[dst]

Hi everybody,

I am doing the mesh for a bended tube with some shape variations along (changing diameter by step or using cone connections). ICEM CFD 11.0.1 under Linux is used.

I have some experience with block-made hexa meshes in the areas of wing-bodies or tubes with internal flows. In this case, I would like to proceed without the 3D block-structures and make a Hexa-Dominant mesh for the cylindrical tubes and Tetra for the cone connections.

I am importing the geometry model from CATIA.

I am able to make a full Tetra mesh or to change the core structure from Tetra to Hexa (12 to 1 modification), but I would like to have a bended Hexa mesh (not Cartesian) like I could make using the 3D-block structeres. This kind of mesh were allready generated with the same geomentry by my college using GAMBIT.

If I am trying to make a Hexa-Dominant mesh, I am getting the following error-message:

error orienting normals, perhaps there is more than one region
error in output_region_boundaries
Hex Dominant meshing failed

I have checked and corrected the surface and surface-mesh normals, but it does not influence on the process. There is one closed volume (at least it looks like that), where I have a Body point.

Any suggestion or ideas would be really very appreciated!
Thank you very much,
DST

[PSYMN]

Hexa dominant starts from a surface mesh (quad shells) and grows them inward as far as it can until it eventually fills the core with tetras and pyramids ( junk ) for connectivity.

The error message happens when you have two volumes, but in simpler terms, it happens when you have a shell with a multiple edge (like a T connection). You could get this with a baffle attached to the wall, etc. Actually, this method probably doesn't support baffles at all.

We brought Hexa Dominant into ICEM CFD from ANSYS Meshing years ago. I would only recommend the Hexa Dominant mesher for FEA applications where the nice regular Hexa mesh near the surface is where the interesting stuff is happening.

For a piping assembly with steps and cones, I would just use ICEM CFD Hexa.

Create an Ogrid for the pipe and split the ogrid to make the steps. Contract the ogrid for the cones. If you don't like your hexa mesh density increasing thru the cones, you can convert the central HGrid block (and/or the surrounding Ogrid Blocks) to free.

Note that we have added a lot of functionality to better support unstructured and swept blocks in 12, 12.1 and 13.0 (due out soon). I suggest an upgrade if you can. MultiZone may be able to mesh your entire model automatically.


Best regards,

Simon

[dst]

Thank you Simon!

The mentioned pipe-assembly problem has cones which are punched and got a lot of deepening surface-parts. So that it is quite difficult to make a hexa-block structure for all of them.
I tried to change the cone-approximation blocks from Mapped into Free (the external blocks of O-grid) but ICEM gives a mistake that block XX can not be meshed. Actually, it is meshing some of external blocks (2 of 4 from external o-grid blocks) normally, but two others are meshed just with a surface mesh, without doing any volume mesh. The blocks have the same properties (just switched to Free) and the geometry which they should fit is also looks quite the same way (unfortunately, I am not allowed to post any pictures of the mentioned problem). So I can not see a reason for that.

As a good quality-mesh solution, colleagues are using GAMBIT and making hexa mesh for pipes with some smooth diameter variations along the length using the Cooper tool. The cone sections are done usually with tetra.

As I understood, there is no tool such a Cooper in ICEM CFD. Am I correct?
There is an Extrude tool for extrusion of the surface mesh along the curve, but it does not allow to describe a tube with a non-constant diameter.

There is one other specific property of Hexa in this case when I have the O-grid split twice in "radial" direction to describe steps of geometry. This long block-set (1 central block and 8 side blocks) is describing the pipe which is bended to 180degrees with a small (2-3 diameters) radius. In this case, for all of the 8 internal edges I need to have 8 curves inside the pipe to connect/associate the edges to that curves (otherwise, if I am connecting only 4 outside-edges to longitudinal curves on the pipe-surface, the Hexa blocks are not bending with the same radius as a pipe). So, is there any possible solution for automation of the mentioned process inside the bended pipes/longitudinal structures?

Best regards,
DST

[PSYMN]

With long question, I like to use numbers to hit all the answers...

1) Unstructured blocks were new at the version you are using. We have had man years of development since then. Try upgrading... Maybe wait a couple more weeks and get 13.0. In the mean time, if you got the surface mesh, you can run Delaunay tetra (from the Compute mesh from existing mesh panel) and it will fill the empty volumes in your model with Tetras.

2) The replacement to the Gambit Cooper tool is ICEM CFD Hexa MultiZone at 13.0. It can handle similar situations with multiple source and targets. There are some situations we are still working on. However, it can also handle multiple directions and other issues that the Cooper tool could not handle. It is also a completely flexible and separate hexa blocking layer and there are many advantages in that, including OGrid, Patch Independence, fitting to similar geometries, edge parameter and vertex location adjustment, etc.

3) OGrid splits assume you want to be square in the middle so you have better quality at the corners of the central HGrid. However, you can link the OGrid curvature using "Edit Edges => link shape". The the reference edge is the one that projects to the curves that you have. The target edges will match the radius of curvature * a given factor. Read the Help to see how to use it correctly. Another option is to create construction curves in your model and just associate the edges to those.

[bluelc]

Originally Posted by PSYMN

Hexa dominant starts from a surface mesh (quad shells) and grows them inward as far as it can until it eventually fills the core with tetras and pyramids ( junk ) for connectivity.

The error message happens when you have two volumes, but in simpler terms, it happens when you have a shell with a multiple edge (like a T connection). You could get this with a baffle attached to the wall, etc. Actually, this method probably doesn't support baffles at all.

We brought Hexa Dominant into ICEM CFD from ANSYS Meshing years ago. I would only recommend the Hexa Dominant mesher for FEA applications where the nice regular Hexa mesh near the surface is where the interesting stuff is happening.

For a piping assembly with steps and cones, I would just use ICEM CFD Hexa.

Create an Ogrid for the pipe and split the ogrid to make the steps. Contract the ogrid for the cones. If you don't like your hexa mesh density increasing thru the cones, you can convert the central HGrid block (and/or the surrounding Ogrid Blocks) to free.

Note that we have added a lot of functionality to better support unstructured and swept blocks in 12, 12.1 and 13.0 (due out soon). I suggest an upgrade if you can. MultiZone may be able to mesh your entire model automatically.


Best regards,

Simon

Hi Simon

Have you guys solved the "baffle" problem in hexa-dominant method?

Or is there any approach to generate hexa-dominant mesh for two regions?

I always get errors like "error orienting normals, perhaps there is more than one region".

Thanks a lot

[PSYMN]

No, Hexa dominant is really more for FEA users who tend to generate their models as multibody parts... (non conformal bodies)...

I think you should probably be trying a different method. Perhaps MultiZone? Or perhaps Octree tetra followed by converting 12 tetra to 1 hexa?