Possible?

[Conrad_Turbo]

I created a solid part (to calculate volume), then shelled it and now want to unfold it. I want to create the base flange where the 4 holes are on the X-Y plane, then have the two identiacal pieces fold off of it, and have the remaining strip (surface on Y-Z plane, arc surface and surface on X-Y plane) fold off the base. Any idea on how to rip this shell apart?

See attached for the file.

[JerryFlyGuy]

A couple points.

1- You've got to ask yourself.. can I REALLY manufacture this?
2- If yes, would it not be easier to just weld that ~4" wide top section [curved] in rather than trying to break and form it all in 1 pc. I realise this is just a light 14ga pc of metal but.. it does beg the question..

3- All sheet metal sections which are curved like your top curve there, need to be tanget to some line at either end. [I've changed your model to reflect this]

4- Typically modeling in this process [what we call the 'old way'] is done the same and then it's 'ripped' to open the edges where we want to weld so that the box can be unfolded. In this case however w/ the curved wall and various other nuences it's much faster to just do two cuts which create 'rips' and they will also give you a much cleaner joint rather than a corner fillet. W/ a little flap disk sanding you'll have a nice sqr corner rather than an exposed fillet joint on the corner/edge.

Sheet metal is a fun tool to play w/. It takes a bit of testing and messing to get used to it.. in time it can be a very fast and powerfull tool.

Hth

J

[Conrad_Turbo]

Wow thank you for the great input! Now to answer your questions.

1- You've got to ask yourself.. can I REALLY manufacture this?
2- If yes, would it not be easier to just weld that ~4" wide top section [curved] in rather than trying to break and form it all in 1 pc. I realise this is just a light 14ga pc of metal but.. it does beg the question..

Yes. The only difference I would make to the model is to have the curved top section lay overtop the side panels. That way I can tack along the edge and have it maintain the proper shape. The only “bad” thing about the design is the dead space when having the part cut out from a sheet, due to the top section jutting out, when it could be a separate piece. Either way I am trying to design something with minimal welding and that could be quickly formed on a brake and then with some good clamping methods easily and quickly weld it up. I updated the model using your techniques but got a few errors. Mind taking a look? The only tearing I see occurring is near the far end of the manifold (away from the TB flange area).

3- All sheet metal sections which are curved like your top curve there, need to be tanget to some line at either end. [I've changed your model to reflect this]

I’m assuming that’s the big reason why I couldn’t rip it in the first place. I have done it with simple shapes, but never anything with a curve. Thanks for the heads up, I can see the 0.100” straight line you put in place to have the arc line up tangent with it.

4- Typically modeling in this process [what we call the 'old way'] is done the same and then it's 'ripped' to open the edges where we want to weld so that the box can be unfolded. In this case however w/ the curved wall and various other nuences it's much faster to just do two cuts which create 'rips' and they will also give you a much cleaner joint rather than a corner fillet. W/ a little flap disk sanding you'll have a nice sqr corner rather than an exposed fillet joint on the corner/edge.

I normally model from the “ground up” per se, however in this case I need to know the plenum volume to begin the design. Is there any way to measure the internal volume of a sheet metal part?

Actually an exposed corner fillet would be ideal since this would be TIG’ed and the aluminum weld won’t be ground down. However for other applications I agree with you, such as if it was stainless steel and was going to be flapper disc’d and sanded smooth.

Sheet metal is a fun tool to play w/. It takes a bit of testing and messing to get used to it.. in time it can be a very fast and powerfull tool.

It’s a very powerful tool, but for standard shapes it works very very well! When there are weird curves or shapes, then I do admit I tend to get stuck every once and a while.

[JerryFlyGuy]

Actually the dead space will/would be a none issue [pretty much anyway] if you get them profile cut, you just rotate every second pc 180deg and place them side by side.. they will dovetail pretty well.

If you expand the "Flatten-Bends5" you'll see those two errors at the bottom..

Right click the first one and select "Whats wrong?"

It tells you that the bend is no longer associated w/ anything.. you can suppress it..

Bascially this was an old bend that got removed w/ changes to the model. SW doesn't delete this [don't ask me why not, I think it has to do w/ legacy changes [reverting back if you changed back]] but keeps it in there. All you do is suppress it and it's gone..[Same for the errors in "Flat-pattern5"].

The only way to get rid of it [no big deal w/ this model] would be to delete the "Sheet-Metal5" feature [and all the attached features below it] and re-insert the "Insert Bends" function.. then those two wouldn't be there. However, if you had added 1/2 dozen new features after you'd made it a sheet metal part.. it'd not be worth putting all those back in there just to remove those two error notes.. At the end of the day, this is not nesc however as they have ZERO impact on your current model.. other than getting your heart rate up for a couple seconds while you figure out what went wrong.

Error proofing and solving is something you just have to learn by doing. I've been at this for ~8yrs, you get to the point where when someone asks you to make a change.. your already mentaly going through the model and calling out the errors it will cause, before you ever make the change..

Back in the day when I took my SW courses they actually had a part of the course on solving errors.. they'd give you a file w/ all kinds of errors in it and ask you to solve them all... it really wasn't as tough as it looked... and was a great learning experiance..

Hth

J