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Creo 2.0 Sheetmetal - Simplified Reps for flat pattern drawings


Creo 2.0 Sheetmetal - Simplified Reps for flat pattern drawings

The flat pattern feature is persistent about being the last feature in a model tree.  There is a way around this using simplified reps.  This work-around is specifically geared toward maintaining a master rep as you default assembly part where the sheetmetal part remains in the formed condition by default.


This technique uses the bend back feature -after- the flat pattern.  It is a similar method to using unbend and bend back but it was requested to study this option using the flat pattern feature.


This is not a good technique for forms.  You will note in the video that the flatten forms option is specifically not selected.  Note that forms can be flattened as a separate operation, but in a simple technique where the master rep should be the master part, this is not as simple as defined in this document or this video.


Please feel free to add comments and further the discussion.


And I apologize for the video quality overall.  It is the best I can do with the tools at hand.


The video aims to:

  • show how to add a bend back feature after the flat pattern feature using simplified reps
  • show how to make a drawing with both types of views using the simplified rep
  • show how to toggle the two states using the display state (all) feature
  • show how the default assembled model is the as-fabricated part.



Thanks alot for showing this.  The one thing that still bites us with simp reps is the drawings. We do use family tables and once you have a simp rep in the drawing that view is locked.

If we do a replace by family table member the master rep with switch but the simp reps will not. The view using the simp rep needs to be deleted and remade.

This is just an FYI for those out there that are not familiar.

Thanks for adding that, Andrew. 

I still haven't got a full handle of all the ins and outs of simplified reps. 

Add family tables and now the problem is compounded yet again.

I'll be the 1st to admit that this still doesn't solve all the issues surounding flat patterns on sheetmetal fabrication drawings.  One can only hope that PTC is watching this for Creo 3.0.


Thanks for the method.  We try to avoid family tables as they tend to be problematic with WindChill.

Here is the cheat sheet that I created:


a.       When creating flat pattern goto options and uncheck “Create relief geometry” and “Flatten forms”.

2.     2  VIEW MANAGER

a.       Create Simplified Rep – eg. “Flat_Rep”

b.      In “All” tab create combined state – eg. “Flat_Display”

                              i.      Select “Reference Originals” in prompt dialog.

                              ii.      Redifine combined state

1.       Orintation: None

2.       Simplified Rep: Flat_Rep

c.       Close

3.     3  Create Bend Back feature

4.     4  Change state of Bend Back feature to Exclude.

5.     5  Save Simplified Rep in View Manager

6.     6  Switch to Master Rep

a.       Resume Bend Back feture.

7.     7  Select combined state “Flat_Display” to create flat view.

There is always more to learn in Creo.

Kevin I really appreciate the work around for the Flat Pattern. This was driving us nuts.

Just wanted to update you on this. Looks like this loophole is "fixed" in Creo 3.0 and it doesn't work. It wont allow you to add the bend back after the flat pattern. even in the simp rep state it is still placed before the flat pattern. So it looks like I wont be able to use this once we go to Creo 3.0.

True, this is also a problem in Creo 2.0.  It would work until you close the part and open it again later.

The problem is that the flat pattern is always the last feature.  I have no idea what PTC was thinking in doing this.

That is why unbend works so well, -IF- you don't need form features flattened.

Ya i have been bugging the PM in charge of Sheetmetal for this and have escalated it to the VP. He will push for it to be in Creo 4.0 *crossesfingers*

And a piece of missing WC technology to support this initiative would be nice to have: Support of part level simplified reps in Creo View


Great tip.

l have used it up to now. Upgraded to Creo 5.0 and this trick doesnt work.

Does someone know how to use something like this in Creo 5.0?


Thx for advice