CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

varying curve mesh spacing at icem surface-mesh?

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

Like Tree2Likes
  • 1 Post By rwryne
  • 1 Post By PSYMN

Reply
 
LinkBack Thread Tools Display Modes
Old   January 13, 2010, 14:45
Default varying curve mesh spacing at icem surface-mesh?
  #1
New Member
 
Mirko Restemeier
Join Date: Jan 2010
Posts: 3
Rep Power: 7
mirko_r is on a distinguished road
Hello ICEM users,

I have a question concerning the generation of surface meshes.

If there are some parts A with very dense meshes (e.g. small surface mesh size)
next to curves of parts B with large surface mesh sizes there is no option available
to tell the mesher to adjust the curve-mesh-size of part B only in these regions
near A.

Maybe the attached picture is more explanatory than this text.

There are 2 possibilities I can imagine but both of them are not very practical:

1) One could set the curve mesh size on the whole outer diameter curve to the
small spacing of the inner parts an then Adapt the interior of the outer part to a
larger size which is still increasing the overall size dramatically.

2) Or one could set a custom spacing distribution for the outer curve with densities
in the regions near the inner parts which would be difficult to keep similar for all of
these problem regions.

It would be much easier if one could tell the mesher to adapt curve mesh sizes to
the needs of the surface mesh (for example to satisfy surface tetra growth ratio).

Maybe I miss a parameter which is doing that or maybe I could do it later after
the surface mesh generation by partial refinement?

Any hint on this topic would be very much appreciated.

Cheers,
Mirko
Attached Images
File Type: jpg Surface-Mesh.jpg (84.4 KB, 163 views)
mirko_r is offline   Reply With Quote

Old   January 13, 2010, 15:03
Default
  #2
Super Moderator
 
Ryne Whitehill
Join Date: Aug 2009
Posts: 313
Rep Power: 10
rwryne is on a distinguished road
If I understand your question right, I think the option you are looking for is the tetra size ratio and the tetra width options within the Part Mesh Setup window.

Try setting Part A's tetra width to a value of 2 or 3 (2 or 3 layers of growth) and its tetra size ratio 1.2-1.5 (the grow ratio)
Seb-Seven likes this.
rwryne is offline   Reply With Quote

Old   January 14, 2010, 07:52
Default
  #3
New Member
 
Mirko Restemeier
Join Date: Jan 2010
Posts: 3
Rep Power: 7
mirko_r is on a distinguished road
Hello rwryne
thanks for the fast reply.

Unfortunately your hint did not work out on this problem.
I set "tetra size ratio" and the "tetra width" before and that had no effect.

For better understanding of the Problem I attached another picture of the resulting
curve mesh which is used unchanged to calculate the surface mesh. You can see
there is insufficient space between the curve with the large spacing and the one
with small spacing.

For a good surface mesh the curve mesh has to be adjusted on the curve with the
large spacing (because increasing spacing on the other one is not feasible)

I hope I expressed myself more clearly now.

Regards,
Mirko
Attached Images
File Type: jpg CurveMesh.jpg (40.0 KB, 79 views)
mirko_r is offline   Reply With Quote

Old   January 14, 2010, 10:13
Default Patch dependent vs patch independent.
  #4
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
You are using the patch dependent mesher.

This mesher uses the curve sizes explicitly as set. This is more commonly appreciated by FEA users. You can bias the sizes, etc. but it is a bit awkward to size one curve based on a near by curve, especially in this situation.

The ANSYS Meshing tool does this much better by using a Gambit like sizing function that works at the surface level to set the curve sizes while taking the nearby curves into account. If you have ICEM CFD Tetra, your license will allow you to try out ANSYS Meshing (versions 12.0 or 12.1.)

Meanwhile, in ICEM CFD, If you instead switched to the patch independent mesher (OCTREE) you would be able to use the sizing function in ICEM CFD, along with the Tetra size ratio, etc. to better create a CFD mesh that would transition between these very different sizes in near proximity. This is what Ryryne is using.
PSYMN is offline   Reply With Quote

Old   January 14, 2010, 13:41
Default
  #5
New Member
 
Mirko Restemeier
Join Date: Jan 2010
Posts: 3
Rep Power: 7
mirko_r is on a distinguished road
Yes I'm using the patch dependent mesher because I dont like the stairsteps in
meshdensity created by octree so much.

What you just said is what i expected so I will maybe try it with ansys meshing.
But what about prism layers then? I never used the ansys grid generation before.

If I find a good solution I'll post it here.

Cheers,
Mirko
mirko_r is offline   Reply With Quote

Old   January 14, 2010, 14:21
Default Replace the Octree volume mesh with a delaunay fill...
  #6
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
What you may not realize is that behind the scenes, Gambit always did an Octree (Cartesian subdivisions with one block subdivided into 8 = Octree), but Gambit would just use this for the background grid and give you a Delaunay tetra mesh as a final result.

You can get the same thing with ICEM CFD… You could even setup your defaults to get it with one step.

The normal two step way is to compute Octree Tetra, then delete the volume mesh (use Edit mesh => Delete elements => and use the last icon in the tool bar to select all the volume elements). Then smooth with Laplace to get the best transitions. If you want you can do all sorts of surface mesh editing in here to get just what you want. Then use Tetra => Delaunay to generate a nice new tetra mesh. You could even use the TGLib option with AF, this is TGrid tech, the decendent of what you had in Gambit. Then smooth the Tetra mesh at the end, run your checks, etc...

To do the mesh generation all in one step, you must first go to the global settings and set the surface mesh method to Patch independent as a default. Then when you go to compute mesh you can go directly to Delaunay. It will realize that it doesn’t have a surface mesh and use the default surface mesh method to generate the Octree surface mesh with your sizing function and then automatically fill with Delaunay. You could also check the options to get Prism and Hexa core out of the same click.


The reason people often do the two step way is they may have a complicated model and want to edit the surface mesh before growing the volume mesh... The two step process offers flexibility.


But trying ANSYS Meshing may also be fun
shereez234 likes this.
PSYMN is offline   Reply With Quote

Old   January 14, 2010, 14:23
Default clarification...
  #7
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
One clarification, Gambit did its octree process only when the sizing function was used...

You can get a hint of this if you use the tool to visualize the sizing function.
PSYMN 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
[ICEM] Hexa mesh, curve mesh setup, bunching law Anorky ANSYS Meshing & Geometry 4 November 12, 2014 01:27
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
[ICEM] Unstructure Meshing Around Imported Plot3D Structured Mesh ICEM kawamatt2 ANSYS Meshing & Geometry 17 December 20, 2011 12:45
external flow with snappyHexMesh chelvistero OpenFOAM 11 January 15, 2010 20:43
problem when converting mesh (made by ICEM) using fluentMeshToFoam Forrest_Lei OpenFOAM 11 October 16, 2009 06:28


All times are GMT -4. The time now is 22:22.