Add Planer and Non-Planar Dimensions to Model Geometry in NX11 and Later.
Solution
In NX 11 and later releases, the ability to use 'Menu -> View -> Show Drawing' as in NX9 and NX10 or 'View -> Show Drawing' as in NX8.5 and earlier was removed.
This method is used to replace it, by creating drafting dimensions directly in modeling.
Note that the preferred method is to create dimensions within modeling using PMI (Product and Manufacturing Information) which will allow the creation of dimensions, notes, GD&T, etc.
For those who still need to create Drafting dimensions in , this method may only be used in the Drafting Application. This method has always worked within NX and may be done in either new or existing views even in very old part files.
1. Within Drafting, add a new view to the drawing.
2. Expand the view using these steps: 'Highlight the view boundary -> Mouse Button 3 -> (select) Expand' which will add a check next to the word Expand.
All objects now created will reside and can only be seen within this view, even after it is un-expanded.
If the dimensions are to be placed in a non-planar drawing view like Trimetric, Isometric or custom non-planar view, then use these additional steps.
3. Orient the WCS where the dimension must be created. Set the XC-YC plane orientation where the dimension must be measured and then set the ZC in the exact location the dimension must be placed.
4. Create the dimension.
5. Now un-expand the view to place the user's creation mode back into the Drawing: 'Highlight the view boundary -> Mouse Button 3 -> (select) Expand' which will remove the check next to the word Expand.
Notes and References
Hardware/Software Configuration
Platform: INTL64
OS: window
OS Version: 764SP1
Product: NX
Application: DRAFTING
Version: V11.0
Function: DIMENSION
Ref: 001-7199067