Catia Export
Catia Export
(OP)
I have to export a Pro/E model to a format that can be opened in Catia. Can someone suggest the settings in Pro/E to be done and the format one should use / available in Pro/E for best data translation.
Is there any special Plugin or Software that is available and can be used either while exporting data from Pro/E or while importing data in Catia?
Promt response is appreciated.
Thanks
Amish
Is there any special Plugin or Software that is available and can be used either while exporting data from Pro/E or while importing data in Catia?
Promt response is appreciated.
Thanks
Amish





RE: Catia Export
-Hora
RE: Catia Export
Thanks a lot for the support.
Amish
RE: Catia Export
ATB bus is $$$$$$
My advice is to stay with STEP. IGES solid from Pro/E is too huge for Catia.
-Hora
RE: Catia Export
RE: Catia Export
My second concern was the quality of data. I have no experience of using Catia. But I expect that since ".model" is Catia's native format, the quality of data translated should be the best in comparison to STEP or IGES. Is this true?
My third concern was that when I open the ".model" file of a Pro/E assembly exported in Catia, I should have the complete structure of sub-assemblies and parts in Catia also. This problem is also solved since while exporting an assembly to ".model", Pro/E asks whether we want a FLAT or DITTOS File Structure. Choosing a Dittos file structure does this job.
Comments are welcome
Amish
RE: Catia Export
You have the ATB bus then. Try to export your assy in both formats (.model and STEP) and choose the one of them.
In the past I had some problems with the .model exported from Pro/E 2001.
Indeed, FLAT will convert your assy in a single part and DITTO will keep the assy structure.
Also, don't forget that a CATIA V4 assembly is a .session and not .model. But it's a madness to create a .session.
I export currently Pro/E files into CATIA V5 and I use STEP. This works fine for me.
Good luck,
-Hora.
RE: Catia Export
I also tried STEP route. Though I got open surfaces here also, but these are managable. Are there any settings in Pro/E that one should set for exporting to STEP format.
RE: Catia Export
The only settings in PROE for STEP is the format (203 or 214). 203 is default and I suggest you to keep it.
Rounds may give you problems. Try to identify the parts with open surfaces and then in PROE remove rounds. Sometimes, is easy to recreate them in CATIA than to loose an incredible amount of time trying to close surfaces.
Play also with part accuracy. This may cause failure in rounds features but can solve some problems.
Another suggestion is this one: Once you have your assy in CATIA, export it again in STEP from CATIA. Then import it again. Incredible, but this can solve a lot of problems, usualy open surfaces. I tell you this because I had such a problem, creating a .model from PROE. I export in in STEP, import in in CATIA V5, export in .model. I obtained a part a with opened surfaces. So before to export in in .model, I made a new STEP from CATIA V5, imported back and then export it in .model. Problem solved.
Good luck.
-Hora
RE: Catia Export
step_export_format ap203_is
intf3d_out_default_option solid
intf3d_out_extend_surface no
intf_in_blanked_entities NO
intf3d_in_include_items SRFS_CRVS_PNTS
iges_out_dwg_line_font yes
fix_catia_iges_sym_note yes
I hope that this helps.
Nate
RE: Catia Export
A .model is considered a V4 file. Therefore, make sure you use MigrateV4ToV5 Utility when trying to open with V5. Do not use File > Open. Oh yeah, make sure you hv min P2 configuration. Batch util will not run on P1.
Peter