[adi.ptb]

Hi Zach,

Thanks for your response. Regarding the overlapped blocks and the fix to this problem that you pointed out it seems like a hard work. Do you mean that I should skip the current topology that I have (delete the farfield geometry) and start with the surface mesh and use connectors to create the same farfield that I already created with CAD? And what happens to the surfaces that I don’t want to extrude them?

Best Regards

[RcktMan77]

Hi Adi,

You don't necessarily have to delete everything. You just need to redefine the connectors normal to the surface and farfield mesh boundaries. Rather than having these connectors extend from the farfield boundary all of the way to the surface mesh, you instead want to re-define them to extend from the farfield boundary to the extent of your extrusion away from the surface.

Doing so is likely going to blow away the unstructured block you created as well as some of the domains that used these connectors. Unfortunately there isn't much getting around this as they were not defined correctly from the outset. However, re-creating these domains and the corresponding block shouldn't take but a few minutes of additional time.

Best Regards,



Zach

[adi.ptb]

Hi Zach,
Thanks again. I hope to resolve this quickly.

[adi.ptb]

Hi Zach,

I’ve been going through PointWise’s tutorials to practice a little bit and then started to generate meshes for some simple geometries. So I generated a mesh for simulating the flow over a flat plate using OpenFoam and I ran into a problem. The problem is that when I export the mesh to OF and run the checkMesh in OF the checkMesh is ok but when I run the case after two iterations the simulation diverges. I’m 100 percent sure that this is due to the mesh export in PointWise because when I use other mesh generators with the same BC and everything the results are ok. Even when I export the mesh to FLUENT in PointWise and run it in FLUENT the results are ok. I wanted to know what the problem is? I setted the volume BC to volumeToCell. Also I wanted to ask you if there is a way to export the .msh file for fluent instead of .cas file so that I can convert the fluent mesh to OpenFoam.

Best Regards,


Adi

[tcarrigan]

Hello,

You'll need to run 'renumberMesh -overwrite' to minimize the bandwidth. Pointwise does not export the grid in a bandwidth minimized fashion, so often the bandwidth will be on same order of magnitude as the face count.

Travis

[adi.ptb]

Hello Travis,

Thanks very much for your response, I did as you said but OpenFoam printed another error: "cannot find patchField entry for SYMMETRY"

[tcarrigan]

You'll need to check your 0/ directory and initial conditions to ensure you specified the symmetry conditions correctly. Also, in the constant/polyMesh/boundary file, ensure the type is set to 'symmetry' rather than 'symmetryPlane'.

[adi.ptb]

Hi Travis,

Thanks so much for your reply. I checked initial and boundary conditions and they are ok. The symmetry boundary is also set to symmetry but still have the same problem. You can check the files for yourself.

Thanks
https://www.dropbox.com/s/upxahwkmouzgu9p/pw.rar?dl=0

[tcarrigan]

It can't find the entry for SYMMETRY. That means you have "SYMMETRY" defined as a patch and it can't find the entry. You'll need to look through your case again. My guess is there is a difference in what you call the symmetry patch in your 0/ directory and what you call the same patch in your constant/polyMesh/boundary file.

[adi.ptb]

Hi Travis,
Thanks for your response. I fixed the problem. Thank you so much

[adi.ptb]

[QUOTE=adi.ptb;606921]Hello PointWise Users,

I have a problem that I need to simulate but first I have to generate a high quality mesh for it and a mesh with full control. The problem is a lobed mixer. It consists of an annular duct formed from concentric pipes, where the trailing edge of the outer pipe is shaped into 12 lobes that are uniformly spaced in an axisymmetric manner around the centerline. The trailing edge of the inner pipe closes to form a conical plug. I have attached the pictures of the geometry. The computational domain is circumferentially sized to include only a quarter of the flowfield, with periodic conditions imposed on the two circumferential ends of the domain. I think I have provided enough information about the geometry and computational domain and it’s time to talk about a kind of mesh that I must generate for the computational domain.
The mesh should be as follow, the surfaces of the lobes and the conical plug must have structured hexa cells except for the nose of the conical plug. Also some inflation layers around the lobes and tri cells for the volume mesh. I was asked to mesh this domain in ANSYS ICEM CFD but after a week struggling with ICEM without any progress I searched for other solutions. Actually, creating so many blocks for the lobes and plugs are very tedious in ICEM. It gets really messy. It’s been 3 days since I have found this great mesh generator (PointWise) and I’m thinking about shifting to it. I worked with its tutorials and it’s really flexible and highly automated which can save a great deal of time for complex geometries like what I have In hand.
So after working with PointWise a little bit I gave the problem a try and I was able to generate the kind of surface mesh that I need which I was not able to generate in ICEM and this is a great progress. I just need to generate the volume mesh to get it done. After generating the surface mesh for all the domains I selected all of the domains and assembled an unstructured block for them. PointWise shows that it is working but it seems that nothing happens and no block is generated. I also used create, assemble special to select the outer boundaries of the domain and then select the interior domains to create a block but there is no option to save the faces (it’s off). I don’t have enough experience in PointWise to figure out what the problem is so I ask for your help. I have attached some pictures and a link to the file.

Thanks in advance

[dgarlisch]

Please repost your NEW question as a top level post. Appending to a one year old post is considered bad etiquette.

See also Guide: How to ask a question on the forums

[Rajan Bhandari]

Dear all,
I could not create mesh for my 2d intake geometry with extrusion somewhere in the middle of the wall. I could not generate structured mesh. I tried to do by creating blocks as in Ansys ICEM but could not. I could not figure out how to create block in pointwise as in ICEM. Anyone can help me with this.

[adi.ptb]

Hi Rajan,

It would be better if you share your pointwise (.pwd) file and give us more details of what you are looking to achieve so that we can help you.