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CATIA V4 (Dassault) >> Pro/ENGINEER / Creo Elements

The following settings are recommended up to CATIA V4.2.5 (Dassault) and Pro/ENGINEER Wildfire 5.0 / Parametric 2.0.

CATIA V4 (Dassault) - System

  • No elements should be placed in NOSHOW/NOPICK.
  • Model should be cleaned of all unused information, because the translator exports the complete content of CATIA-parts. Delete:
  • Unused DETAILS (in all workspaces)
  • Unused elements from NOSHOW (in all workspaces)
  • Drawings
  • Update SOLID-M into SOLID-E with CATSOE utility.
  • Perform SOLIDE/UPDATE, also if message UPDATE ALREADY DONE appears. (Regeneration removes inconsistencies.)
  • Generate Volumes from SOLID-E and delete SOLID-E in all workspaces. (Geometry is still exported as a solid in STEP.)
  • Scaled and mirrored dittos (EXPLODE function) should not be used.
  • Before export elements of special CATIA modules (e.g. PIPING, BUILDING DESIGN) need to be converted to STEP conform elements.
  • Use CATCLN.
  • Assembly structures in SETs should be transferred to DETAILS.
  • Link all SETs if possible (SETS -> LINK).
  • Solids/Volumes consisting of separate Bodies should be avoided.
  • Objects used for Boolean operations should show good penetration.

STEP Preprocessor

  • Option "Use Short Names" should be deselected (unless appropriate libraries are available).
  • Recommended settings in Declaration File:
  • CATST1.STEP.USE_SHORT_ALIAS=FALSE
  • CATST1.STEP.EXPORT_NO_SHOW=FALSE
  • CATST1.STEP.EXPORT_UNUSED_DETAILS=FALSE

STEP File

  • The supported STEP file extension depends on the used Pro/ENGINEER version:
  • Pro/ENGINEER 2000i² and Pro/ENGINEER 2001: The STEP file extension must be *.stp, otherwise it has to be renamed.
  • Creo Elements: The STEP file extension can be either *.stp or *.step.
  • Pro/ENGINEER Wildfire: The STEP file extension can be either *.stp or *.step. If the extension is *.step an error message occurs: "Selected file is not of the selected type." but the file will be opened.
  • Only one dot in the STEP filename is allowed (wrong: file.name.stp; right: file_name.stp) for Pro/ENGINEER 2000i² and Pro/ENGINEER 2001 and special characters must be avoided in the filename syntax. Pro/ENGINEER Wildfire is not sensitive for more than one dot in a STEP filename. Special characters and white spaces in the STEP filename are not allowed in Pro/ENGINEER Wildfire.
  • For Pro/ENGINEER 2000i² and Pro/ENGINEER 2001 the filename including file extension should be no longer than 35 characters. For Pro/ENGINEER Wildfire the filename including file extension is limited to 39 characters.

Pro/ENGINEER / Creo Elements - STEP Postprocessor

  • Some STEP specific settings can be added to the configuration file config.pro:
  • With Tools -> Options... you can add the below mentioned settings in Pro/ENGINEER Wildfire.
  • With File -> Options -> Configuration Editor you can add the below mentioned settings in Creo Elements
  • With Utilities -> Options...  you can add the below mentioned settings in Pro/ENGINEER 2001.
  • With Utilities -> Preferences...  you can add the below mentioned settings in Pro/ENGINEER 2000i2.
  • Recommended config.pro options:
  • fix_boundaries_on_import yes
  • enable_absolute_accuracy yes
  • intf3d_in_close_open_boundaries yes
  • intf_in_blanked_entities yes
  • To import a part (does not work with assemblies) in Pro/ENGINEER 2001 with an accuracy other than the default accuracy, the following procedure is recommended:
  • Open a new part file
  • Change to desired accuracy ( Set Up -> Accuracy -> ...)
  • Import model with menu option Insert -> Data from File.
  • The parameter enable_absolute_accuracy in the config.pro needs to be set to yes if absolute accuracy is needed.
  • A recommended setting of the absolute accuracy is 0.01mm. If the part is not imported correctly, try again by changing the accuracy to 0.02mm and 0.05mm.
  • To import a part (does not work with assemblies) in Pro/ENGINEER 2000i² and Pro/ENGINEER Wildfire with an accuracy other than the default accuracy, the following procedure is recommended:
  • Open a new part file
  • Change to desired accuracy ( Edit -> Set Up -> Accuracy -> ...)
  • To import a part in Creo Parametric with an accuracy other than the default accuracy, the following procedure is recommended:
  • Open a new part file
  • Change to desired accuracy (File -> Prepare -> Model Properties -> ...)
  • Up to Wildfire 3 import model with menu option File -> Import -> Append to model.
  • In Wildfire 4 and higher choose File -> Open and select STEP as type.
  • The parameter enable_absolute_accuracy in the config.pro needs to be set to yes if absolute accuracy is needed.
  • A recommended setting of the absolute accuracy is 0.01mm. If the part is not imported correctly, try again by changing the accuracy to 0.02mm and 0.05mm.
  • If the STEP file contains assembly data, see to it that it is imported as an assembly (otherwise, Pro/ENGINEER gives a warning).
  • Depending on the further usage, hybrid models and multi solids can be imported in part or assembly mode. Part mode allows import with user defined accuracies, in assembly mode all solids/surface can be individually handled.

Pro/ENGINEER / Creo Elements - System

  • Shaded view is helpful for a first impression of the model quality.
  • Highlighted menu option Info -> Geom/Check gives hints about geometric problems of the imported model. In Creo Parametric a similar functionality can be found in File -> Prepare -> ModelCheck Geometry Check
  • The color of the model in wireframe display indicates its type (with Utilities -> Environment -> Colors turned off):
  • yellow for wireframe or surface boundary without connecting surface (might indicate bad areas)
  • If solid/shell cannot be created because of open gaps (look for yellow boundaries!), menu option Feature -> Redefine -> Fix Bndries -> Zip Gaps might help closing those gaps. (use Auto Select for quick help).
  • The Pro/ENGINEER 2001 and Wildfire Interface Guide gives more information.

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