Can't Select All Sketch Entities

[JPM73]

Hi Everyone,

I created a sketch on a datum plan & used the rectangular feature & fully contrained the sketch.

After exiting out of sketch & using the Extrude feature, some of my curve entities are not selectable, even after use filters such as single curve, connected or tangent.

What would cause some sketch curve entities to not be selectable for a relatively simple command? More importantly, how can I get my extrusion?

Thanks

Jason M.
Unigraphics NX Designer

 

[JPM73]

I forgot to mention, in case it makes a difference that I'm using NX 7.5.

Jason M.
Unigraphics NX Designer

 

[JohnRBaker]

Make sure that some of the curves were not accidentaly created as 'Reference Curves' (indicated by they being displayed using a 'phantom' line font). Reference Curves are not considered part of a sketch profile and therefore are not selectable in modeling operations, such as Extrude.

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.org/museum/

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

 

[JPM73]

Hi John & Others,

As far as I can tell & should be, all curves are on the same plan - In most instances, on a datum plan. None of the curve entities that I'm trying to extrude are references curves either.

My cue line says my sketch is fully constrained, which it appears to be. However, for whatever reasons, I cannot select some of the (solid) sketch curve entities. With other sketches, within the same CAD file, I have virtually the same thing & have no problem getting a solid from the extrude feature.

I even selected sketch curves entities in different order & that didn't seem to help either.

Any other reasons that would cause this or how I can get this fixed?



Jason M.
Unigraphics NX Designer

 

[cowski]

Can you duplicate the problem consistently (ie in a new file)? If so, contact GTAC.

 

[JohnRBaker]

Try going to...

Preferences -> Grid and Work Plane...

...and checking the options in the 'Objects Off Work Plane' section of the dialog.

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.org/museum/

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

 

[jerry1423]

There is a chance that the curves that are not selectable are not within the sketch, and are either in the model space, or part of a differnt sketch.

 

[jerry1423]

Do an "info > object" on the curves that are not getting selected and see the info it gives, including being part of that sketch

 

[JPM73]

Hi Everyone,

Thus far, the above suggestions are not working.

Just to test or to see if I can duplicate thei issue, I put a sketch on a datum plan & made a rectangle, using the internal sketch rectangle feature & let the auto constraints provide some constraints. I then exit out of sketcher, used the Extrude feature & made a rectangular solid, as it should.

Then, I went into sketch edit mode, applied some simple dimensional & geometric constraints & made a "fully contrained sketch".

When exiting, my 2 vertical sketch lines were no longer part of my extrusion string. I also attempted to add them back in, but I cannot select, no matter which option I choose.

What the heck is going on with NX 7.5 or this issue?

Any suggestions to how to get fixed (quickly)? It appears that I need to contact GTAC to.

Thanks

Jason M.
Unigraphics NX Designer

 

[jerry1423]

yea, probably contact GTAC. They may ask you to send them your file.
If it is a bug then it really needs to get fixed.

 

[JohnRBaker]

I was not able to reproduce the described behavior using NX 7.5.2.5, which should be available for download early next week.

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.org/museum/

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

 

[JPM73]

Hi John & Others,

I submitted my file to GTAC for review. This may be file specific issue, but I did have some other instances where I had the same situation. However, at the momenent, I can't duplicate the issue.

As for NX 7.5.2.5, I need it today if this the solution to my issue.

Thanks


Jason M.
Unigraphics NX Designer

 

[JPM73]

Hi Everyone,

My problem is resolved!!!

It appears that I had my modeling tolerance too high & by going to:

Prefernece --> Modeling, General tab, change the Distance Tolarenace from 0,0254 to 0,010.

Thanks

Jason M.
Unigraphics NX Designer

 

[jerry1423]

Thanks for the update, and what turned out to be good advice

 

[JohnRBaker]

Out of curiosity, exactly how SMALL a rectangle were attempting to sketch and then extrude?

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.org/museum/

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

 

[JPM73]

Hi John,

I was creating a .020 x 1 rectangle. Apparently, having 0.0254 model tolerance was a little too high.



Jason M.
Unigraphics NX Designer

 

[JohnRBaker]

Yes, the problem was that since two sides of your rectangle were only 0.020mm apart and with a modeling tolerance of 0.0254mm, after you had selected one side of the rectangle, when you tried to select the curve opposite it the system thought that you were trying to select the original curve twice.

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.org/museum/

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