NX5 - create silhouette curves from within Sketcher

[acciardi]

Hello -

I have been test driving NX5 a bit and I was disappointed to see that using 'Project Curves' from within the Sketcher environment still will not let me select the edges or silhouettes of a cylinder or any curved surface (from existing geometry) to project onto the sketch plane.

I was under the impression that this functionality would be available in NX5.

Has anyone been able to do this?

Note: This is not the same as using 'INSERT/CURVES FROM BODIES/EXTRACT/SILHOUETTES. This function has been around a while and creates entities seperate from the sketch.

Thanks,

Ed

 

[JohnRBaker]

There was never any promise, implied or otherwise, that we would ever provide that type of functionality in UGS NX 5 or any other future release of UGS NX.


John R. Baker, P.E.
Product 'Evangelist'
UGS NX Product Line
SIEMENS
UGS PLM Software
Cypress, CA

http://www.siemens.com/ugs

http://www.plmworld.org/museum/

 

[acciardi]

Sorry John, but we were told this by a UGS representative. We also made an ER to get this in.

Regardless of the current situation, is this something that could be added, or is there some good reason for leaving this out? It is an incredibly useful function to have.

Ed

 

[JohnRBaker]

Just because it's "something that could be added" does not mean that it will be.

As for the "UGS representative" that you mentioned; remember, not everyone is in a position to know what is really going on nor be in a position to influence what does happen. After all, I work DIRECTLY for the Vice-President of NX development and while I can and have influenced the content of our products, even I can't wish that something were so, just because it was a good idea.

Now that being said, if you'd be interested in a PROCEDURE that accomplishes the same thing, and fully assoiciatively, just not directly, try this:

First establish a Datum Plane that you wish to place your sketch on, which by definition if you were to look normal to at the object that you wish to get the silhouette of, the 'edge' of the surface that you see would be that 'silhouette' curve. Now go to Insert -> Curves from Bodies -> Extract... and select NOT the 'Silhouette Curves' option, but rather 'Isoline Curves'. Now select the Datum Plane as your 'vector' direction and hit OK. When the next dialog comes up set the 'Isocline Angle' to 0 (zero) and hit OK and then select the face of interest.

Now create your Sketch on the existing Datum Plane and once in the Sketcher you don't even have to project the Isocline Curve into the Sketch if all you're interested in is creating other sketch curves constrained relative to it. Of course, if you do wish the silhouette to be part of the sketch profile, you can always first project it into the sketch and go from there.

Hey, it's NOT 'Silhouettes in a Sketcher', but at the end of the day, the results are exactly the same.

It's like in a former life when I worked as a butcher and we would tell the customers; "Don't ask me what's in the sausage, just enjoy it when you're eating your breakfest tomorrow" ;-)




John R. Baker, P.E.
Product 'Evangelist'
UGS NX Product Line
SIEMENS
UGS PLM Software
Cypress, CA

http://www.siemens.com/ugs

http://www.plmworld.org/museum/

 

[acciardi]

John -

Thanks for the detailed reply. Your method is in fact one way that we've been advised to do it. However, it is extra work and I think to be directly able to create the isoclines/silhouettes from within the sketch would be a very good thing.

I understand that UGS has their priorities for what to add and when. For me this has been a very big 'wish list' item since I began with NX a year ago.

Ed

 

[JohnRBaker]

Perhaps, but I've given you (and apparently someone else has as well) what appears to be a usable solution to your 'problem'. My advice would be to try it for yourself and if it fulfills your needs, go with it.

In the 30 years (this coming August) that I've been using this software, if I had stopped everytime I came to something that required me to learn a procedure where I would have preferred to have had an automatica one-button-push solution, I'd still be back there drawing 3 views of a ball bearing.


John R. Baker, P.E.
Product 'Evangelist'
UGS NX Product Line
SIEMENS
UGS PLM Software
Cypress, CA

http://www.siemens.com/ugs

http://www.plmworld.org/museum/

 

[acciardi]

John - we have an alternate procedure that we have been using that keeps the geometry in the sketch:

If you are trying to project the edges of a cylinder, you can select the end faces, then turn them into reference. Then you can snap a new line entity to the quadrant points.

This works great for simple cylindrical shapes, but for complex revolves of course you'd have to use the isoclines.

Thanks for the help.

Ed

 

[JohnRBaker]

I'm glad that you're able to utilize the tools that are there to help you accomplish your tasks.


John R. Baker, P.E.
Product 'Evangelist'
UGS NX Product Line
SIEMENS
UGS PLM Software
Cypress, CA

http://www.siemens.com/ugs

http://www.plmworld.org/museum/