Visible in view

[cubalibre000]

Hi,
I'm converting a part from the old approach to the master model approach.
In the part, the last feature, the sketch named 'DATARI', is visible in the drafting.
When I generate the specification and import the drafting in the specification the sketch is not visible.
Without generate the sketch in the view, how can I render visible the sketch in the view of the specification ?
I know that the specification hasn't the same layer category of the part, but the our UGS support has told us to use the standard NX specification template.

Thank you...

Thank you...

Using NX7.0 and TC8.1

 

[JohnRBaker]

I suspect that the system is doing exactly what it was designed to do. The 'Model' Reference Set should ONLY contain the solid body and NOT any other curves or items such as the Sketch. By default, the 'Model' Reference Set is what is used when you create a Master Model drawing.

But first, why do you even want to see the Sketch in the Drawing? I would expect that you would only want to see the part itself since that is what the drawing should be documenting, not the sketch.

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.

 

[IanxXx]

I havn't got NX7.0 so i cant tell from your file. but if its just a case of reference sets then just use the Entire Part reference set in your specification the use visible in view to make that visible in the relevant view.

Its standard practice for my company to use the entire part reference set whilst drafting as a a lot of sketches are created when defining a part for manufacture and it makes sense to recycle them in drafting.

 

[JohnRBaker]

From looking at your part, you may also need to reset the Visible in View setting for your drawing views since even setting the Component Reference Set to 'Entire Part' is not showing you your sketches. So go to...

Format -> Visible in View...

...and from the list of views, select the one you wish to see the sketches in and hit the 'Reset to Global' button. Repeat this procedure on any Drawing view which you wish to have all the layers set the same as the Drawing file.

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.

 

[cubalibre000]

John,
the sketch 'DATARI' represent the dater positioning for the plastic part.
I need to show only this sketch in the view.
If I set the referenced part with the reference set to entire part, it show all.

For example, in the master model approach, if I would like to show one plane or one sketch, which is the procedure to accomplish this ?

Thank you...

Thank you...

Using NX7.0 and TC8.1

 

[JohnRBaker]

OK, then go back to the master part file, and create a new Reference Set and ONLY inlude in it the Sketch. Then in your drawing use that Reference Set.

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.

 

[cubalibre000]

Ok John...thank you..

Thank you...

Using NX7.0 and TC8.1