×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Updated Sketch

Updated Sketch

Updated Sketch

(OP)
I have updated a sketch but there seems to be a hole in the chain? Is there a analysis tool I can run quickly to find the gap instead of going through the sketch bit by bit?

RE: Updated Sketch

One way is to start the extrude command, change the curve selection rule to 'feature curves' and select your sketch; a large 'asterisk' type symbol should highlight any gaps in the chain of curves.

www.nxjournaling.com

RE: Updated Sketch

You appear to be running NX 10.0 but with the old interface style. Note that the clock is ticking...

But getting back to your issue; yes, there is a way to visually see if the profile has no gaps. Seeing if there are gaps is a bit trickier, but at least there is a way to spot where there MIGHT be problems.

When you're creating your sketch, as you're adding lines and arcs, the end points SHOULD snap together so that they are coincident. If they are there will be no gaps in the profile. However if the end points of the curves are merely one on top of the other but NOT constrained to be coincident then they may or may not be a gap. You can tell that curve end points are coincident or not by the size of the end-point symbol. A large 'dot', the ends are constrained coincident. A small 'dot', they are not constrained coincident. Now even if they are not constrained coincident, there may not be a gap, just that there is no guarantee that there isn't. The picture below shows you what I mean:



Now there is another way that works as well and might actually be a bit easier to use, particularly if the sketch is a bit complex. While in the sketch and with all the curves visible, go to the 'Show/Remove Constraints' function and when the dialog opens, make sure that the 'All In Active Sketch' is selected along with the 'Include' item. Now set the 'Constraint Type' to 'Coincident' and all of the 'Coincident' corners should highlight while the other corners will not.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources