How to set bocos on 2D model for ANSYS CFX (tuts no help)
I'm trying to mesh a basic shape in 2D for use in ANSYS CFX (hence it needs to be one cell thick). I need to refine the mesh near the bottom wall and set up all the boundary conditions.
I've managed to produce a suitable mesh to start with, but can't work out how to set up the boundary conditions at various locations on the model/mesh:
generated points (in one plane/2D only)-> generated curves -> generated surface -> meshed this surface via blocking -> extruded this mesh by one cell
Can I set the boundary conditions from where I am now or do I have to use a different method?
The other method I've tried is:
generate points in two planes (a 'front' and a 'back' very close together) -> connect all the nodes/points via curves to get a very thin 3D (pseudo 2d) shape -> generate surfaces from each side of the shape
Do I set boundary conditions somehow from here?
From here I do surface meshing then volume meshing?
I'm doing the meshing in ICEM CFD because the inflation layer tool in the meshing in ANSYS Workbench is not refinining the mesh near the corner (see image below) at all and I don't appear to be able to control how high the inflation layers go.
So it looks like you have to create parts to create locations for the boundary conditions.
However, when I go to set the boundary conditions via Output -> Boundary Conditions
Then select the part in question and click on "create new" I don't get a list to select a boundary condition from. (Select Solver set to ANSYS CFX for Output and ANSYS for Common Structural Solver).
When I change the Output solver to straight ANSYS however, I get a list to select a boundary condition from. The problem is that the ANSYS solver does not provide the CFX style boundary conditions.
Any idea what is wrong?
Different mesh file formats support different boco info...
Right, use parts in ICEM CFD (or named selections in ANSYS Meshing). Not sure why you are not getting what you want our of ANSYS Meshing, but I know it is capable. There are different controls for prism to turn on or off stair stepping and to control the prism by smooth transition (what you have) or by initial height, growth ratio and number of layers (what you want), so maybe give it another shot. Or perhaps this is a 2D limitation, I usually use 3D.
As for the boundary conditions... ICEM CFD supports over 100 solver formats. Not all of them provide a great way to setup bocos directly in their mesh file.
In this case, CFX would prefer you to create the mesh with the part names and then setup the bocos in CFX Pre, so just open the boco file, hit apply and export the file.
However, your next question would be when CFX Pre rejects your model because it doesn't accept 2D models. It actually requires them to be one cell thick (2.5D) so you would need to extrude, etc.
However, CFX can read in 2D models if they are in Fluent mesh format (it auto converts them from 2D to 2.5D)... And Fluent Bo-co setup is more complete (you can set "Velocity Inlet", but the mesh file won't contain the velocity magnitude, that is in the case/data file, so just set the boundary types in ICEM CFD and then setup the numerical values in Fluent), or you can do it the same way and just set the part names in ICEM CFD, which will default to "Wall" and can be edited easily in CFX Pre or Fluent.
boundary in ICEM CFD is missing in OpenFOAM
Using parts in ICEM CFD v13.0, generated and then exported a mesh to Fluent6.0 but when I convert this to OpenFOAM (fluent3DtoFOAM), one of my boundaries appears as a "zone" and not a boundary. The difference between this surface and all others is that it is an internal boundary.
I have tried to force the boundary through ICEM's "output" tab but this is clearly for periodic conditions.
Any explaination for what I am doing incorrect?
Sorry, I am going back thru some older posts (I was on vacation at this time) seeing if there are any that looked interesting...
I am not familar with any special needs of OpenFoam, but are you sure you have shell elements in this internal part? You can get a quick count for each part by running info => Mesh info.
If you do, then that should be enough.
If not, maybe post this on the OpenFoam solver site and see if anyone there knows more about this problem.
If you have since figured out the problem, I would be interested to hear the solution. Perhaps it is something we could fix on our end so other users have an easier time.
|All times are GMT -4. The time now is 07:50.|