[AKll]

Hello together,

After using Surface meshes and Delaunay to build up my mesh for a while, I found that the unstrucutred mesh is too coarse in a region of interest.
My solution for this is to implement an inflation layer.

My problem with it is, that I am unable to integrate a prism mesh during the usual surface + Delauny meshing process. It fails. (Error: open edge encountered. prism terminated prematurely) or it just puts the error after a certain layer.
Also trying to add a prism layer after surface and Delaunay volume meshing fails.

So, I switched to Octree with prism (and also tried adding it after but the outcome is similar), which tends to work, however, now I have these local misdistributed areas, in which very large elements are created that exceed the max size limit I set. See picture.

Now, my question would be that maybe someone already encountered this problem and has a solution at hand or an idea on how to go about it?

I spend a lot of time trying to change the prism layer settings and min and max size of the general mesh settings, but this problem persists.

Thank you in advance and for reading!

[Gert-Jan]

The current picture shows 2 surfaces that overlap. Is this the case? Then you won't be able to mesh it anyway. You need to make sure they match perfectly.
Better show your geometry in 3D, and explain where you want prisms and where not.
If you have a "thin cut" where the surface touch, then look for "thin cut" with specific settings.

[AKll]

Originally Posted by Gert-Jan

The current picture shows 2 surfaces that overlap. Is this the case? Then you won't be able to mesh it anyway. You need to make sure they match perfectly.
Better show your geometry in 3D, and explain where you want prisms and where not.
If you have a "thin cut" where the surface touch, then look for "thin cut" with specific settings.

Thank you for your reply!

I noticed, that my picture leaves room for interpretation without further comments.

It is indeed a 3D mesh.
It shows the shell mesh of 2 surfaces that are spanned at a near 40° angle.
There is a bottom surface, which I hide for presumably more clarity, which basically is just a flat surface on the buttom on which the inflation layer is set to.
So both walls, the green and the yellow surface, have the correct inflation layer build on the bottom.

The problem itself doesn't seem to be with the inflation layer, it is with the Tetrahedra mesh above the prism elements. At some local points in the mesh octree seems to fail to keep the general mesh sizing.

This results in huge elements with sharp angles.

I added a cutplane view of an other part of the mesh. Before, meshed with octree and after with then added prism layer.

However, this problem persists, when I do add prism layer during the initial octree volume meshing as well.

[Gert-Jan]

What version of ICEM are you using?

[AKll]

This is with ICEM CFD 2023 R2

[Gert-Jan]

Using Octree,
- Step 1: create a nice Tet mesh as good as possible. Smooth, smooth, smooth as far as possilble.
- Step 2: Create a prism mesh using the following settings:
Prism height limit factor 0.5
Number of surface smoothing layers 1
Number of volume smoothing steps 1
Max directional smoothing steps 10
First Layer smoothing steps 15
- Step 3: Global Smooth Tets (fix prisms)
- Step 4: Smooth all elements, but smoothing step by step. Carefully watch what the elements do.

[AKll]

Thank you very much!

I will do this and reply when done.

[AKll]

This method did work!
Thank you very much, I was able to fix the issue with the unevenness in the elements!

However, I am still not able to use the mesh in CFX.
I can import it and set up my boundary conditions.


But there I notice a disbalance in the scattering of the arrows at the inlet. (see picture) (I had to hide the actual geometry inside)


They are prominently gathered at the top part on the inlet of the my mesh.
there is no wall or bump or anything behind it, it's a straight channel until the geometry starts further back.

Is this due to still relatively bad mesh quality?
Are there any pointers?



The simulation doesn't start, I am getting an "out of bounds" error

[Gert-Jan]

it can be anything.
However, my first guess is that it is in your mesh. And therefore the problem is in your ICEM geometry. Possibly there are multiple curves very close to each other on the edge that you are looking at. Zoom in a lot, take a close look (hide surfaces, make curves thick) and make the geometry as clean as possible. I think you need only one curve per edge. So, I mean "remove all curves (and assiciated points) that are not strictly necessary to span up your geometry".