CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   STAR-CCM+ (http://www.cfd-online.com/Forums/star-ccm/)
-   -   Flow-aligned trimmed mesh of automotive injector's nozzle (http://www.cfd-online.com/Forums/star-ccm/123454-flow-aligned-trimmed-mesh-automotive-injectors-nozzle.html)

ecto September 13, 2013 04:54

Flow-aligned trimmed mesh of automotive injector's nozzle
 
2 Attachment(s)
Hi everybody!

I have a big question: I'd like to construct a flow-aligned trimmed mesh in a nozzle of an injector. I had no problems in doing the same in the holes of the injector.
I tried so many times, but it seems that trim doesn't accept a reference system different from a Cartesian one. I have only one region, and I noticed no advantages in having different regions or using per region meshing. I use also prism layer mesher with many layers at the walls because I do a low y+ calculation.
I attached two images to try to explain. Imagine that these are half sections of the nozzle. The flow of gasoline in the nozzle goes through the hollow space between two overlapping cups.
I use Starccm+ 8.04.

Thanks!

Jimmy123 September 13, 2013 07:32

I don't think you can get an aligned mesh it like that with a trimmed mesh no matter where you put the alignment location.
Maybe it can get a little better by using more prism layers/advancing mesh. But I think that the best result will be achieved with a directed mesh.

ecto September 13, 2013 09:54

Quote:

Originally Posted by Jimmy123 (Post 451514)
I don't think you can get an aligned mesh it like that with a trimmed mesh no matter where you put the alignment location.
Maybe it can get a little better by using more prism layers/advancing mesh. But I think that the best result will be achieved with a directed mesh.

Hi Jimmy123! Thanks for the answer!
Oh yes, I just discovered directed meshing, because I come from Starccm+ 7.02.
Do you think I can really obtain a flow oriented mesh, with a lot of prism layers at the wall, with this?
Could you please explain me briefly which are the steps to do in order to mesh with directed meshing?
I think I have to prepare my start surface mesh.

I also read under

Preparing CAD Parts for Directed Meshing


"Each part must have a regular section profile along its length. There cannot be any features intruding into the sweep path between the source and target surfaces. For example, shapes such as Y-junctions cannot be meshed without being split into two mirrored parts."

I don't understand what "regular" does mean...

Jimmy123 September 13, 2013 18:12

4 Attachment(s)
I think it can get better by using prisms, but not as good as a directed mesh.

By regular, I think you can think of it as a clean path. It can’t be divided into two channels or so, and there can’t be any shapes that block the way.

I made a small guide and I also attached some images with pasted print screens. I hope it can help you :)

1. Create a part.
2: Add the part to a region. (so that you later can create the volume mesh)
3: Right click the part, Create mesh operation->Directed mesh
4: Choose a surface to use as source mesh and a corresponding surface to use as target. (Figure 1)
5: Right click on the boundary you choose as source mesh again. This time choose New Source Mesh-> Patch mesh. Then patch the topology. All lines should become green. (Figure 2)
6: After you have done that, change mode to “patch mesh”. Click on the lines and choose how many times they should be divided. All of the lines have to get numbers before you see a mesh. (Figure 3)
7: Close that window, add a New Volume Distribution. Choose how many layers there should be, and then generate the volume mesh (Figure 4)

ecto September 16, 2013 09:33

Thanks Jimmy!!! That's a great guide! I appreciate it very very much. I'll try to do that.


All times are GMT -4. The time now is 14:28.