UG NX 11 -Model Not Showing in Drafting Mode

[DerkMc]

We received some UG files from a customer. They used master modeling mode and when I open the model, I can see the 3D geometry. When I open the drawing "model" file I can see the complete drawing, but when I swap to the model side of that file the 3d geometry does not show up. All layers are turned on. The correct reference set is selected. When I activate the 3d model file in the drawing file, it will let me edit the features...without showing me any 3D geometry and the drawing will update to those edited features.

What simple thing am I missing that is preventing me from seeing the model in the drawing file?

Thanks in advance!

 

[Toost]

This is NX version # ?

Try Layers visible in View and the Reset button.

Regards,
Tomas

 

[DerkMc]

NX11. I put it in the title but, maybe I should have put it in the body also.

That did not change anything. Does "Layers Visible in View" change the "model" portion of the file?

 

[Toost]

I missed the title...
The reason i asked was that Siemens actively tries to remove the possibility to view the model in 3D in the drawing file.
It was simple but getting more difficult.

The layers visible in view ,
each view can have view dependent layer settings visible/invisible. ( The Work layer is still a global setting but it can be invisible in the single view you are looking at...)
the intention of this is good.
imagine an assembly of 2 parts, A and B.
A resides on layer 2 and B on layer 3 ( in the drawing file)
In view 1 on the drawing you set layer 2&3 visible. Both A&B visible together.
view 2 on the drawing you set layer 3 invisible. ( only A visible)
view 3 on the drawing you set layer 2 invisible. ( only B visible)

But, if one looks at a modeling 3D shaded view, you can globally have layer 2&3 selectable ( Layer settings), but in this view, layer visible in view, set layer 3 invisible, you will only see A.
And then , if you make Layer 3 the work layer, it's still invisible. create "something" it will be created but you will not see it. ( nowadays there is a warning on this.)

the assembly navigator when you are viewing the drawing,
- do the assembly components have icons with a miniature drawing underneath ?
Or do they appear "normal "

/ Tomas

 

[DerkMc]

The component icon has a miniature drawing underneath.

Also, I have noticed that my actual title may be misleading. "Model Not Showing in Drafting Mode" when 'Drafting Mode' should read 'drawing file' to be more accurate.

So, just to be clear for anyone that may find this thread in the future. My issue is in the drawing file of a master modeling file set. But my issue is not on the drawing itself. My issue is in the 'modeling' side of my 'drawing' file.

 

[Toost]

I think i know the issue.

You have a case where you have an assembly ( or piece part) containing the model and "above that" a drawingfile which contains the drawing, showing the model in the views.
and if you open the drawing file and then switch to the modeling application but keep the drawing file as the displayed file,
it's "empty".

The icon with that drawing underneath is a "drawing component" , also called "View from part".
It does only appear in the drawing views * and never in 3d. * projected from the initial view or detail views/section views.
The intention of drawing components was to add a view of a related part to a drawing, maybe illustrate the context of a detail.
i do not know of a replacement method , to switch a drawing component to a regular component.
Drawing components will not appear in partslists.


Regards,
Tomas

 

[DerkMc]

This appears to be the exact issue.

As a test, I just started a blank drawing and inserted a "Base View" of a part that was already loaded into memory. This created a "Drawing Component' in the Assembly Navigator.