Assembly states in drawing

[red devil]

I have an assembly which I have 2 plates that are connected bya hinge. I want to be able to show the assembly in the closed and open (90 degrees open) states on the same drawing sheet. Anyone know if you can do this?


TIA


RD

 

[vlad1979]

Don't think you can do this for the same assy. When I want to showthe assy in closed position I close the assy and save it as a shrinkwrap. Thenthere are two ways to do the drawing:


1.you assemble the shrinkwrap into your assy (assemble default) and the view will show both states (I'm making the shrinkwrap part phantom transparent to clear the view view/drawing display/component display/ style/ phantom transp).


2. or you make a separate view to show the closed position with the shrinkwrap part as model for this view.


The disadvantage of doing like this is that you have to make a new shrinkwrap every time you change something in your assy.


Or you could make an instance of that assy to show the closed position (just put theangle dimension in family table).I'm not doing this because I need to show open/closed position in the same view.

 

[raw2448]

hi


Yes it can be done, very easily by using family tables.


If you need detailed help on how to do this post your email address and Iwill send you a word document giving step by step instructions

 

[proengineertips]

using simplified rep can acheive as well

just create simplified in ur model and u can set it in your drawing view.

 

[jabbadeus]

No, no, no, this absolutely can be done.


Okay, it sounds like your assembly is a mechanism, as in you have components that are connected with connections (e.g., cylinder, slider, pin).


What you want to do is take snapshots of the assembly by selecting Applications > Mechanism andusing the Drag icon (looks like a hand) and taking Snapshots (upper right hand corner, looks like a camera)to represent the various positions you want to depict the assembly in. In that same dialog box there is an icon that looks like a camera, almost like the snapshot icon but with a box around it, that makes the snapshot available in drawing mode. (Hover your mouse over the icon, and it will explain the functionality as "Make selected snapshot available in drawings.")


In the drawing, place a view, and go to the View States tab, check the "Explode components in view" option, and from the drop-down list, your snapshots will be available to you.


I know it's not intuitive; I had to be shown this functionality by a PTC person.