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c.strohhacker1-Visitor
1-Visitor
May 11, 2011
Question

Problem creating cross-section view in a drawing

  • May 11, 2011
  • 4 replies
  • 5083 views

I’m having a problem creating a cross-section in a drawing view for a large assembly, reducing the parts (rep them out) eventually creates of the section; unfortunately that’s not a viable option. I am able to create the cross-section in the model window, however when I try to add the section to the drawing I get the error in the dash board...


"Cross-section creation in view "new_view_4", on sheet 1, aborted."


It looks like a memory issue; I.E. ProE runs out of capacity, not the computer. The system is Win7 Dell 5500, 12 gigs of ram, Quadro 5000, WF3. Are there any option which deal with this, or does anyone have a work around? Does WF4 offer better handling for drawing section views?



Thanks,


Chris.


4 replies

M
mkelley1-Visitor
1-Visitor
May 11, 2011

Coincidentally, I *just* encountered this same error this afternoon!


This is typically caused by accuracy problems - by default Pro/E uses relative accuracy set to .0012


A better value is .0001, in my experience...


This setting is often propogated thru start parts which inherit the (bad) default setting 😞


(And - better yet, use Absolute Accuracy in your start model. The problem with this is your part database size will typically get larger, and you must set it to different values for different parts. Both are small prices to pay, IMO.)


I solved my issue by isolating the part which had the issue using simplified reps. Simply (yuk yuk!) remove parts one-by-one from the Simp. Rep used to create the drawing section view & regen the drawing view until you find the offending member...


Sure enough, it had Relative Accuracy=.0012 (just as Karnak predicted)

D
dgschaefer21-Topaz II
21-Topaz II
May 12, 2011
This has to do with how relative and absolute accuracies are
implemented.



Relative accuracy defines a ratio of largest part edge or dimension to
the smallest allowable edge for new features.



Absolute accuracy directly sets the smallest allowable edge.



Relative has been the default in Pro/E since I've used it. The thinking
was, I believe, for very large parts, you could not manufacture small
details, nor would you want to. However, with long extrusion lengths or
large injection molded parts, that is simply not true. Also, as you've
seen, it can inhibit cross section creation if that section creates
small edges.



I think in WF4 or Wf5 the default changed to absolute, but most folks
build from a start part created years ago, so new parts will take their
accuracy from it.



I've used nothing but absolute accuracy, set to 0.0001", for the last 15
years with great success. When I have trouble creating features that
should be easy, I check and it's frequently that the accuracy has been
set to relative.



Doug Schaefer
W
wnicsir1-Visitor
1-Visitor
April 23, 2018

If you couldn't afford to change the accuracy for whatever reason, just try creating a new drawing view and a new section feature. I don't know why it worked, but maybe the view or the section lost some references. It might or might not work, I guess it depends on the situation.

T
TomD.inPDX17-Peridot
17-Peridot
April 23, 2018

I work with things that leave pointy features (cone) right at the section.

99.9% of the time they section fine on the drawing. 

But when you run into the 0.1%, heroic measures are required.

This has been an issue since the dawn of time on these particular assemblies. 

The problem still exists today (Creo 2.0) regardless of how many tip and tricks you apply.

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