SolidWorks 2005 help needed - Sheetmetal

Anybody running 2005 SolidWorks and are familiar with the sheetmetal functions? I have four books on SolidWorks, plus the online tutorial, and all of them use simple boxes with 90º sides as examples. I can do that easy enough, but if I apply the same exact methods and sequences on a box with angled sides, it isn't at all happy with me. The method all my reference material suggests is to make a solid the correct shape, then rip the corners and insert bends. When I insert bends, it comes up with an error that says, "Attempt to add auto-relief failed. Could not create a bend with the given radius. Please try a different radius or add reliefs."

I've tried bend radii from zero through .750" (nominal being 1/16") with no effect, and I can't find how to add reliefs by any other means that the auto-relief function, with which I've tried numerous shapes and ratio's with no luck.

This is an 18ga mild steel part that I would really like to have to our laser/forming shop on Monday. If any of you would like to see the file, I'd be more than happy to email it to you as a solid.

As a note, I've been trying all this without the 'tail' and the flange...my thinking is that it would be easier to add those two features later.

Thanks for any help guys.

are you sure you are allowed to have the sides closed like that when trying to flatten?

I rip the edges first, if that's what you're talking about. If not, can you please elaborate?

It works on mine, but it's 2006. No flanges, extrude, draft, shell, rip, and then convert to sheetmetal with obround reliefs. It wouldn't work with a tear. It works with the rips one way or both. Doesn't seem to care if I rip first, or while doing the conversion.

Thanks Wes. I tried it again, following the exact sequence you said and it still comes up with the same errors.

When you say "convert to sheetmetal", you're talking about the 'insert bends' function, right?

Insert bends is something you do by drawing sketch lines on the piece. It's quite different from convert to sheetmetal.


Chris P

I beg to differ, if we're both talking about 2005 anyway. What you're refering to is called "sketched bends".

However, if you're familar enough with SolidWorks to feel compelled to jump in this thread, would you care to offer some help?

Yeah, 'insert bends'. I tried shelling the bottom, and the 'tail' end, to leave the other 3 faces. Works fine, but when I add the 4th wall it won't put any relief other than a tear in it no matter what I select. That will let me add the wall with straight sides, but if I angle them out parallel with the other faces it bonks.

It also didn't like trying to rip across the flange, gave me a geometry too complex error.

Your best bet might be to model it in sheet metal. I usually create the base flange with the corner reliefs modeled in, rather than let the system insert them with the bends. I think that may be your only choice with these angled walls anyway.

The other thing that 'fixes', is to let you create the walls to the proper length so the bottom flanges are all on the same plane. If you just stick them on the edges created by the shell and conversion, if you ever get it to do that for you, they'll be at different levels and will require fiddling with offsets to get them where they need to be.

I've got the model here looking about like what you posted. If you give me dimensions I can finish it up and send you an IGES. Let me know what you want to do where the flanges intersect at the corners and I'll see if I can fix that.

Thanks a bunch for the effort Wes, it's definetely appreciated. I understand what you're telling me to do except for modelling the reliefs in a base flange. Do you just extrude cut those?

Incedently, one of the people I asked for help was one of the laser shop's employees, and he got it finished within 15 minutes (bastard!), but he's also running 2006, and as you probably know, if I get an IGES file, there's no information included in it that gives me any instruction....just a solid. Damn solidworks for making everybody update every year just so they can still communicate.

So Wes, it's not necessary for you to keep putting time into this unless you want to. The base measures 8.000" x 12.500", not including the 'tail'. The tail end and two sides are at 10º, and the front end is at 30º. The tail face is 10" from top to bottom, and goes straight after the flange. The flange is .750" wide around three sides, and it really doesn't matter how it's split at the corners, although 45ºs would be nice.

That's good news. By coincidence, I modeled mine at 10 and 30°.

I got in the habit of putting corner reliefs in the first feature I extruded. I never liked the notch cuts Pro-E and SW always put in, and by making it myself I can control what I have. I got tired of playing with the various settings and never being satisfied.

I start with mat'l thickness, plus bend radius and a little. Depending on the angle of the bend you might be able to tweak that down.

Another thing I've done with odd angle parts, when I can't get what I want, is to model the part, flatten it, and get dimensions off it. Then use those to model a flat piece and bend it from there.

Yes I was confusing it with sketched bends. I never use the convert from solid because our vendors don't like or have much to do with the shapes rips produce.

This is also my point about Solidworks "Sheetmetal" - there are things that confuse it and the algorithms blow up.

Given the speed of creating shaped tabs with Solidworks, I'd say go that way in future so you have control over the bend reliefs. Different sheet metal suppliers have different tool selections and so you need good control.

Chris P