CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   [ICEM] Create geometry (iges or step file) from fluent mesh (

muketa September 24, 2010 04:05

Create geometry (iges or step file) from fluent mesh
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 September 27, 2010 04:33

Any suggestion??

sac September 27, 2010 07:16

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 October 5, 2010 18:53

I totally agree with SAC. Good post.

arapha October 12, 2010 09:43


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 !!

PSYMN October 15, 2010 11:40

ICEM CFD Output Tab.
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 July 26, 2013 07:59

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.

Jan Smedseng July 26, 2013 12:51

Export Geometry in ICEM CFD

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.


Jan Smedseng
CFX Berlin Software GmbH

jose_zola August 4, 2015 05:06

export geometry from fluent
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?

Jan Smedseng August 4, 2015 09:56

Separating grid

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.


jose_zola August 5, 2015 05:38

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

All times are GMT -4. The time now is 13:53.