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closed section error

kklinger
1-Newbie

closed section error

Forgive me if this is a simple question. When in sketcher and creating a
revolved part, for example, and you try to regenerate the sketch, it
gives the error that the "Section must be closed for this feature." But I
scan the sketch and it looks like all the lines are connected. How do you
determine where the sketch isn't closed? I thought that ProE would
highlight the points at the open section, but, of course it didn't. TIA.

Kirk Klinger

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1 ACCEPTED SOLUTION

Accepted Solutions
msmith
14-Alexandrite
(To:kklinger)

Creo Parametric 1.0 was enhanced to introduce Sketcher Inspection Tools to assist in such situations. With the Open Ends option turned on, any vertex that is not connected to another vertex will get highlighted with a red box. Clicking the Overlapping Geometry button will highlight sketch entities where there is overlapping geometry. See the image below and article CS182581.

 

msmith_0-1638799032302.png

 

View solution in original post

7 REPLIES 7

This can be frustrating. When I receive this error message with no
highlighted points I start a "seek and destroy" using the trim function. Go
around the entire sketch selecting adjacent elements with trim active and
you will generally find the problem. Not pretty or efficient but it usually
works for me.
Jim

It often puts a "dot" or some symbol in the location where it's open. It's
often too small depending on how far you are zoomed out. If you zoom in,
the screen repaints and the symbols go away.... 🙂 Same thing happens if
the error dialog box is covering your sketch. When you move it out of the
way, in my case, it "smears" the sketch (that sounds like a graphics card
or driver issue though both are "certified").

I will often use the "Trim entities..." command to *force* lines to
intersect together. There are other workarounds too, just depends on the
sketch.

Can you mail the sketch to the list ?? You can do a "Save" inside
Sketcher...

Regards
Hall






"Kirk Klinger" <->
Sent by: -
11/23/2004 09:05 AM
Please respond to "Kirk Klinger"

sip
1-Newbie
1-Newbie
(To:kklinger)

Other thing that has happened to me: double entities. Go around the sketch,
delete and undo delete the entities ione by one. When there are two
entities on top of each other, it seems to not delete it. That's the one
that's giving the trouble.
Sip

In my experience, I've seen that this can be caused by one of two situations:

1. there are two identical sketch entities on top of each other. To find, delete one entity, then repaint to see if there is another one underneath it. If not, undo and move on to the next entity.

2. The constraints and dimensions in the sketch are such that there are two endpoints that are on top of each other, but are not constrained to be "attached" to each other. To find, try modifying some dimensions to see how the sketch moves. Sometimes this will make a gap appear. Also, just looking at the constraints and dimensions. If something looks over constrained, there's your problem.

The second situation seems to be more common. I find that using the dynamic trim function is usually what causes it. While trimming, Pro/e seems to temporarily suspend all constraints, then tries to apply the constraints all at once when you leave the trim command, causing it to make incorrect assumptions.

To avoid the situation as much as possible, my advice is to keep your sketches simple.


Happy Modeling,
BPT

This is one area that could really use an enhancement. I've wasted a lot
of time over the years trying to find a hidden duplicate segment or a poor
intersection. If PRO was capable of better highlighting these areas I know
that would have a direct effect on my productivity.

www.ptc.com/appserver/cs/enhance_req_logger/EnhancementRequestLogger.jsp
msmith
14-Alexandrite
(To:kklinger)

Creo Parametric 1.0 was enhanced to introduce Sketcher Inspection Tools to assist in such situations. With the Open Ends option turned on, any vertex that is not connected to another vertex will get highlighted with a red box. Clicking the Overlapping Geometry button will highlight sketch entities where there is overlapping geometry. See the image below and article CS182581.

 

msmith_0-1638799032302.png

 

View solution in original post

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