Frame generator notching/unfolding issues

[sailah]

Hi,

Please forgive my rookie status here, just learning Inventor 2014.  I have gotten the basics and am looking to draw up a mtorcycle frame based on dimensions I have in the shop.  I'm just playing around at this point and sketched a trellis frame and used 3/4" ANSI pipe for the tubes.  In reality I will be using 1" DOM 0.065" wall tubing.

  I notched a couple of the tubes and can isolate/open those individual parts.  I have (tried to) follow a couple tutorials on how to "unfold" or rip the notched tube so that I can print out a template, wrap it around the tube and cut/cope it in the shop.

I keep getting an error message saying it can't rip it.  Now I drew a tube myself in another part file just by extruding a couple circles and it ripped that just fine, and would unfold it.

Is it the ANSI profile I am using from CC?  Is it because it is notched?

To be honest I couldn't follow the steps in the following http://forums.autodesk.com/t5/Inventor-General/Unfold-a-tube/td-p/3168764

I tried to thicken the part, fail haha.  I'm not sure what I should be doing here.  I can thicken it fine, but then I can't "delete face solid lump"

Again, sorry about the beginner question I'm really starting from the bottom here

[JDMather]

Check the attached fix.

You Sculpted the surface bodies into a second solid body for the Combine-Subtract.
Inventor sheet metal does not support multi-body solids - thus the error.

I deleted your Sculpt and deleted the extra surface faces you had. (When Copy Object to get the surface - you only need the outer contact surface).

Now I used Sculpt (or Split) to cut away the excess without creating an solid bodies).

[jeffsteiger6735]

I realize this is an old thread, and I've found some newer ones, but this one seems to have the best information. But I'll be damned if I can get it to work on my particular part. The Rip command never seems to work, just errors with "unable to rip". Split does the trick, but thats where I get stopped. I cannot unfold and flattening just makes another round pipe.

I've made a very thin thickened surface as I need to make a paper cut out of this once done, like this video https://www.youtube.com/watch?v=KoOfekvSVsA, but I get stalled after picking the round face as my stationary reference, I have no option to select anything after that.

Part attached.

[johnsonshiue]

Hi! This can be done easily. The Thickness value on the part is different than the actual body thickness. Please try the following and Rip should work.

Option 1: Go to Manage -> Styles Editor -> Sheet Metal Rule -> change the thickness to 0.05mm (the body thickness d27).

Option2: Go to Sheet Metal Default -> uncheck "Use Sheet Metal Rule" and change the thickness value to 0.05mm or d27.

Many thanks!