Two views assembly configurations on one drawing

[ASC]

Good morning,

I have one assembly and I'd like to show it in two configurations, one with a part constrained to a 45º and another with the same part at a 90º angle.

I have tried to do this with Simple Reps but to no avail.

I first tried to give the angle constaint a different value in each representation but it changed throughout all SRs.

I then tried to have two angle constraints, enabling and disabling per SR but again the enabling and disabling changed throughout all SRs.

Any advice gratefully received.

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[jsarkar · Accepted solution]

You should use snapshot instead of simplified representation. Lets make the angle 45 deg, then u open drag components and click on save snapshot. right click on snapshot and make toggle for drawing. similarly do for other configurations.

Now in the drawing, place view and properties box u check for exploded views and selecte the snapshots.

https://www.ptc.com/appserver/cs/view/solution.jsp?n=CS30049&posno=2&q=snapshot in drawing&nav=ptcproductgroups||||Product+Group||&source=Search

[ASC]

Thank you, Jayanta. I'll have a play around and let you know how I get on.

[jsarkar]

Dear ASC,

welcome to the forum.

Regards,

Jayanta Sarkar

[BrianMartin]

Perfect answer. The only thing I'd suggest in addition would be putting a mechanism so you can leverage some of the benefits it offers. But if you're more comfortable regenerating each time you wish to view a different configuration this method still works. This is by far the best technique to use. I wish more people knew about it.

[rreifsnyder]

HUGE DISCLAIMER: As with most things with Pro/E there are numerous ways to accomplish a task, The optimal choice may depend on many factors regarding what output you need and how it will be tracked.

If you just need to see the component at those 2 places, I would stay away from both mechanism and snapshot. Mechanism is one of those tools that has great power but in my opinion is overhead when you just need to see a component(s) at discrete positions. Snapshot will not update the view automatically when design changes happen and to update you will have to put the assembly back in that configuration to update the views that use those configurations.

I know family tables have a horrible reputation but this is the type of example when it may be the most appropriate course.

The way to do this with a simplified rep would be to use a technique called "overloading". Using this technique the same component is assembled at each position you need to see it in, then use simp rep to see only one at a time.

[Dale_Rosema]

Or you can add angle dimension to the family table and have the two separate instances. I do that frequently with things that are closed (0 degrees) and open (90 degrees).

[ASC]

Would this cause 2 BoM items to be created (i.e. Part1_Open and Part1_Closed)? Our requirement here is to maintain a single BoM reference.

[Dale_Rosema]

Only if both parts were in the asembly together. If you have only one in the assembly, you can just switch between the two to show the two different options. Or for drawing purposes, you could have an open assembly and a closed assembly, the only difference being with part is referenced in the assemlby, the open or closed version (but only one of them is in the assembly).

You can have both models in the drawings but the BOM driven by one or the other (not both). That was you can show both instances in the drawing. Same is true for RH & LH assemblies.

[rreifsnyder]

Since in the assembly angle dimension change Family table method you are still just using the same parts, then no.