extracting 2d geom in Pro Detail

ProE 2001
Win2K
I have a drawing that includes many models and assemblies. It has one view
for each model/assembly with a few dimensions per view. Correct me if I'm
wrong, but when I open the drawing, all models and assemblies are loaded
into memory.
I would like to convert the parametric drawing views to 2d (to scale), but
still be able to add dimensions, translate/copy/delete/modify the line work.
Basically, I'd like any user to open the drawing & add dimensions without
having access to the 3d models. The final 2d geometry will not be
associative. Ideally, I'd like to be able to create a view (or open an
existing drawing), extract/convert the views line work to 2d, then place the
view it in a new drawing (unassociative).
Even if the answer is "copy/paste" this is not an option because in our
release of 2001 it "crashes" ProE. I believe the "use edge" option is
parametric to this doesn't seem to be the solution.
Any advice?
Thanks in advance,
Scott
Reply to
Scott
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Scott,
Pro/DETAIL has the functionality that you're looking for. It's called 'Snapshot'. You can choose individual views to 'Snapshot' or 'All Views' to convert all of the 2-D drawing's views to non-associative, 2-D, draft entities. It works really well, but there are a few things that you should probably be aware of:
1) Cross-section cutting plane lines and their corresponding arrowheads will get their appearances changed. Not for the good, by the way.
2) You can create new dimensions that reference the remaining 2-D draft entities. Their values will be based upon a 1:1 'Draft Scale'. *NOTE: There is a drawing setup file option called 'draft_scale' that can be modified to reflect the scale that you would like for any new dimensions' values to be based upon. Also, with Pro/LEGACY activated while working in a drawing that has had all of its views snapshotted, you will be able to assign individual view scales to any view that you would like. The Pro/LEGACY module allows the user to work in the same manner in which they would with other strictly 2-D CAD applications. The functionality may not be as powerful as traditional 2-D systems such as AutoCAD, Microstation, CADRA, CADAM, etc., but it will suffice. I can assure you of it. I've tested Pro/LEGACY and Pro/DETAIL out very thoroughly and it works just fine once you understand its behaviors.
To get view geometry *minus* dimensions over to another 2-D drawing, you'll have to create a Symbol of it in the source drawing. Then place it as a Symbol instance in the target drawing. And you'll have to 'Explode' the Symbol in the target drawing in order to be able to work with it. You will need to re-dimension this geometry in the target drawing. That is the one limitation that is rather significant for most users. Other than this limitation, the combination of Pro/DETAIL and Pro/LEGACY is functional for non-associative, 2-D CAD work. Of course the menu structure is a bit dissheveled, but that's the nature of most things PTC. :-)
S.T.
Reply to
S.T.
Some additional info for you Scott. Release 2001's Snapshot functionality can be found under: Views-Modify View-Snapshot-Pick View/All Views
In Pro/E Wildfire, as David Janes pointed out already, the Snapshot functionality can be accessed under: Edit-Convert to Draft Entities
With Wildfire, you pre-select the view(s) and then choose Edit-Convert to Draft Entities to Snapshot them; which converts the associative view geometry to non-associative draft entities.
Best regards,
S.T.
Reply to
S.T.

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