Multiple part configuration in a drawing

[looslib]

We have an assembly of a box with a hinged cover. We want to show with the door open in one view and the door closed in another view. How do I show this?

WF4 m150/WC/PDMLink 9.0 m050


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[dgallup]

I would use family tables and load 2 instances into the drawing as models.

 

[looslib]

Instances gives me the same problem as using simplified reps, increased part count.

NX has arrangements and SW has configurations, which can show different views with parts in diferent orientations. I thought Pro/E had something similar, but cannot find it. I may be wrong.

We tried making the mating od the lid a flexible component, which works in the asembly file, but we have no way of showing the multiple states in the drawing.

I am trying something with a mechanism joint, pivot, but again have the issue of showing different positions in the drawing.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[jmadd]

If you can move it in mechanism, you can show it in different positions in a drawing. You will need to create a snapshot of it in the non-default position, and enable that snapshot to be used in the drawing.

A snapshot is essentially an exploded view that holds the desired orientation/position of parts. You add the view to the drawing and set the explode to the desired snapshot through view properties/view states.

This is a broad overview of how to do it, you can use the help fuctions (look at "Snapshot") or ask for more particulars.

Hope that helps!
John

 

[dgallup]

Snapshots don't update when your part changes. I don't understand your objection to family tables. It's a separate model added to the drawing, not to an assembly.

 

[looslib]

To build the FT assembly, I would need to have 2 lids in my assembly file. One in the closed position, one in the open position. Now my BOM count is off in PDMLink, showing 2 lids.



"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[dgallup]

If you want to do it at the assembly level (which you didn't state initially) just have an assembly dimension (angle or distance) that controls "open" and "closed". Add that dimension to your assembly family table. Create assembly instances of open and closed. Add the instance to your drawing models and add a view. It does not increase your parts count.