[Pj.]

Hi everybody

I'm a newbie of Pointwise, while I worked a lot with snappyHexMesh, so maybe what i'm saying is just wrong.

I'm trying to obtain two blocks, both of cubic cells. The first one should be made of 10x10x10 cells, while the second should be made of 5x5x5 cells.

I create the first one extruding a patch made of structured 10x10 faces.

Then i don't know how to tell PointWise to change one face from 10x10 faces to 5x5 without alter the previous block.

Is this possible to do this in PointWise?

EDIT: I attach an image of what i would like to obtain. To do this picture I moved a second block close to the first one, but they are seen as two separate zone of the mesh with no common face.

Thanks

[cnsidero]

Luca,

Pointwise doesn't have a split-hex capability like snappyHexMesh does. There's two approaches you can take. The way your mesh is now, there is a non-pointed matched interface between the blocks. Non-pointed matched interfaces can be coupled in OpenFOAM with AMI (or GGI depending on the flavor of OF you're using) boundary conditions. You'll need to set a 'patch' type boundary condition on each of the non-pointed match domains in Pointwise. Once you've exported the mesh to OpenFOAM, you'll have to edit the type of those patches in the constant/polyMesh/boundary file from 'patch' to 'ami' (or 'ggi').

If you'd rather stay away from the non-pointed matched approach, you can create a transition block using tet cells. Creating a gap between your blocks with enough room to fill the void with an unstructured block. I've replicated your mesh strategy but moved the blocks apart by the distance of the cell height in the coarse (5x5x5) block. Then I created 4 unstructured domains to close the gap and created an unstructured block using the 4 unstructured domains and the structured domain from the adjacent structured blocks (see first pictured). Then initialize the block (see second picture). The resulting quality was really good in the transition block.

Let me know which approach you use and if you have any further questions.

-Chris

[Pj.]

Thank you Chris.

Honestly I prefer to avoid the AMI/GGI boundary condition.

I already though to create a transition block and I think I'll choose this approach.

I also though that a possible approach could be to create all the mesh as 10x10x10 and then refine it using snappyHexMesh or the refineMesh command in openFoam. Do you think this is a doable approach?

Since i started using pointwise one week ago, I was indeed asking if there was a way for pointwise to do such thing: your answer is perfect: NO.

Thank you very much for the answer.

Luca

[cnsidero]

Originally Posted by Pj.

I also though that a possible approach could be to create all the mesh as 10x10x10 and then refine it using snappyHexMesh or the refineMesh command in openFoam. Do you think this is a doable approach?

Yes, good idea. So the third approach would be to create two blocks of the same resolution - this ensures the interface is point matched. Then to facilitate refinement using the refineMesh create a volume condition for the block you want to refine, name it and change the type to 'volumeToCell'. Before exporting the mesh go to CAE, Set Solver Attributes and ensure CellExport is set to something other than None. Use Sets or SetsToZones as the refineMesh utility can modify a set of cells (check out the sample refineMeshDict). Set FaceExport to None.

The purpose of doing this is to group the cells into a set to make it easier to refine them with refineMesh.

[Pj.]

Thank you very much for the last tip. I'll look for those options.

I'll keep you posted on the result.