Inner geometry gets lost exporting mesh from ICEM CFD to CFX-Pre
I have a problem while exporting mesh from ICEM CFD to CFX5Pre.
I hope you can help me!
For better understanding I'll tell you in a few sentences what i intend to do!
I have to do a simple CFD-Simulation how an additional tube in a test chamber influences the air flow.
First I build a CAD-Model of the test chamber with CATIA V5 and imported it as in .igs into ICEM CFD.
There i referred the surfaces to different parts.
I'd like to create a mesh with 10 layers of prism around the tube and the small nozzle, the rest of the volume should be filled with tetra.
I created the mesh as follows :
Register Mesh - Compute Mesh - Prism Mesh.
There i selectes the parts for the prism layers and clicked "ok".
Then i clicked surface mesh up, chose the surfaces of the tube and the small nozzle and applied.
Then: Register Mesh - Compute Mesh - Volume Mesh. I enabled create prism layers and computed.
The result looked good so i exported it with the Register Output - Select Solver. I chose Ansys CFX and ANSYS and applied.
Then Register Output - Write Input and enabled BINARY instead of ASCII.
The result is shown in the image icem_cfd_mesh!
Then i started CFX-Pre - New case - Simulation Type: General
Click with the right mouse button on mesh - import mesh - ICEM CFD and chose the created .cfx5-file.
As you can see in the image ifx-pre i "lost" the whole inner geometry!
Where is the mistake?
Since ICEM CFD needs a closed volume for creating a mesh i closed the former open in- and outlets at my CAD-Model.
If i don't close the CAD-Model my inner geometry still appears at CFX-Pre but the mesh now is also outside the test chamber, shown in image CFX-Pre_Open
I would be very thankful if someone has an idea...
You should create material points (also called Bodies by ICEM) which are nothing more than points that give your volume elements a name. Do this for every region of closed surfaces you have. Each Body should be place inside the set of closed surfaces you're representing.
For any region where you don't want mesh to be generated, create a material point named 'ORFN'. This will tell ICEM to ignore that region (it seems like this is the step missing from your script).
By the way, although possible, ICEM might loose itself if you create the prismatic elements before tetras. So try this instead:
- first create a mesh using the Robust (Octree) method
- smooth the surface mesh using the Laplace algorithm
- recreate the volume mesh now using the Delaunay method and keeping the surface mesh previously generated
- smooth the new mesh again
- generate the prism layers
- smooth the mesh several times freezing the prismatic elements
- do one last smoothing step lowering the desired quality by one or two orders of magnitude now including the prisms
Hope this helps.
Thanks Bruno :)
But one question: Refer your hints to the first configuration with the in- and outlet closed or to the second one with the open holes?
...and i don't know if it's important, but i forgot to say that my CAD-Model is a surface model, no solid...
I have created the Bodies now. But before that, i added surfaces to my CAD-Model, which means that i have closed the nozzles and the tube with each a surface at the beginning and at the end. So i got several volumes surrounded by closed surfaces.
I believed that this is necessary?!
Then i created a tetra volume mesh.
Now i wanted to create the prism layers around the tube and the small nozzle.
The result looks strange :confused:
You can see it in the Image. I hid the outer wall of the chamber!
I hope someone can help me...
|All times are GMT -4. The time now is 14:50.|