Render Sets (Drafting) 1

[mcclark]

I'm creating a drawing of an assembly and I want to make one part in the assembly have phantom lines. I used render sets to make the lines in that component phantom, but when I did so, the edges that were previously hidden (because another component was blocking it from view) are now showing up as phantom lines. I currently have "edges hidden by edges" selected, which seems to only hide the edges that are hidden by other edges in the component with phantom lines, it isn't hiding the edges that are behind the solid line components. The component with phantom lines is behaving correctly and the component with solid lines is behaving correctly, but they aren't working correctly together (I'm seeing phantom lines that should be hidden by my solid components as well as solid lines that should be hidden by my phantom component). It seems like this should be a simple fix. Any help is appreciated.

Running NX7.5

 

[tk369]

MC..
Instead of using render sets, have you tried to click on the component, and edit>object display>linefont>phantom? This changes the whole solid model component to phantom. The hidden lines will be invisible/dashed per your preference, while the solid object itself will come in phantom. I just tried it on my assembly. Cake!

ted kralovic

VisVSA, NX-6, Macbook, iPhone 3GS, Garmin 765T, Garmin Forerunner 405, Garmin eTrex Vista Hcx, among others

 

[eex23]

tk369: your option will work, if you want to have phantom lines (eg for one of your components) in all drafting views. To have phantom lines in only one drafting view (for same component) this trick will not help. The only solution then is "view dependent edit" but it takes too much time.
I also facing with the problem mcclark described above. Have not found solution for this yet.

NX7, 64bit

 

[jerry1423]

If you are making only one component phantom then go into the model space of the assembly drawing and change it there.
In the Visible Lines tab under View Style make sure the font (middle pull-down) is set to Original
and then it will appear as phantom on the drawing

 

[eex23]

jerry1423: on the drawing in all views you will have this object with phantom lines how to make phantom lines in only one view?

 

[jerry1423]

Ok, I will redo my above reply so you can get want you want:
If you are making only one component phantom in certain view then go into the model space of the assembly drawing and change it to the display of the model to phantom (and probably thin line width) in there.
In the view(s) that you want that object to show as phantom in the Visible Lines tab under View Style make sure the font (middle pull-down)
is set to Original (top choice) You may want to do a similar thing to the line width (next pull-down menu to the right) so that it comes in as Original (so the phantom lines come in thin)
In the view(s) that you want that object to show as solid in the Visible Lines tab under View Style make sure the font (middle pull-down)
is set to Solid Line (second from the top choice)

 

[eex23]

jerry1423, thanks.

 

[Dave K]

When you create the render set, I set the "hidden line" option to invisible, and the "visible lines" option to hidden.

If that doesn't work for whatever reason, I'll wave a copy of the solid onto a different layer, and change the edge font of that to phantom for those views.

-Dave

NX 7.5