Solidworks - Lofted Bend Flat Pattern

[SimpleD]

Does anyone know how Solidworks determines the flat pattern length for a Lofted Bend? Or can anyone verify its validity? It doesn't seem to take any material properties or bend allowances into account. It doesn't seem to simply "unroll" the perimeter either. Somehow it depends on the thickness though. If I create a simple half cylinder and flatten it, the flat length ends up being something that I can't predict mathematically - using inner radius, outer radius, or neutral axis.

 

[TheTick]

Even if SW could flatten a lofted bend, I would doubt the pattern's validity. I've seen more than a few Pro/E users fall victim to improperly developed flats of non-gaussian (free-form) forms.

Unfolding non-gaussian geometry is a task fit for FEA-based specialty software. Many stamping toolmakers have such software.

We don't even make flat paaterns anymore. Even if we did, our toolmakers would just make their own.

"Great ideas need landing gear as well as wings."--C. D. Jackson

http://www.EsoxRepublic.com

 

[JNR]

We are talking about rolling again (look back in several recent threads) as opposed to bending. Bending can be analytical, but even then if you talk to any sheetmetal house many of them use tables. They may even vary from press to press! It depends on how accurate you need your sheetmetal (we have some parts with .010 tolerances round 2 or more bends). So how the algorthim for rolled or formed material is done is anyone's guess - it more of a stretching operation really, since the change occurs throughout the material, not just in a local bend region. You should be able to get data from an internet search - after all, they get from somewhere.

BTW: Why do you want to predict what SW is going to give you? Why not just measure the flat pattern? Is this a real requirement or just for you own amusement? I think the only way you could verify it would be to do a real test or ask the vendor to tell you what the flat pattern length should be for your part and compare. They must be able to figure it out since they do it all the time.

I suspect that in practice there may be some variation due to exact process or machine as with bending.

We have the luxury of not having to do flat pats. We just give the vendor the finished part drawing and let them figure it out - heck, they are the experts. The few formed parts we use are hyro-pressed.

I was - and he did. So at least I didn't get coal.....

 

[MElam]

SimpleD,

We have also had problems with the lofted bend and you're right, it does not take bend allowances, k-factors, etc. into consideration. I agree with the others that the shop guys should make thier own flats, but that is another battle. We have reported the issue and I suggest you do also.

If you must make the flat, here is the work-around we have found:
Modifying the initial sketch used to create the loft can solve the problem. If you take the thickness of the metal and multiply by the k-factor for that metal, and then add that number to the radius in the sketch, this should result in a correctly flattened part. An example would be a lofted 16-ga. stainless steel part with a 1/2" initial radius and .37 k-factor. Instead of the .5 for the radius, use [.5 + (.0598 x .37)], or .5221.
This works for our shops with our tooling (which is where the .37 came from)and an initial sketch which is an arc.

Of course this is a bad idea since it makes your formed part wrong. Create different configs so you can use the correct formed part where needed.

Michelle

 

[SimpleD]

JNR - Trust me, I wouldn't waste your time if this was my idea of amusement. "Why not just measure the flat pattern?" I have measured the flat pattern produced by SolidWorks and it doesn't make sense. I don't have a real part for comparison because it doesn't exist yet. The details of my project aren't as important as the basic need to understand how an engineering tool works before blindly using it, but I'll give some more info for the sake of brainstorming...

I need to design a complex 3D part that can be molded (yes molded) economically in the flat state and then ROLLED into the 3D form. The material in this case is not metal, but plastic and/or foam (therefore, no yeilding). If SolidWorks Sheetmetal doesn't even use material properties to flatten a Lofted Bend (unlike edge flanges, etc. where bend allowances seem to be taken into account), then I figure that I just might be able to apply the technique to non-metal materials. Even if it does somehow take material properties into account, such as bend allowances, then perhaps I can give it the right inputs to neglect yielding.

The reason that I can't use simple hand calcs to determine the flat shape is because the pattern is complex. It's not just a simple rectangular sheet formed into a cylinder. But if I could get Solidworks to unfold something that simple into a predictable flat pattern, then I might trust it to do a more complex shape.

Thanks.

 

[JNR]

Hmmm..... I see your problem. I have never used the SW unrolling tools in combat. I just assumed that it might give you a reasonably accurate result (well, in metal anyway). Silly me... I keep fogetting "assume" makes an ASS out of U and ME! You would think I would remember by now - got enough scars......

Forming plastic is a whole different ball of wax anyway as you say, so I don't think SW will probably ever get to that point. So your parts are flexible and do not remain in the formed state on their own - only in the assembled configuration? How about using a design table to edit the flat pat configuration using some Excel calcs? Maybe not if your shapes are pretty complex.

BTW: I suppose you know you can do anything Excel you want in a DT whether embedded or external. You just leave a blank column or row at the bottom or right edge of the DT proper and the rest of the worksheet is yours to mess with. So you can do data entry, links, calcs, even check-boxes, etc. and just link the results into the DT cells. Actually you can do calcs in the DT cells themselves, but I find it cleaner the other way if things get complex.

I was - and he did. So at least I didn't get coal.....
OK, OK, It's a reference to my holiday sig. "Be naughty - Save Santa a trip..."