lvmckane Posted May 1, 2014 Share Posted May 1, 2014 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 Quote Link to comment Share on other sites More sharing options...
JD Mather Posted May 1, 2014 Share Posted May 1, 2014 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 Quote Link to comment Share on other sites More sharing options...
lvmckane Posted May 1, 2014 Author Share Posted May 1, 2014 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 Quote Link to comment Share on other sites More sharing options...
JD Mather Posted May 1, 2014 Share Posted May 1, 2014 ... 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. Quote Link to comment Share on other sites More sharing options...
lvmckane Posted May 1, 2014 Author Share Posted May 1, 2014 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. Quote Link to comment Share on other sites More sharing options...
lvmckane Posted May 6, 2014 Author Share Posted May 6, 2014 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 Quote Link to comment Share on other sites More sharing options...
JD Mather Posted May 6, 2014 Share Posted May 6, 2014 It imported as two solid bodies. Read this - http://home.pct.edu/~jmather/AU2008/ML205-1P%20Mather.pdf Quote Link to comment Share on other sites More sharing options...
lvmckane Posted May 6, 2014 Author Share Posted May 6, 2014 ok i think i understood that. how was i supposed to separate the solids? how do i separate them currently? Quote Link to comment Share on other sites More sharing options...
JD Mather Posted May 6, 2014 Share Posted May 6, 2014 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. Quote Link to comment Share on other sites More sharing options...
lvmckane Posted May 6, 2014 Author Share Posted May 6, 2014 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... Quote Link to comment Share on other sites More sharing options...
JD Mather Posted May 6, 2014 Share Posted May 6, 2014 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. Quote Link to comment Share on other sites More sharing options...
lvmckane Posted May 6, 2014 Author Share Posted May 6, 2014 settings feature tree after import. only one solid still Quote Link to comment Share on other sites More sharing options...
lvmckane Posted May 6, 2014 Author Share Posted May 6, 2014 i got it. i changed the import option "levels (layers)" to "groups". and then i got my two solid bodies Quote Link to comment Share on other sites More sharing options...
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