to do it in ICEM. The problem is to model a single channel PEM fuel cell which consisits of the following zones for both halves of the cell (anode and cathode) and also a fluid porous membrane zone separating the two halves:

From outer to inner

Solid Current Collector (CC)
Fluid Flow Channel (FC) running through middle of CC (open space)
Fluid Gas Diffusion Layer (GDL) connected to FC and CC (porous)
Fluid Catalyst Layer (CL) connected to GDL (porous)

I created the geometry in workbench first of all and then also from co-ordinate points in ICEM. Each zone is rectangular so to mesh it I am simply splitting the geometry into blocks, associating edges and curves which all directly overlap in space and then adjusting pre-mesh parms to get the fine grid I desire.

To model the fuel cell in Fluent I have also labelled several surfaces which are important for the physics, such as the inlet and outlet of the flow channels on each side, the outer faces of the current collectors are terminals and the flow channel sides, cell ends and cell sides are all defined as walls.

My problem now is that there are several adjacent fluid zones with surfaces that are not important for this model and I have labelled them as interfaces and set the boundary conditions in ICEM. Once the mesh is loaded from the blocking I have tried to split these internal walls (which, necessarily or not, I have also ticked as internal walls in the part mesh setup) so that I can define the mesh interfaces in fluent and have two surface to link together. However, not all of the interfaces are being picked up when I select "split internal wall" and some of the surfaces I've set as being walls are being picked up.

Any light that can be shed on how to properly define interfaces and how ICEM decides which ones to let you split would be greatly appreciated. It may be that I have done something wrong or it could be a bug in ICEM.

I am happy to send files or pictures as the files are quite large.

Many Thanks

Tom Tranter

[macfly]

Hi Tom,

Look at the attached figure. It's a rectangular duct with inlet/outlet. Geometry is made of 2 adjacent rectangular parallelelepipeds. Blocking is made of 2 blocks, each block having a different name (create part\blocking material...). This way the internal wall between the 2 fluid zones in preserved in the output mesh. Apply interior boundary condition to the internal wall.

Hope it's what you were asking for!

[pmtgt]

Thanks for the reply but this isn't working for me. The way it seems to work is to define the boundaries between adjacent fluid zones as interfaces and then use the split mesh tool under the edit mesh tab to give fluent two surfaces to link together as an interface.

I'm not sure what the difference is between an interior or an interface, my guess would be that interior surfaces are produced in the meshing process to aid the creation of mesh elements and bear no significance on the physical processes being modelled whereas interfaces can represent a boundary between two physically different regions...

I've now managed to create a mesh that runs in fluent as some of my boundaries can be split in ICEM and for the rest fluent creates corresponding surfaces to link together. My intial question is still open though and I am now getting problems with reversed flow but that's for another forum.

Thanks once again for your suggestion

[macfly]

Originally Posted by pmtgt

The way it seems to work is to define the boundaries between adjacent fluid zones as interfaces and then use the split mesh tool under the edit mesh tab to give fluent two surfaces to link together as an interface.

The surface between the 2 fluid zones is defined as interior, not an interface.

No edit mesh, split mesh, etc., is necessary. What's important is to have the blocks in different parts (e.g., fluid_1, fluid_2) in order to preserve the interior surfaces between the blocks. Otherwise, if all the blocks are within one part, the interior boundaries between the blocks vanish in the mesh output.

[pmtgt]

Ok, I started from scratch and defined all the internal fluid to fluid boundaries as interiors and the mesh works in Fluent. - Thanks.

Just to clarify then, when should interfaces be used?

[macfly]

Good. I'm not familiar with interfaces, haven't used them yet.

[AA29]

Hi guys,

I need to extract some internal faces in a hexa volume mesh(in ICEM itself) to create a faceSet(i need it in OpenFoam). Is it possible to do so? i.e. if i create two different block parts will I be able to extract the surface mesh between those two blocks ? Please note that I do not have an interior surface(geometry) where I am splitting the blocks, I just need that faceSet. It creates problems for me later in OpenFoam, if I have an internal boundary surface.

Thanks.

[FORGODSAKE]

Screenshot 2021-05-17 002808.jpg
I want to do simulation for a microchannel with Water and air. water is flowing in main channel and air is there in 8 column. i thought i have to create seperate meshes for both and i did it. as shown in attachment. is it the right approach. i want to give slip boundary condition for air water interface. after setting BC following error is shown WARNING: Mesh has uncovered faces.
Done
WARNING: Mesh has uncovered edges. ANSYS 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
Done with translation.
Could someone please help me with this. Thankyou in advance

[bluebase]

Originally Posted by FORGODSAKE

Attachment 84384
I want to do simulation for a microchannel with Water and air. water is flowing in main channel and air is there in 8 column. i thought i have to create seperate meshes for both and i did it. as shown in attachment. is it the right approach. i want to give slip boundary condition for air water interface. after setting BC following error is shown WARNING: Mesh has uncovered faces.
Done
WARNING: Mesh has uncovered edges. ANSYS 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
Done with translation.
Could someone please help me with this. Thankyou in advance

You might want to open a new post next time for a new problem.

Moreover, what did the search yield regarding the error message?
You might learn quickly, that uncovered faces is a very common beginner's issue, so there are dozens of threads.

Anyhow, to solve it, you need to check your boundary edges/faces. Every boundary needs to be associated. Really. All of them.
If there is an edge left unassociated (not green), then no boundary elements will be created for that edge when converting to unstructured.
But Fluent (and other solvers) needs boundary elements.


After converting to unstructured, hide everything but the line elements. You'll need to find edges which did not result in line elements (in case of 2d).