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OneSpace Designer >> Pro/ENGINEER / Creo Elements

The following settings are recommended up to CoCreate Modeling 16.5 and Pro/ENGINEER Wildfire 5.0 / Creo Parametric 3.0.

OneSpace Designer – System

  • Components of an assembly should have names no longer than 16 characters.
  • System accuracy should be set prior to modelling.
  • Recommended values are 10-6 mm, 10-5 mm, 10-4 mm.
  • The smallest extent value (e.g. edge length) can be set under:
  • SystemSetting ->Advisor/Check Setting -> min Edge
  • All Advisor Checks (voids, nonmanifold, knife edge, min edge) should be active while modeling the part.
  • Complete body checks should be done frequently during design and prior to export to STEP.

OneSpace Designer - STEP Preprocessor

  • When invoking the STEP export choose as option target system e.g. (CATIA IBM) or CATIA (debis) or Pro/ENGINEER.
  • If, in case of an assembly export, the option Assemblystructur/Shared Parts is set ON, individual colors of instances cannot be exported.
  • If the target system cannot process assembly structure information or geometric transformation, then you should select NO to suppress this information.
  • Hybrid models must be exported with multiple products. You can also use the Structure Browser to make your selection. If you try to specify a part by clicking in a viewpart, you will select only faces or edges instead of the whole part.

STEP File

  • An adjustment of the STEP file is not necessary.

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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