×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Multiple part configuration in a drawing

Multiple part configuration in a drawing

Multiple part configuration in a drawing

(OP)
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

RE: Multiple part configuration in a drawing

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

RE: Multiple part configuration in a drawing

(OP)
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

RE: Multiple part configuration in a drawing

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

RE: Multiple part configuration in a drawing

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.

RE: Multiple part configuration in a drawing

(OP)
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

RE: Multiple part configuration in a drawing

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.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources