CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > STAR-CCM+

Flow-aligned trimmed mesh of automotive injector's nozzle

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   September 13, 2013, 04:54
Default Flow-aligned trimmed mesh of automotive injector's nozzle
  #1
New Member
 
Join Date: Nov 2010
Posts: 16
Rep Power: 6
ecto is on a distinguished road
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!
Attached Images
File Type: png Iget.png (2.1 KB, 9 views)
File Type: png Iwouldlike.png (2.8 KB, 9 views)
ecto is offline   Reply With Quote

Old   September 13, 2013, 07:32
Default
  #2
New Member
 
Jimmy
Join Date: Apr 2011
Posts: 12
Rep Power: 6
Jimmy123 is on a distinguished road
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.
Jimmy123 is offline   Reply With Quote

Old   September 13, 2013, 09:54
Default
  #3
New Member
 
Join Date: Nov 2010
Posts: 16
Rep Power: 6
ecto is on a distinguished road
Quote:
Originally Posted by Jimmy123 View Post
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...
ecto is offline   Reply With Quote

Old   September 13, 2013, 18:12
Default
  #4
New Member
 
Jimmy
Join Date: Apr 2011
Posts: 12
Rep Power: 6
Jimmy123 is on a distinguished road
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)
Attached Images
File Type: jpg Directed Mesh 1.jpg (46.6 KB, 16 views)
File Type: jpg Directed Mesh 2.jpg (83.0 KB, 15 views)
File Type: jpg Directed Mesh 3.jpg (95.6 KB, 15 views)
File Type: jpg Directed Mesh 4.jpg (72.0 KB, 15 views)
Jimmy123 is offline   Reply With Quote

Old   September 16, 2013, 09:33
Default
  #5
New Member
 
Join Date: Nov 2010
Posts: 16
Rep Power: 6
ecto is on a distinguished road
Thanks Jimmy!!! That's a great guide! I appreciate it very very much. I'll try to do that.
ecto is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
Sonic flow for exhaust nozzle beanlee999 FLUENT 1 May 10, 2012 14:34
Surface aligned mesh rpasiok OpenFOAM Meshing & Mesh Conversion 6 January 7, 2008 06:55
Convergence moving mesh lr103476 OpenFOAM Running, Solving & CFD 30 November 19, 2007 15:09
Gambit problems Althea FLUENT 21 February 6, 2001 08:05


All times are GMT -4. The time now is 14:03.