Deform area on a Thread forming punch in sheetmetal

This one got me too. Seems difficult to thin the material in Sheetmetal for the pierce and extrude. I ended up making the part outside of Sheetmetal. I'm sure there is a way, but every feature wanted to maintain the material thickness. Since this is not the case with the pierce (it thins as it extrudes), it mattered to me.

Personally, I model that I see. So when I place these kinds of features, I also want to see them. It is too easy to overlook this at a higher level design review and suddenly you find yourself with an interference in the real parts.

Some tips with regard to this in Sheetmetal would be helpful indeed.

Hmmm, guess I'll try to replace this feature with a regular Pro/E formed feature and see if I can get anywhere close. This is geometry that has been translated from another tool. I'm not sure if there was a flat pattern for it before, but I'm pretty sure we'll have to have it in the future.

I know at the TC's, we have discussed with PTC about introducing manufacturing features that produce variable thickness (deep drawing, plastic deformation, etc.), but the technology just wasn't readily available.

Thanks for the feedback Antonius and Brian. It's good to have some validation.

Today I had a great opportunity to see how this could best be done. Indeed, there are some -serious- limitations to making features part of the base material in Sheetmetal.

1st I tried the Inheritance Features. I could not get anything to merge with the base sheetmetal part. So I thought, "great, I can make Sheetmetal PEMS and use the as Inheritance features..." NOT. Make a pierce and extrude sheetmetal part and "merge"... NOT The ladder could be inherited but you could not join it to the main model.

So I have never used Form features, until today. Mind you, I am using Creo 2.0 and I have done some sheetmetal model types with good success.

I looked at Joshua's linked model and the 1st thing I noticed is that it doesn't have the "1st wall" feature. This is key to beginning any sheetmetal model. Second, What am I missing here... I cannot see any history in release M030(?) (tools/investigate/model history; we've discussed this before). Lastly, I cannot see any features as they are created from Pattern 9 (unpattern\ungroup) only when the Solidify is applied to I see anything.

So on one of my Creo 2.0 sheetmetal parts I use the "half shear" tutorial to help me learn about form features. I successfully make it work and find I can easily make the feature represented in the initial post. So I do that; reduce the OD if the extruded wall (made with the form feature); add fillet radii to the inside base and the outside thread hole; next apply a cosmetic thread. I do all this in an "unbend" state. I reactivate the Bend Back and the feature moves with the wall as expected.

So a form feature seems to do what you want. You can do more operations to that form feature that are more core feature operations. If you have a lot of these to do, you'll find that they do not pattern, necessarily.

The moral of the story, always generate a "1st wall" feature be it planer or revolve. And create this after the initial datum features.

I had an issue where a guy had tried to do something in sheetmetal and it almost worked, but I couldn't modify it at ALL. Like Brian said, once you pick a thickness you're done. I think sheetmetal should be an optional package, with the commands inside regular Pro/E, so if you did some sheetmetal part, and then machined some other area, or if you wanted something like sheetmetal (because you needed both folded and flat patterns) but it would in fact be an IM plast part (with bosses, which is impossible in sheetmetal). For me, since I needed a flat state, a state where just the leads were bent, and when the leads and the flex circuit was bent, I ended up having to do my part as a family table assembly of family table parts that all had spinal bend features in it to get what I needed. Something so simple ends up being so difficult......