[PietW]

Hello everyone,

After a few days of trying my best on my own, I now reach out to seek your help. I was reading other forum posts and tried everything that came to mind with the trial & error approach. I was yet unable to resolve the issue. I am working in ICEM CFD and want wo export to CFX.


I am trying to generate a mesh inside the big box. This box also has an inlet and outlet. Every Body inside of this box should be solid and thus not meshed. At least that’s what I think is the reason to create more bodies inside in the first place

I was able create a nice tri mesh for all surfaces and using a Delaunay approach for the volume mesh. The first picture shows the geometry of the project I had no problem in meshing both volume and surface mesh. The thin sheet in front and around the solid disk is not a body but I defined the surfaces of that part as wall in CFX Pre. That works fine.

I proceeded to include the internal geometry as a whole bunch of surfaces. Even though I might not have chosen the most elegant way to create all the surfaces needed, it still worked and there should not be any overlapping surfaces or holes. (Picture Nr. 2)

The surface mesh looked fine to me. Sadly, this approach didn’t work out for me as the volume meshing failed afterwards using a Delaunay approach. I would describe it as the nodes and vertices snapping out of bounds. Suddenly the whole mesh is trash. I was not able to spot the problem in this mass of surfaces, so I started dividing the big internal geometry in smaller boxes. After some initial trouble defining the body correctly I was able to use my basic geometry and include a box which I was then able to mesh as I wanted. I created a nice tri surface and Delaunay volume mesh again. The disk in front of the outlet and the newly added box both were not meshed on the inside. I figured they are correctly defined as bodies and have both no holes. (Picture Nr. 3)


Now my actual problem began. After adding the second box I got the same corrupted volume mesh as I got when trying to mesh and implement the inner geometry as one big part.

I tried several different boxes and constellations. It turned out that everytime a box is touching another box (picture 4), the created volume mesh is corrupted. You can see the resulting volume mesh in picture 5.

Can anyone help me with that issue and explain what I am doing wrong? Maybe the problem lies somewhere earlier in the project but I just don’t realize it.


Thanks for reading. I’m looking forward to your replies.

[Stel]

I'm not 100% sure if I understood the problem, but I have some suggestions:
1 - Why are you creating bodies inside volumes you don't want to mesh? If what you want to mesh is the bigger box enclosing the other ones, create a body there and delete the bodies inside the boxes where no mesh is expected to be created.
2 - The two rectangular bodies that are touching each other, they can be simplified to a single one. That is, try to delete/recreate surfaces so that no different surfaces would be touching each other. ICEM could be understanding that there is some volume between them. So, try to unify them together as a single contiguous volume (pretty simple using ICEM own geometry features). The problem could be this: when you see the two rectangular (solid boxes), the upper face of the lower one has some overlapping area with the upper one; ICEM should mesh the non-overlapping area, but not the overlapping one (this is what you expect), but right now as the whole surface is probably named as a single part it may not understand this for some reason (that is, maybe it doesn't understand that the surface mesh has to stop at the edge dividing the overlapping and non-overlapping areas between the rectangular boxes).

[siw]

I do not fully follow your description of the geometry and what you are doing. I looks simple enough though. You did not say how you made the surface mesh. Anyway, a few steps:

1. Ensure you make Material Points in the fluid regions. You can make ORFN points inside the solid regions where you do not want elements.
2. Run Build Topology.
3. Use Octree volume mesh. Delete the volume elements. Check and smooth the surface elements.
4. Use Delaunay with TGlib On and Use AF to generate new volume elements. Check and smooth the surface and volume elements.

[PietW]

@Stel:

Thanks, I actually dont need to define any more for the parts that should be solid.

The rectangular bodies that you want me to simplify to a single one seems to go back where is was before. I started with this geometry as a single part with coherent/touching surfaces. That sadly didnt work out. Thats why I tried it with separate rectangular bodies in the first place. Sadly the Problem persists even when I remove all overlapping surfaces.


@siw

Well, I have a Box that is defined by the 6 walls an Inlet and an Outlet. Every Geometry that I place inside the box should be solid.

I really like your Idea of creating and Octree volume mesh with my geometry and remove the volume mesh. maybe this way I can achieve a surface mesh with sufficient quality for the delauney volume meshing.

Build topology confuses me. It creates new parts and faceted surfaces that I dont see as helpful. I might have to figure out exactly how that tool works.

~~~


Meanwhile I was able to create and mesh all parts in my project except for this complex body (Picture 2 of original Post). I will try @siw 's ideas and post an update. Sadly I will be on vacation the next week so I hope this thread won't be forgotten until then.


Thank you both very much for your ideas and help!

[siw]

You need to use Build Topology before running the Octree mesher, you'll need to read the User Guide. The method I listed (which I have mentioned in previous posts) makes a better quality surface mesh. Remember that your element sizes will follow the Octree rule of 2^n (n is integers and 1 over integers).

[PietW]

Hello Stuart,


I'm really thankful for your help. I was able to fix my errors with the build topology and analysing tools like curve color by connectivity. Sometimes taking your time and simply reading all the user guides provided by the help tool in Ansys is all that it takes.