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NX 12 - Phantom line for one body in drafting

Experimenter
Experimenter

Hello people,

i've been searching for all day and i am little bit desperate about it.

Problem:

I made draft from assembly. Also some views and sections and i need that one part from assembly will have phantom lines in all views. I tried a lot of settings but nothing helps me. I have also changed object settings for that part but nothing happens. Still normal line there. Can anyone help me with this? I found that i can use edit object settings but don't work and don't know why... Thank you for your help

10 REPLIES 10

Re: NX 12 - Phantom line for one body in drafting

Siemens Phenom Siemens Phenom
Siemens Phenom

Hi @Barny,

Edit Object Display (Ctrl+J), select component from assembly navigator. In edit object display dialog, set line font to phantom, OK.

From part navigator, select the drawing node > RMB > Update. Selected component will be displayed with phantom line in all the drawing views.

 

Regards,
Ganesh Kadole
#IngenuityIsNX | NX - What's New

Re: NX 12 - Phantom line for one body in drafting

Honored Contributor
Honored Contributor

It appears the view setting for "Secondary geometry" will do this on a view by view basis.  I know there was an old view setting that would to this too, but I can't remember what it was...it was a bit obscure, and very legacy.

-Dave
NX 11 | Teamcenter 11 | Windows 10

Re: NX 12 - Phantom line for one body in drafting

Siemens Phenom Siemens Phenom
Siemens Phenom

Actually, another way to handle this requirement is by defining a Render Set (it can be a quicker and less complicated method than defining Secondary Geometry). To use render sets, you must first define/create the render set using the Drafting Preferences dialog box, and then apply that render set to all the views in which you want to display the change. (Tip: If you apply the render set to a base view, than subsequent projected views will also display the render set. And you can remove or add render sets to any existing view).

 

So, to define a reference set, use the Drafting Preferences- dialog box-->View-->Common-->General node-->Render Sets group-->Define command. Here's a link to procedure in the Help that demonstrates how to set up a render set.

 

Second, apply that render set to one or more views in your drawing. Here's another link to a procedure that demonstrates how to do this.

 

For an explanation of the difference between Render Sets and Secondary Geometry, and examples of when you would want to choose one over the other, see the information at this link.

Re: NX 12 - Phantom line for one body in drafting

Honored Contributor
Honored Contributor

"Render Sets" is what I couldn't remember, thanks.

-Dave
NX 11 | Teamcenter 11 | Windows 10

Re: NX 12 - Phantom line for one body in drafting

Siemens Honored Contributor Siemens Honored Contributor
Siemens Honored Contributor

Hi @Barny,

 

Here's a quick movie showing how to apply a Render Set and Secondary Geometry.  Note, however, that Secondary Geometry needs to be enabled prior to placing the views, so it wouldn't have been an option in this case.

 

(view in My Videos)

 

Regards, Ben

Re: NX 12 - Phantom line for one body in drafting

Experimenter
Experimenter

Hi Guys,

thank you very much for your replies.

I've tried both ways but with no success. Do you think that there is some problem with settings or with setting with display or something like that?. 

I have created render set but i've got different buttons in view setting. Can't find render set in view setting. Only in general setting for drafting. 

Do you have any idea what it should be?

Thank you very much.

Re: NX 12 - Phantom line for one body in drafting

Siemens Honored Contributor Siemens Honored Contributor
Siemens Honored Contributor

Hi @Barny,

 

Are you collapsed groups hidden?  Open the View Settings dialog and click the gear icon on the top left and see if you have the option to show collapsed groups:

 

 Screenshot - 7_2_2018 , 7_42_25 AM.png

 

Regards, Ben

Re: NX 12 - Phantom line for one body in drafting

Experimenter
Experimenter

No still did not help.. 

 

NX12_settings.jpg

Re: NX 12 - Phantom line for one body in drafting

Siemens Legend Siemens Legend
Siemens Legend
Do you have "Visible lines" as "original" and NOT "solid" ?
- "Solid" will override any other types and make all visible "solid".

Regards,
Tomas