When a part is exported out of Pro/E, make sure the following IGES settings are set. If the user changes any of these settings, they must reboot Pro/E. Making sure that the IGES file will read back into Pro/E is a great first test. Also have the Pro/E models checked for GEOMETRY ERRORS. If any exist, have them fixed!!!
IGES settings for Pro/E
iges_out_all_srfs_as 128
iges_out_spl_crvs_as_126 yes
iges_out_spl_srfs_as_128 yes
iges_out_trim_curve_deviation .001
iges_out_trim_xyz no
iges_out_trim_srfs_as_143 no
iges_out_mil_d_28000 no
iges_out_JAMAIS_compliant no
intf_out_blanked_entities no
intf3d_out_extend_surface no
IGES Settings for Pro/JR & PT/Modeler:
iges_out_all_srfs_as 128
iges_out_spl_crvs_as_126 yes
iges_out_mil_d_28000 no
PT/Modeler & JR did not allow a model to be checked for Geometry Check Errors last time I saw it.
When importing a Pro/E file into SolidWorks and it will not convert to a solid, try the following:
1) While in Pro/E, Check for GEOMETRY ERRORS. If any occur, they must be fixed! This means that they have a hole in their geometry.
2) Adjust the accuracy in Pro/E. PTC抯 default accuracy is .0012. Try courser accuracy and create a new IGES file.
If a SolidWorks file does not automatically convert into a solid in Pro/E, try the following:
From their (PTC) menuing structure, select;
Feature /Redefine / Sel By Menu / Last Feature (Select the imported SolidWorks model)
2) SELECT Fix Boundries THEN Zip
3) SELECT Attributes / Make Solid
This should convert the surfaces into a solid. If any problems or surfacing errors occur while importing a SolidWorks IGES Surface file into Pro/E, the corrupt surface(s) will display as a yellow colored entity.
If a SolidWorks file does not automatically convert into a solid in Pro/E, try the following:
From their (PTC Rev 18) menuing structure, select;
Feature / Redefine / Sel By Menu / Last Feature (Select the imported SolidWorks model)
Select "Fix Boundries" then "ZIP"
Select "Attributes / Make Solid"
This should do the job.
Any problems or surfacing errors with the import of a SolidWorks IGES file will display as a yellow colored entity in Pro/E.
I believe it is now possible to import cylindrical and conical IGES surfaces from Pro/E which may be assembled with the concentric mating constraint using build 97/341 or higher.
To make SolidWorks recognize cylindrical & conical surfaces as such, place the following into Pro/E's Config.pro:
iges_out_all_srfs_as 128
To use the edges of imported cylinders as arcs within SolidWorks' sketch environment, set Pro/E's Export Opts menu to WfrmSurfs upon exporting.