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Sketch preferences / behavior

Valued Contributor
Valued Contributor

Are there any indicators that can be set so that I will know if there are gaps (not closed) between sketched lines that are supposed to interesect or if there are double lines on top of each other?  I'm working on a sketch for creating a feature in a part and am having trouble getting the sketch usable for an extrude.  I'm getting a message that the sketch can't be used for an extrude, so I'm going into the sketch and checking every line and intersection to see what the problem is.  I'm also used to using another CAD software and when a sketch was completely closed with no gaps, the whole sketch would turn shaded.  That would be very helpful now.  Is there a similar option in NX?  Thanks

3 REPLIES

Re: Sketch preferences / behavior

Siemens Phenom Siemens Phenom
Siemens Phenom

Hi @s_hightower,

When there are any gaps between the curves of a sketch then extrude result will be sheet, not the solid. The gaps will be highlighted with the asterisk symbol upon curve selection.

ex1.PNG

For the overlapping or intersecting curves, use the 'Stop at Intersection' or 'Region Boundary Curves' selection filter as shown.

ext.gif

 

Regards,
Ganesh

Re: Sketch preferences / behavior

Phenom
Phenom

I find in NX when creating extrusions, it looks for any closed contour than if there are overlapping sketch elements or not. Yes, it’s sketchy and flimsy.

You may try “Curve intent Rule” incorporate with path selection tools. Also  there will be stars indicating open ends of contours.

In the other software, I am sure you have seen, “Check Sketch for feature” tool as well to highlight the problematic, overlapping, gaps areas to correct them efficiently.

Hope NX will introduce them in future.

Michael Fernando


Die Designer
NX 11.0.2.7 + PDW

Re: Sketch preferences / behavior

Siemens Legend Siemens Legend
Siemens Legend

Besides using the above mentioned selection intent methods, there is also a new function (NX 10)  in the sketcher (it is also available outside the sketcher) called 'Optimize Curve'. It is intended for the the situation you mentioned, especially if you have imported curves from some other CAD system.

 

The function should take care of automatically deleting duplicate curves lying on top of each other as well as removing gaps between end points smaller that a specified amount.

 

This command should be run before constraints are applied as it will remove some constraints and you do not have a choice as to which constraints are removed.

 

Hope this is helpful,

Abe

Regards,
Abe