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

[ICEM] Create geometry (iges or step file) from fluent mesh

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

Like Tree4Likes
  • 3 Post By sac
  • 1 Post By PSYMN

Reply
 
LinkBack Thread Tools Display Modes
Old   September 24, 2010, 04:05
Question Create geometry (iges or step file) from fluent mesh
  #1
New Member
 
Join Date: Jul 2009
Posts: 5
Rep Power: 8
muketa is on a distinguished road
Hi everybody,
having a Fluent mesh (file .msh) is it possible to open that mesh in ICEM to reconstruct the geometry and export that geometry in a IGES or STEP file? I've just tried the Mesh-->Facets command, but then I'm not able to export facetted geometry to IGES file...

Is there any method to recreate geometry (in a neutral format like iges so that i can read that geometry in a CAD software) from Fluent mesh?

I would appreciate any help. Thank you for your attention.

MUKETA
muketa is offline   Reply With Quote

Old   September 27, 2010, 04:33
Default
  #2
New Member
 
Join Date: Jul 2009
Posts: 5
Rep Power: 8
muketa is on a distinguished road
Any suggestion??
muketa is offline   Reply With Quote

Old   September 27, 2010, 07:16
Default
  #3
sac
Member
 
Join Date: Jun 2010
Posts: 44
Rep Power: 8
sac is on a distinguished road
In workbench take the part into FEModeler and set the cut angle to 0 then skin the geometry. This will create a surface for every facet.

Use the create parasolid command to create a parasolid from this and then use the sew tool to sew it together (you may need to play with the sewing tolerance to get this to work).

From this you can then export the parasolid.

Other programs - such as Rhino can do exactly the same type of operation. Also there is a macro for Mechanical APDL that does pretty much the same thing from IDAC's website.
PSYMN, hityangsir and FJSJ like this.
sac is offline   Reply With Quote

Old   October 5, 2010, 18:53
Default
  #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
I totally agree with SAC. Good post.
PSYMN is offline   Reply With Quote

Old   October 12, 2010, 09:43
Default
  #5
New Member
 
Join Date: Oct 2010
Posts: 19
Rep Power: 6
arapha is on a distinguished road
hey,

I am trying to convert a .cgns file created in Pointwise to a .msh file for use in another in-house CFD code. Is there a way for me to create a .msh file directly in Pointwise, or a way to convert the exported .cgns file to a .msh file through FLuent or another software ?
Thanks !!
arapha is offline   Reply With Quote

Old   October 15, 2010, 11:40
Default ICEM CFD Output Tab.
  #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
ICEM CFD can do it thru the output tab. You may also be able to do it in Fluent or Pointwise... You may also be able to find converters on line.
PSYMN is offline   Reply With Quote

Old   July 26, 2013, 07:59
Default
  #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
I was privately asked for more details here, and specifically, if we could convert a mesh to IGES or STEP in ICEM CFD...

Converting mesh to facets is not the way. That is a good way to get towards an STL file (a faceted data format), but you could more easily export the mesh as STL. Instead, we use that conversion when we want to convert a mesh to a geometry so we can generate a new mesh from an old one. I like using the mesh editing tools to fix up STL files and then turn them back into STL files before I mesh them.

IGES and STEP need nurb/bspline surfaces. These are not faceted formats, instead, each surface has i and j data. It just so happens that our hexa blocking faces do have what is needed, so it is possible to convert via Edit => Structured Mesh to CAD faces. Then you would use File => Export Geometry...

I have seen users do this to create a coarse hexa blocking shrinkwrap around engine parts and then export them... But ICEM CFD is a meshing tool, it was not designed as a geometry prep tool so not much effort has been put into the File => Export Geometry and that step tends to be the weak link.

Other tools (Such as FEModeler or Rhino, as some have already mentioned on this thread) do a much better job. FEModeler is a free module in ANSYS Workbench, which comes free with ICEMCFD.
hityangsir likes this.
__________________
-----------------------------------------
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, 2013, 12:51
Thumbs up Export Geometry in ICEM CFD
  #8
New Member
 
Jan Smedseng
Join Date: Jul 2013
Posts: 9
Rep Power: 4
Jan Smedseng is on a distinguished road
Hi.

Try this:
- Import the fluent mesh in ICEM CFD.
- Edit mesh >> Delete elements >> All volume elements
- Save the project
- File >> Export mesh >> Write STL file.

Now you have the STL file of the geometry.
You can import this STL file to the ANSYS DesignModeler (you have to change the postfix filter to |all files (*.*)|) or to ANSYS SpaceClaim.

You're now able to fix the geometry, add missing faces, merge faces...

You also have the possibility to export the geometry in different formats.

Regards,
Jan



-----------------------------------
Jan Smedseng
CFX Berlin Software GmbH
Jan Smedseng is offline   Reply With Quote

Old   August 4, 2015, 05:06
Exclamation export geometry from fluent
  #9
New Member
 
frety
Join Date: Jul 2015
Posts: 7
Rep Power: 2
Samer_Wakim is on a distinguished road
hii all,
Please i need i little help here. i wrote a udf to change the porosity inside a volume in order to get some sort of a flow inside tubes. Now after i interpret the function a need to export the new volume( with the new porosity distribution) to be able to print it 3d. please any ideas?
Samer_Wakim is offline   Reply With Quote

Old   August 4, 2015, 09:56
Default Separating grid
  #10
New Member
 
Jan Smedseng
Join Date: Jul 2013
Posts: 9
Rep Power: 4
Jan Smedseng is on a distinguished road
Hi.

Thats not so hard. In ANSYS Fluent you can define a region by an Isovolume. Just select "Adapt >> Isovalue".
In the next step, you can separate the mesh by this new region. Just select "Mesh >> Separate >> Cell"

Now you have two possibilities. You can write a case file and import it to ICEM CFD or you can switch to fluent meshing an export an msh file there.

The rest is as described in the post above.

Regards,
Jan
Jan Smedseng is offline   Reply With Quote

Old   August 5, 2015, 05:38
Thumbs up
  #11
New Member
 
frety
Join Date: Jul 2015
Posts: 7
Rep Power: 2
Samer_Wakim is on a distinguished road
thank you so much for your reply. you help me a lot. one more question what value should i use for the iso value(velocity, pressure.. ) i tried to limit the velocity but it seems that isnt working
Samer_Wakim is offline   Reply With Quote

Reply

Tags
fluent mesh, geometry, iges

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
1.7.x Environment Variables on Linux 10.04 rasma OpenFOAM Installation 9 July 30, 2010 04:43
OpenFOAM Install Script ljsh OpenFOAM Installation 82 October 12, 2009 11:47
DxFoam reader update hjasak OpenFOAM Post-Processing 69 April 24, 2008 01:24
DecomposePar links against liblamso0 with OpenMPI jens_klostermann OpenFOAM Bugs 11 June 28, 2007 17:51
convert FLUENT mesh file to CFX mesh file?? frederic felten FLUENT 5 December 6, 1999 10:32


All times are GMT -4. The time now is 04:24.