Points & lines in views in NX 8.5

[Jashe]

I need to draw some points & lines in a view in NX 8.5 but I cannot get the points or lines to snap to the part (e.g. to a center of a hole or the end of an edge). Anybody know how to do that?

 

[JohnRBaker]

Are you working in the context of an Assembly? If so, make sure your 'Section Scope' is set to 'Entire Assembly'.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[JohnRBaker]

I meant 'Selection Scope' (damn spell checker).

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[Jashe]

I'm actually in the Drafting application (context).

 

[Xwheelguy]

If you're not using the Sketcher in Drafting, MB3 (right click) on the view boundary and select Expand from the pulldown. You should now be able to snap to any valid geometry in that view. Keep in mind that any geometry you create will ONLY show up in that view (often called View Dependent geometry).

NX uses View and Model Dependent concepts for things like this. If you want the View Dependent geometry visible in other views, MB3 on the view, select View Dependent Edit and then select View to Model to move the geometry to the Modeling side. If you have ANYTHING associated (dimensions, view boundaries, etc.) to the View Dependent geometry, you will NOT be able to move it over to Modeling.

Tim Flater
NX Designer
NX 8.0.3.4
Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[JohnRBaker]

Even if you're working on a Drawing the 'Entire Assembly' option is still relevant.

And there is no need, if you're using NX 8.5, to have to 'Expand' a view before you can add curves to it. You now simply select the view, press BM3 and select the 'Activate Sketch' option and you can now add SKETCH curves to your view while still working in the context of the entire drawing.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[Jashe]

Ok, so I can create geometry in a view but is there a way to constrain lines and circles to the part. When I try to constrain something I can't highlight the part of the body I'm trying to constrain to.

 

[UGperson]

You have to extract the edges in the view. To do that RMB click on the view in the part navigator. Then pick style under the general tab check the extract edges box.

 

[Toost]

You must make sure that Extracted Edges is ON.
Double click the view ( Style...) on the General tab in the top box , turn ON Extracted Edges.

If this is already on, make sure that the layer with the model is Selectable.
Since Drawings use the option "Visible in View" it is possible so see the model despite that the model is "non- selectable".


Regards,
Tomas