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Creating Flat States using Part Simplifified Representations


Creating Flat States using Part Simplifified Representations

Cero currently allows you to create a simplified representation of a flat state to display the formed model.

However by the default Master Rep is the part in its flat state. This makes using the part in assembly’s an issue if you were to use this method.

It would be very powerful if the simplified rep of the formed model was the flat state, instead of using the Family table method (so the master rep would be the formed model)

This would make part and drawing management a lot simpler, Have experienced Issues with Flat states of models been linked to two generic parts. Issues with copying models and their associated drawings can cause delays while they are sorted.

Allow a simplified Rep to unsuppress a feature in a part.

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I had the exact same problem. Its weird how family tables arer a completely accepted solution for this! I found unbending then bend back worked well. They automatically unbend and rebend all bends in the part so you don't have to keep clicking on each one. This then allows for a simplified rep where the bend back feature is supressed, allowing master reps to still have the bend features. This does not work with forms however, for our purposes it worked well. - the thread I made previously. Hope that helps!

What Hannah said.

I create an Unbend feature and a Bend Back feature. This makes the final state (default state) bent. In the simplified rep "Flat" I simply Exclude the Bend Back feature. In the drawing, you can have both views, and in the next level assembly, it comes in bent by default.

Of course, the Unbend and Bend Back can be finicky but for basic sheet metal, it seems to be working well.

It seems the Unbend is replacing the Flat Pattern. You don't get the Bend Back option with Flat Pattern. There must be some logic here that I am not aware of.

The thing with the flat pattern is that it handles forms as well, unbend wont do that.

Plus there is that thing where Pro/E will always put the flat pattern at the bottom of the feature tree.

PTC has to look over this basic requirement for Sheet_metal,


‌A work around for this would be to use the Defualt Rep of your assembly. You would assemble the sheet metal part and display it in the formed state and assemble additional parts to it. You could then set the configuration option to open Default Reps by default. Master Reps and Default Reps are the same at the start the difference being you can save changes in model displays to the Default Rep. No family table needed just a change in the way you work with the models And which reps you work with by default.

Two things of note were models assembled to a sheetmetal will display in an orientation with respect to which state the sheetmetal part is displayed in and doesn't seem to be modifiable and you can save a part rep named default and it will show up as Default Rep but will cause Creo to crash if you try and save the model. This was done using Creo 2 M070.

5-Regular Member

Look at this video, but this trick is allowed only in Creo 2:

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