ASSEMBLY DRAWINGS IN NX9

[64polara]

would someone please explain to me what the icon in the drawing navigator means.
When I add a base view of a component (only assembly files) that has been added to the drawing file, I get two components to unpack, 77x2087-101 files as shown in the attachment. one has the icon that looks like a drawing, where as the other is icon is the usual.
if I select the first -101 component it does not hi-light in the view but it does appear on the modeling side of drafting.
if I select the second -101 component with the drawing icon it hi-lights the component in the view but does not appear on the modeling side of drafting. Why is this?

I know what I need to do when adding views to hi-light the model and it appears in modeling, add base view from the drawing and all works fine, just need to manipulate the layers in each view.


Wayne Huseby
Drafting Checker/Drafter
United Technologies Aerospace Systems
Jamestown, ND 58401

 

[JohnRBaker]

Are you a new user? If so, I suspect that you need to be properly trained or at least mentored by someone who knows how to make proper Drawings from an Assembly.

That being said, it appears that you've added an additional Component to the Assembly Drawing file itself. Now there might be times when this is desirable, which is why NX allows you to do so, but it's generally not the normal workflow. What exactly are you trying to do with this added view?

John R. Baker, P.E. (ret)
EX-Product 'Evangelist'
Irvine, CA
Siemens PLM:
UG/NX Museum:

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[64polara]

No John, not a new user, 32 years of UG. It has been a while since adding assemblies to drawings.
Our standard practice is to create the new drawing file then add the component to be drafted to the drawing.
I have just noticed recently this happening when viewing the file structure from other drafters.
Just wanted to know the significance of the icon for the additional component.
as for the reason for the extra view, just to show what happens where one assy shows and the other does not in modeling side of drafting.

You have been around for almost ever and glad to see retirement as not taken you away from UG. I have always valued your comments.

that said, what is the best and recommended practice for adding a component to a drawing? Actually what we do is open the component to be drafted, create the new drawing file, add component to the drawing using assemblies then place views on the drawing and do our thing.

Thanks your thoughts.

Wayne Huseby
Drafting Checker/Drafter
United Technologies Aerospace Systems
Jamestown, ND 58401

 

[NutAce]

Basically, working mastermodel, when you have the component open and create a new drawing, Nx should recognize the component and add it to the drawing...
From there you can start create your base views and select the drawing file as the reference for the views. (actually if I am correct it should do this automatically)

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2
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[cowski]

The icon that shows a yellow cube on top of a drawing is known as a "drafting component"; these are imported views from other files, they do not show up in the modeling application nor do they show up in a parts list. Drafting components have been around for a while in NX, but around the NX 7.5 timeframe, they became the default OOTB option. When using the "base view" command, pay special attention to the "select part" step; here you can select the current drawing file or a different part. Adding views from other parts can be handy, but it is not necessarily the desired default workflow for longtime users with established practices.

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