Sketch Solver in NX6

[mrsdesign]

Hi,
I am a recent convert to NX - I am used to v5 and miss the sketch solver. Can anyone suggest an efficient way of telling whether your sketch is joined together fully - all intersections G0 - I am getting fed up of going into downstream operations just to find I am not quite there.
Your advice would be gratefully appreciated.

 

[fighterpilot]

In your status bar it should tell you when your sketch is fully constrained. See attached for the message.

I'm with you, I like all my sketches to be fully constrained. Old Pro/E and V5 habits don't die. You can set an option to show all constraints as you sketch (Tools/Constraints/Show All Constraints) which may help you as well.



--
Fighter Pilot
Manufacturing Engineer

 

[mrsdesign]

The trouble is that you can be fully constrained, but with open profiles and common lines in a sketch. It is only when you look to perform solid operations on them when you find out you have self-intersections or open curves.

It would be great if NX could show you if your profiles are open or closed and highlight gaps, maybe it can and it is just me not knowing where to start.

 

[moudy1]

Curve ends that are Coincident will show a small square. You may need to toggle on show all contraints and uncheck the sketch preference "Dynamic Constraint Display". When checked, constraint symbols do not display if the associated geometry is very small.

 

[JohnRBaker]

The issue of having an 'open' profile has absolutely nothing to do with 'solving' your sketch. For most the functions where a sketch can be used as a profile, an 'open' profile is just as valid as a closed one. In fact, for many functions, such as freeform surfaces and many of the Sheet Metal operations an 'open' profile is the desired and often expected type of input object. Therefore, 'warning' the user that a sketch is 'open' would be seen as a nuisance by anyone creating profiles which would be used for things like Swept surfaces, Variational Sweeps, Surface Through Curves, etc., or even by someone using Extrude/Revolve to create sheet bodies which would be used to trim other solid bodies. Besides, when selecting a sketch profile for something like an Extrude or a Revolve, where normally one would expect there to be an 'closed' profile the majority of the time, you will be shown that the profile is open, but you can still continue, since that might be what you're looking for.

And as for so-called duplicate or self-intersecting curves in your sketch, again there it nothing inherently 'wrong' with creating a model such as that since the functions which can use a sketch as imput often can accommodate things like duplicate/redundent curves with no problems. Granted, it might be seen as a poor modeling practice, but it's not one that will cause you models to be invalid or inaccurate. And as for so-called self intersecting sketch profiles, again, by using the 'Curve Rules' during the creation of things like Extrudes or Revolves with their ability to stop at intersections, follow fillet, and the recently added 'Path Selection' tools, these allow the user to use sketches which were easier to create since they did not need to be reduced to a single closed loop in order to be usable. This allows the user to constrain a sketch in a much more direct way and then using the curve rule to select the proper profile.

Here's an example of what some might considere a self-intersecting sketch...

...or at least one where there is no single unambiguous profile which can be used to create say an extrude. But what if all I wanted was the interior loop of curves and yet I needed to dimension to the theoretical corners of the rounded triangle. Think about the extra trimming and creation of reference lines which I would have to do in order to get a single unambiguous profile. However, with this sketch I have a couple of options when it comes time to actually select it, such as using Connected Curves with the Follow Fillet option toggled ON, or more recently, by just doing a single pick in the middle of the profile using the new Curve Rule 'Region Boundary Curves'.

Remember, the sketcher is just a tool which when used in combination with other tools can result in a much easier and efficient workflow, one which does not necessarily require that the sketch be taken to some pristine, totally constrained and unambiguous state before is can be used in some feature creation operation.

Oh, and if you didn't consider the above example 'self-intersecting' enough, then consider this one, keeping in mind that the 'profile' I'm eventually going to be using is what is represented by the interior shape consisting of lines and arcs. Think abour how much extra work you would have to do to get an easy to edit, fully constrained sketch which consisted of a single unambiguous (i.e non-self-intersecting) profile.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.com/museum/

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

 

[DaSalo]

The extrude tool can very easily double as an open loop/self-intersection check even if you aren't using the sketch for an extrude.

Create your sketches through the extrude tool (requires 1 extra mouse click) and leave the selection intent default as "feature curves" (which, I believe, is the out-of-box setting in NX7.5) then as soon as you click "finish sketch" you will immediately return to the extrude tool where it will instantly show you big orange asterisks at all openings and self-intersections. Then you can return to the sketch in one click to fix them or, if you are ok with them being there, continue to create your extrude.

If you weren't intending to create an extrude just hit "cancel". When you hit cancel you will be asked if you want to save the sketch and, conveniently for this situation, the default is "yes" (do save the sketch) so you can just hit middle mouse and your done.

I suppose it would be possible to create a tool within the sketcher that would do this but it would only save two mouse clicks or so.