与PROE的交换 IGES设置

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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.