Stp file conversion to flat layout (sheetmetal)

a customer is supplying me with .stp files and i am not able to use the flat pattern feature in inventor to create a flat pattern. what is the process (procedure) for converting a folded up .stp file into a flat pattern?

base-cubby.zip

1. Open file.

2. Click Convert to Sheet Metal.

3. (the most often missed step) Set your Sheet Metal Style thickness to the same thickness as the part (in this case 1.2mm).

4. Click Flat Pattern

wow that was almost too easy ... that file worked just like you stated, but why wont this one do the same? its almost as if it imports it as a solid?

05-32135-000.zip

... its almost as if it imports it as a solid?

Uhmm, last time I touched a sheet metal part it is a solid. In fact, for it to work in Inventor - Inventor must see it as a solid.

I opened the file and Inventor placed the solid part in an assembly for some reason. Might be able to set some Options so that it didn't, but not worth the effort. Simply right clicked on the part node in the assembly browser and selected Open - then repeated the same steps as above. It was easy.

0.063 inch

1.60000000000122 mm

Well I was curious and changed some Options and this time it didn't place in assembly.

ok great! yes JD im a self taught newb but thanks to gurus like you ill be getting better everyday. thanks for your help! it was just a matter of learning the navigation really... and thanks for showing me how to get just the part and unfold properly.

Hey JD,

now my customer is sending .igs files... the approach for .stp files does not seem to work... any ideas?

21033114_ASM_1_1.zip

It imported as two solid bodies. Read this - http://home.pct.edu/~jmather/AU2008/ML205-1P%20Mather.pdf

ok i think i understood that. how was i supposed to separate the solids? how do i separate them currently?

You need to separate them into separate solid bodies before running flat pattern.

Either go to Manage tab>Make parts to push out the parts

or

Delete one and Save Copy as

Undo

Delete the other one and Save Copy as.

No tricks here.

do these settings look ok to you?

after import; they arent importing as two solids so how can i remove just one?

so this is after i did copy to construction, quality check, stitch, copy object (solid), and finished construction, then convert to sheet metal. shouldnt i see two solids? i can tell im just missing one or two details...

do these settings look ok to you?

No - you already know that it is more than one solid body.

Uncheck that Import assembly as single part.

You need for it to import as two solid bodies - Multiple Composite Features.

You should see a Base1 and a Base2 (two solid bodies) in the feature tree.

settings

feature tree after import. only one solid still

i got it. i changed the import option "levels (layers)" to "groups". and then i got my two solid bodies