Point in expanded view. 1

[jerry1423]

I am on NX6
I am trying to put a point in an expanded view, for a folded radius dimension, but "point" is greyed out.
Why is that?

 

[cowski]

If you customize the menu/toolbars you will see there are 2 options for the "Point" command. 1 works in expanded views, the other does not. Add the one that you need to your toolbar/menu.

As to the "why" question: I think it is just to confuse us!

 

[JohnRBaker]

I can't help but ask, if all you wish to do is place a point within a Drawing view, why are you 'expanding' it first? After all, if you're using NX 6.0 you can now simply make a Drawing view a 'sketch' view and then you can create all the points that you wish (as well as lines, arcs and splines). Just select the view of interest, press MB3, select the option titled 'Active Sketch View' and you can now use any curve function found on the 'Sketch Tools' toolbar, including 'Points'.

BTW, with NX 7.5, if you DO decide to expand a drawing view the, 'normal' point function will now work just fine.

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.

 

[DaSalo]

John,

What are the limitations of using a drawing view as a sketch view? For example, can you sketch a spline in a drawing view and then use it for a broken out section boundary? What is the fundamental difference between placing geometry in an expanded view vs. placing the same geometry in a sketch view?

Thanks,
Dasalo

 

[JohnRBaker]

With respect to what you can do with the curves created in an expanded view verses in a sketch view, in terms of using them to perform Drawing specfic operations, such as controlling partial sections, redefining view bounds, or simply to add reference geometry which can be dimensioned to, there is virtually NO difference whatsoever. The big difference is in how do we know where the curves are going or not. When creating simple non-sketch objects we NEED a scheme by which the system KNOWS where the user expects the curves to be create relative to, therefore you need to EXPAND the view of interest before you're allowed to create curves which will 'live' in the view. However, when creating a sketch view, all the user needs to do is INDICATE which view (or the drawing sheet) that he wishes to create the SKETCH objects relative to. The idea is that as sketching becomes more usable and functional, that this will provide more productive workflows when making drawings then the need to pop in and out of viewing using something like Expand/Unexpand operations. It's basically a productivity issue since the feeling is that it's more intuitive and straightforward.

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]

I forgot all about "sketching" in the drafting mode. I will try that.
Thanks for the guidance.

 

[NXrabbi]

I'm surprised to see that none of the responses mention the Offset Center Point function. Wassupidat, John? Using an Offset Center Point was the recommended best practice for creating Folded Radius Dimensions. It is a fairly robust function and tends to work well within the confines of keeping drafting entities view dependant to the drawing view and not the archaic practice of creating drawing geometry inside of Member Views. Tends to remove layer considerations from the picture as well if you have a standard layer for all drafting objects.

- Garrett

 

[jerry1423]

Thanks NXrabbi,
I thought I remembered a post like that, but I couldn't find it.
We are working on some huge parts, with large radii, so I better take the best route when doing this type of dimensioning.