Editing Line colour in drawings

[Nick Green]

Another query coming from my evaluation of NX as a replacement for Inventor.

We regularly change the colour of components in drawings from black to grey to give clarity to drawings. So for a fabrication, the first sheet would have isometric views with the BOM table and balloons, sheet 2 would have the primary structure with minor components hidden, and sheet 3 would show the minor components with the primary structure shown in grey.
In Inventor, I can select a sub-assembly or component part from the model tree and change its line colour & style in any view. At the moment I have had no luck finding a way to replicate this in NX without changing the part colour which isn't helpful.

I'm sure there is a way to do this so could someone show me where I am going wrong please!

Nick Green
Lead Design Engineer
IHC Engineering Business Ltd.
UK

 

[gowri91]

There are few options:-
1.Render sets(to change line type, width, color, and visibility).
2.Hide component in view(Edit-view-hide component in view).
3.View dependent edit(to change line type, width, color, and visibility).

 

[Nick Green]

Nice ideas, obviously 2 is just hide so not a solution...

Is there a way to be able to select a whole component for 1 & 3 rather than just faces & edges? It seems a very laborious way to do this.



Nick Green
Lead Design Engineer
IHC Engineering Business Ltd.
UK

 

[ewh]

As to no. 2, one method is to change your type filter to solid body when erasing objects in the View Dependent Edit operation. Any extraneous geometry may have to be selected separately.

"Know the rules well, so you can break them effectively."
-Dalai Lama XIV

 

[Nick Green]

Erasing objects isn't what I am trying to do, though it is a useful tool.

What I don't seem to be able to do in the View Dependent Edit is to be able to select an entire component rather than having to select every line.

So I right click on the view border and select View Dependent Edit. In the View Dependent Edit popup window, under Add Edits, I select Edit Entire Objects and then Apply.
This brings up the Class Selection popup window but unfortunately now the only selection options available seem to be No Selection Filter, Curve, Edge & Face. This isn't exactly helpful.

Nick Green
Lead Design Engineer
IHC Engineering Business Ltd.
UK

 

[petulf]

I would use partial component shading if I wanted to add emphasis to a specific component on a drawing.

See the attached pdf file for a how to.

Edit: If you do not want any shaded faces, only change the line width and curve type and set translucency to 100%

 

[MND71]

Secondary geometry representations i a new function in NX11.

https://docs.plm.automation.siemens...index_whatsnew:id1241822:xid718233:xid1096348

I-deas
NX8->NX11
Solid Works 2016
Windows 10

 

[Nick Green]

All good stuff.

I was having a confused time until I remembered that greys don't work if the drawing is set to monochrome!

A way I have found for selecting whole parts or sub-assemblies in the View Dependant Edit process is to hide all other components and then use Select All in the Class Selection pop-up, hit OK and then make everything else visible again. This is a bit laborious but is at least easier than selecting by curves, edges and faces.




Nick Green
Lead Design Engineer
IHC Engineering Business Ltd.
UK