Solid to Sheet metal - distinc elements

[plos]

Hi,

I have created a solid part and converted it to sheet metal part. It consists of 4 distinct pieces. I can unbend all of them but how to create the drawings of each flat piece? 

best regards

Piotr

[Mahesh_Sharma]

Drawing for each distinct piece cannot create.. commonly all the walls should be merged and and a single flat state defines the part for drawing. 

Can you share the file for review? 

[plos]

Thanks for the answer!
Here's the file. I wanted to have each wall as a separate part. I thought there should be an easier way than create 4 different .prt

[Mahesh_Sharma · Accepted solution]

@plos 

As I mentioned previously, you cannot create drawing for each distinct piece.. 

Still if you need that, one of the alternate option can be material removal feature to have each side individually and control by family table. 

As, create extrude features for solid material removal in such a way that it will leave only one side for each extrude. later use family table and control extrude features.. 

[plos]

Thank you. I'll try this way

[Pettersson]

Another way would be to use copy geometry functionality (the way Creo is meant to use to do the things you do with multi-body parts in other programs).

Either do the first part as surface geometry and use it as a skeleton part in an assembly, or just do the part in sheetmetal as you have and make Publish Geometry* to publish the four sides. Then make new parts that copy these surfaces and use the Offset command in Sheetmetal to convert it to a sheetmetal part.

If you want to be extra fancy, you could even make a notebook to store parameters like plate thickness and bend radius, so they are controlled in one place, rather than in each part.

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* Publish geometry is not strictly necessary, but it's usually a good idea to keep control over your references and communicate your design intent to others. In this case, however, your part is simple enough to skip it.

 

[plos]

That sounds right, thank you!  I just need to get Advanced Assembly extension to use the skeleton functionality.

[Pettersson]

Aye, therein lies the rub. I keep forgetting that this isn't part of the basic package.

[StephenW]

Creo does not do multi-body parts (like solidworks and NX).

In Creo, each part is a separate part file and then an assembly is used to put the parts together.