Where did I get some of this information?
Most of this was adapted from Section 4.6.2, page 448 of the ICEM Tutorial Manual, called “Hybrid Tube”
For any other hints I would check out CFD online which is where I find other hints and tips. The link is given here.
If you have any comments or suggestions, please let me know. Especially, if you can help with some of the problems I am having which are in RED
What is a hybrid mesh?
A hybrid mesh is one where the mesh is both structured and unstructured. A structured grid usually contains hexahedrals and can be created through the BLOCKING tab in ICEM. An unstructured grid usually contains tetrahedrals shapes and is irregular meaning it can usually be used for strange or unusual shapes. This flexibility is extremely useful for complex geometry, where a structured mesh may be difficult to create around or in the shape.
Most of the time, unstructured meshes are used in finite element analysis which may look at stresses / heat transfer etc, where diffusion is much greater than the convection. However, in fluid dynamics a finite volume method is usually taken which involves structured meshes which are better for problems where convection dominates the diffusion of a particular scalar, e.g. the heat transfer to the surrounding air from a pie on the window sill is more pronounced than the heat transfer from the random movement of molecules in the air (diffusion).
A hybrid mesh is then useful in computational fluid dynamic (CFD) when fluid flow wants to be resolved accurately but also with the need to go around complex geometry, as shown in the picture at the top of the page of a swirl burner that I am working on, the design of which is by Cambridge University. The bottom half is structured since it is just the pipe that I am modelling and the top half is unstructured since the blades I had some difficulty when trying to use a structured mesh around them.
How to do an hybrid mesh in ICEM
I am assuming that the basics of ICEM are known. For more details, please see the user guide and learn how to do the basics before attempting this. The manual gives over 1000 pages of tutorials, and once you have learned how to do the first 200, you should be pretty confident to do this (maybe).
1. Create your geometry (either from scratch or importing, perhaps through a cad drawing)
2. Create surfaces that enclose your geometry. Afterall, you don’t want the fluid to leak out! Not that it would. The program would just moan at you. A good idea is to do a CHECK GEOMETRY option, which should point out any errors and delete any extra surfaces, curves, points etc… Always check it visually though. I find sometimes this tool can add in extra surfaces or lines which should not be there.
3. The important part. You want to tell ICEM what part you want to mesh as unstructred and the parts you don’t.
- Create surfaces which you know will connect both the structured and unstructured meshes, call these “INTERFACES” under the Create Part option. In the example I have, I have a surface at the bottom of the blades and then a few surfaces after the blades which enclose the whole volume that I want to mesh. SAVE!
- Create a body inside the volume you want for an unstructured mesh. Go to Geometry ->Body -> Create Body -> By 2 points, and select two points inside the volume. Click “Apply” and ensure that the body you created looks as if it is inside the volume you want to do a tetra mesh. SAVE!
- Click “Mesh” and go to both “Curve mesh setup” and “Surface mesh set-up”. Set the maximum number of nodes to what you desire.
- Compute the volume mesh.
- This might take a minute, or crash the computer if you’ve set the nodes too small. If it does crash, then reload the saved file and try with less nodes.
- Once the mesh is created, go to File -> Mesh -> Save Mesh as, and call it something like “tetra-mesh.msh”
- Close the mesh. File->Mesh->Close Mesh
- Use the blocking tool to create the correct structured mesh and be sure, after editing the block, delete the block which you were previously working on. I always do this first to ensure that I don’t have multiple blocks to eventually delete.
- Once blocking is finished and using Pre-Mesh to check everything is associated properly, go to File-> Mesh -> Load from blocking.
There should not be a warning sign here about merging or replacing the mesh. If there is, hit “cancel”, and save as & close your unstructured mesh: File -> Mesh -> Save Mesh as , then call it something like “tetra-mesh.msh”. Now go to File -> Mesh -> Close Mesh.
- File -> Open Mesh. Open the mesh titled, “tetra-mesh.msh” or whatever you called it.
- Warning box should appear asking if you want to replace or merge it. Click “merge”.
- At this stage, if the mesh was loaded into FLUENT, interfaces would appear and the mesh would be non-conformal. However, for a more consistent mesh we wish to join the nodes.
Go to Mesh -> Merge Nodes and select by part the INTERFACE, one at a time (unless they are connected e.g. two interfaces connected together along an edge). Click “Apply”.
- The nodes should merge.
- Export the mesh in the usual way
- Load in the mesh. Go to the boundary conditions and change the interfaces from INTERFACES to WALL. Then from WALL to INTERIOR.
As I mentioned at the beginning of the post, I wanted some help with the items in RED.
Joining the nodes. This is fine and works, but appear to give me a very bad mesh quality and skewness. Is there anything that can be done to help improve the quality of the mesh other than smoothing?
Thanks for reading!