CFD Online URL
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[ICEM] ICEM 12.1 - car meshing

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 23, 2011, 17:12
Default ICEM 12.1 - car meshing
  #1
New Member
 
Tiago Portolon
Join Date: May 2011
Location: Brazil
Posts: 11
Rep Power: 5
T_Portolon is on a distinguished road
Hi everyone,

I'm facing a little trouble in surface meshing with ICEM 12.1. Using the mesh type "all tri" and mesh method "patch dependent", I have had as result, that the boundaries of the surface are meshed with quad elements, instead of triangular elements. How can I solve this problem?

Thanks in advance

T_Portolon
T_Portolon is offline   Reply With Quote

Old   July 25, 2011, 00:21
Default Width...
  #2
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
You have set a "width" setting on your curves.

This is typically used for FEA to create "washers". They would combine this with a bolt spider to stiffen those regions.

Go back and set the width on the curves to zero... If you are setting the sizes on the parts and want to set a width to the surfaces but not the curves, that can be done (look for the checkbox option on the Params by Parts pop up)...

Simon
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   July 25, 2011, 19:30
Default Curve & surface meshing (and one more question)
  #3
New Member
 
Tiago Portolon
Join Date: May 2011
Location: Brazil
Posts: 11
Rep Power: 5
T_Portolon is on a distinguished road
Simon,

Thanks for the help! Actually, I'm following these steps to obtain a surface mesh:
1. mesh the curves (width may vary, depending on the location)
2. mesh the surfaces (applying size in the mesh, different from Gambit)
It usually works, but with the tetra elements on the boundaries.

I didn't mesh the volume, yet. It's because when I try to run the volume meshing, the program goes wrong, creating something around 14 million elements, and gets stuck. What am I doing wrong?

Thanks again

Tiago
T_Portolon is offline   Reply With Quote

Old   July 26, 2011, 15:06
Default paradigm shift
  #4
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Skip the first step...

Just set sizes on your geometry (curves are required, surfaces are bonus) and go straight to meshing the surfaces with patch conforming...

Alternatively, you could also just skip right to volume meshing with the Octree Tetra... It has many advantages and is probably the easiest way to go.

Try a couple tutorials to help transition you from a Gambit mind set to an ICEM CFD mind set... If you keep thinking with the Gambit paradigm, you will miss most of the ICEM CFD advantages.

If tutorials are too much work, at least take a look at some movies on youtube or the customer portal. Here is one about skipping right to volume mesh...

http://www.youtube.com/ansysinc#p/u/29/SdUjpjwUnew

Have fun with it.

Simon
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   July 26, 2011, 20:57
Default Direct volume meshing
  #5
New Member
 
Tiago Portolon
Join Date: May 2011
Location: Brazil
Posts: 11
Rep Power: 5
T_Portolon is on a distinguished road
Simon,

I made the mesh as you said, and it was ok.
Now, I gonna try to use a density around the model, to refine the mesh a little bit.
I used to work with ICEM as I did it with Gambit (meshing edges, faces and volumes, in this order).

Thanks again!

Tiago
T_Portolon is offline   Reply With Quote

Old   August 18, 2011, 17:39
Default Delaunay for tetras
  #6
New Member
 
Tiago Portolon
Join Date: May 2011
Location: Brazil
Posts: 11
Rep Power: 5
T_Portolon is on a distinguished road
Hi Simon,

I made some volume meshes with octree, and it was ok. Now I'm trying to use Delaunay, to reduce the number of cells (around 3-4 million). I tried to use densities around the car body, but the final mesh reached 9 million of cells.

Using Delaunay, the problem is the volume mesh is created around the volume (wind tunnel) that I want to mesh.


Do you know how can I fix this?

Thanks

Tiago
Attached Images
File Type: jpg ScreenShot011.jpg (41.3 KB, 80 views)
T_Portolon is offline   Reply With Quote

Old   August 21, 2011, 00:54
Default
  #7
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Was your tunnel surface meshed?

I would suggest starting with your Octree mesh... Then delete the volume mesh, smooth the heck out of the rest with Laplace turned on... Then smooth once more without Laplace, then run delaunay from that.

It will keep your surface mesh, make it nicer and then fill in the volume with delaunay.

Best regards,

Simon
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   August 22, 2011, 18:53
Default
  #8
New Member
 
Tiago Portolon
Join Date: May 2011
Location: Brazil
Posts: 11
Rep Power: 5
T_Portolon is on a distinguished road
Simon,

The surfaces were meshed before delaunay volume meshing. For first, I selected "mesh internal domains", and meshed the volume. I think I had a problem with the geometry. Then, I saved it in parasolid format, and repaired with SolidWorks resources.

And so, I meshed the volume following your recommendations, and it was right again.

Thanks

Tiago
T_Portolon is offline   Reply With Quote

Old   August 29, 2011, 21:31
Default Case and data transfering
  #9
New Member
 
Tiago Portolon
Join Date: May 2011
Location: Brazil
Posts: 11
Rep Power: 5
T_Portolon is on a distinguished road
Hi Simon

Thanks for helping with ICEM. Do you work with Fluent? I've been using a
8-processor machine to run the simulations. When I try to open those files in my machine (4-processor), it doesn't work.

Thanks in advance


Tiago
T_Portolon is offline   Reply With Quote

Old   September 1, 2011, 23:57
Default
  #10
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
I don't know what the problem is, but it doesn't matter that one machine had 8 cpus and the other had 4...
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   February 7, 2012, 05:08
Default
  #11
Member
 
Join Date: Jun 2011
Posts: 59
Rep Power: 5
maalan is on a distinguished road
Hi, Simon!! I am facing a 3D hexa mesh of a car with ICEM CFD by using the o-grid. I find it such tool very useful and I am getting very good results. My car model is within a wind tunnel and separated 50 cm from the ground so I am having trouble in meshing the zone under the car.

I find it your help in this forum very useful!!
Thanks in advance!
maalan 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] complex 2D meshing on ICEM kassab ANSYS Meshing & Geometry 26 April 14, 2014 22:02
[ANSYS Meshing] Hybrid meshing ICEM djoul ANSYS Meshing & Geometry 2 January 17, 2012 19:18
Wind tunnel hexa meshing in ICEM CFD 12.1 matheusguzella ANSYS Meshing & Geometry 1 March 14, 2011 18:14
[ICEM] ICEM meshing problem xyq102296 ANSYS Meshing & Geometry 6 October 28, 2010 11:09
Missing tets along line when meshing with ICEM CFD Georges P. Côté CFX 6 March 23, 2006 01:34


All times are GMT -4. The time now is 22:47.