Different views with different reference set

[cubalibre000]

Hi,
I've a part that has two body inside, one is the screw and the other is the clip.
I've three reference set, one 'model' with two body, one reference set with the clip body and one with the screw body.
This part is bought with these two parts.
I need to make a drawing that explain the dimension of the forniture.
How can I make two different view that are linked to two different reference set ?
See attached image.

Thank you...

Using NX 8 and TC9.1

 

[ewh]

Try using Arrangements

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

 

[cowski]

How can I make two different view that are linked to two different reference set?

You don't. Reference sets are not intended to control drawing views.

I'm not sure that arrangements will work if both bodies are contained in the same file. Arrangements work best with components. You could make a proper assembly out of the two bodies, then use arrangements. Alternatively, you could also use "layer visible in view" or a view dependent edit

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[cubalibre000]

I'm sure that it's possible because when we create sheet metal drawing we have tha reference set model where we dimension the sheet metal part and a flat-pattern wiew that are related to the same component (double in the ANT) that are related to the flat pattern object reference set.
We attend Jhon or I open an IR.

Thank you...

Using NX 8 and TC9.1

 

[stephlouv]

I see two solutions.

A/
At the drafting level, put each body an different layer.
And then, make them visible or not in your views using the "layer visible in view" (Ctrl+shift+v)
A bit tricky as nothing indicate it. Would be a kind of mistery if someone else is working on your file.

B/
Use the "Hide Component in view" tool. (Drafting edit toolbar)

In your case, as you have few objects, i'll go with B.

Stéphane

"My english is bad ? That's why i'am french."

 

[cowski]

The sheet metal application creates a new view for the flattened part, it does not control what is in the drawing view(s) via reference sets.

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[cubalibre000]

Sorry, but the flat pattern view is controlled by the reference set. If you change the reference set to model, the flat pattern view change to visualize the 3D model.

Thank you...

Using NX 8 and TC9.1

 

[stephlouv]

Erratum :
"Hide component in view" won't work as your 2 bodies are inside the same file (not assembly components).

"My english is bad ? That's why i'am french."

 

[JohnRBaker]

Try putting the bodies on different Layer and then use 'Visible in View' to set the visible layers for each view.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[ewh]

You can still erase (View Dependant Edit) the solid from the view instead of hide component.

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

 

[cowski]

If you are set on using reference sets, you can add the model to your drawing twice and use the 'clip' reference set for one view and the 'screw' reference set for the other. If there is a parts list on the drawing, you will have to use the 'plist ignore...' attribute to remove one of the copies so the quantity on the parts list is correct.

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[cowski]

Sorry, but the flat pattern view is controlled by the reference set. If you change the reference set to model, the flat pattern view change to visualize the 3D model.

In sheet metal there is the flat solid (which will get added to its own reference set) and the flat pattern (curves that will be added to a custom view). If/when you create a drawing file and add your sheet metal part as a component, you can change between the flat solid and model reference sets to see your part in different states. But you cannot use both reference sets simultaneously to get two different views of your part on the drawing. If you are using the model ref set and create a drawing view, the drawing view will show the model ref set. When you change to the flat solid ref set, upon updating, the view will show the flat solid. You can add the custom flat pattern view from the sheet metal part to view that on the drawing, but that is not using reference sets to control a drawing view.

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[cubalibre000]

Hi cowski,
what NX does for sheet metal parts can be replicated on normal parts, I've to use the John solution.

Thank you...

Using NX 8 and TC9.1

 

[cowski]

what NX does for sheet metal parts can be replicated on normal parts

This is true, but this discussion about sheet metal is a red herring. There is nothing sheet metal does that will solve the problem you originally posted.

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