Is there any way to create a grid that looks like this?
 

Hi guys,

I'm trying to get a grid that looks like this (see attached picture) in Ansys meshing 13. My problem is, that mapped face meshing in the center region leads to strongly distorted elements. Is there any way to do this more handmade instead of the auto-tools?

Thanks for any help!

Hi Rodrigues,

Yes it is possible to create this type of mesh.

In Gambit:
Firstly, you should create or import the boundary edge geometries.
Secondarily, mesh these edges with gambit edge mesh menu.
Finally mesh the surface with structured quad elements.

In Gridgen: There is a tutorial about this geometry. (Tutorial 2: 2D Bump)

Thanks husker,

I will try to do the tutorial first...

In ICEM CFD hexa, it is just a CGRID around the bump.

I'm currently learning to mesh with ICEM... not too easy :cool:
What I tryed to do is:
-create and export the geometry with design modeler
-create the grid and all "named selections"
-export the setup for FLUENT
Is this the best way?

That is not ICEM CFD, that is ANSYS Meshing...

To do this in ANSYS Meshing, you could draw out the segments as you want, imprint them on the geometry in DM. Then once in ANSYS Meshing, you could right click on the mesh tab to insert a mapped method on these parts...

Then compute mesh and away you go.


In ICEM CFD (which does have some learning curve, but once you learn it is the most powerful hexa tool on the market), you would start with a rectangular 2D block and associate it with the "corners" of your geometry. Then split around the bump (3 simple split commands) and insert a CGrid (one command). Then delete the central HGrid portion of the CGrid (one command) and associate the edges to the curves. With some hexa practice, you could do it in a minute or two.

I guess my post was missleading. Up to now I used ansys meshing. Now, I want to give ICEM a try. Thats why I used the geometry that I allready created with design modeler. I exported the geometry to open it with ICEM. My plan was to create and export a grid and open this with FLUENT. The question is: Is this way ok, or completely bad?

Sure...
 

Oh yea, thats fine. Save the AGDB file in DM, open that with ICEM CFD (File => Workbench Readers), then block it, convert to unstructured mesh, output to Fluent... Fluent Bocos and Zones are applied based on Parts in ICEM CFD. So if you want one end to be an inlet, make sure you create a new part named "INLET". If you create these as Named Selections in DM, they can be imported, but you need to check the right box. If they come in as geometry subsets instead of Parts, you can right click on subsets and turn them into parts.

Some things to watch out for... Fluent expects this in the Z=0 plane. Also make sure you associate all the perimeter edges to curves or you will get a null pointer error due to your uncovered edges.

Great, this is the first time where I got it running. Thanks!!!

Update: Your youtube tutorial is great and solved nearly all of my problems!!!

I uploaded a picture of some random test. Just for my understanding: Why doesn't the grid line stick to the block in the middle part of the c-grid (but it is bended)? It seems to work at the left and right part and at all other block edges.

It is trying (and succeeding) to raise the quality in that acute 5 element corner.

You could slide the corner nodes a little so the angle is more balanced and you would get a more even result between the three edges. (my recommendation)

If you want to force it straight regardless of quality, just add an edge split in the middle of that edge and use it to straighten out the edge.

You could also just leave it alone. The quality is good enough for any solver. You don't actually need straight lines. You should probably adjust the o-grid edge distribution first and see how it looks then.