I was "upgraded" from 4.0 to 22.214.171.124 one week ago and have run into an issue with creating drafts. PTC has added several features to the draft function to deal with rounds and chamfers. Now it does not work as expected. I created a square pocket, put chamfers in 2 corners and want to draft all sides independently. The default setting interprets the chamfer as seen in the left pocket. The right pocket was created by drawing the chamfers in the pocket sketch and drafts as expected.
When I uncheck "Create round/chamfer geometry" the chamfers disappear as shown in second image.
Is there anything I am missing or is this a BUG in Creo 7.0?
This is the description from Creo 7 (incomplete) help files.
Create round/chamfer geometry check box—For geometry that was attached with rounds or chamfers, recreates rounds or chamfers after attaching the drafted geometry.
In Creo 5-6 there was a documented limitation that the rounds/chamfers had to be recognized by flexible modeling functionality. If these limitations are still relevant it may explain the behavior you observed.
• This enhancement enables the handling of rounds and chamfers based on previously available capabilities in Draft. It does not extend the general capabilities of the draft feature, such as to draft previously drafted surfaces.
• This enhancement only supports round and chamfer types that are currently supported within Creo Parametric Flexible Modeling.
You can test this by exporting your model with draft/chamfers and then importing it and using this enhanced draft function. If it recognizes and retains the chamfers when altering the draft then that would suggest that your native chamfers may not be recognized by the flexible modeling engine.
Config options relevant to this.
• draft_tan_propagation_default—Determines if draft is automatically propagated along tangent surfaces. Values are yes or no. The default is yes.
• draft_preserve_inlying_rounds—Determines if inlying round and chamfer surfaces are preserved and not to be drafted. Values are yes or no. The default is no.
======================================== Involute Development, LLC Consulting Engineers Specialists in Creo Parametric