Flat patterns from simple curved sufaces

[jderou]

Their has to be software that can do this. I have a sheet metal part that looks like the picture below. It is a simple curve which could be closely defined by 3 or 4 radii. I need to make a flat pattern. Solidworks sheet metal functions won't do it, its too complex. What I have to do is offset the inner surface to the neutral axis, convert to a .dwg, open in autocad, then manually figure out the arc lengths and convert them to straight lines, figure out the distance to holes, etc. very time consuming!
It seems like I should be able to take a surface that is offset to the neutral axis, and flatten it out. Seems simple (though it may not be), makes me want to reach into the monitor and smash the surface flat.
Does anyone have software that can do this?? Or is their an easier way?

Thanks,

Joe

[JerryFlyGuy]

Joe, is it possible to post the file? It's tough to see it in a picture and know the geometry. SolidWorks should be able to flaten a simple part such as this, there might be some simple issue that needs resolving.

Jerry

[jderou]

Here you are, you can suppress all the operations. It is an imported solid btw, from catia.

One problem is their are no flat surfaces to select for the sheet metal feature. I tried adding a flat surface off the bottom edge but it said the geometry was too complex to flatten.

Joe

[JerryFlyGuy]

Well Joe, I'm kinda slow and that was for sure a difficult part to get through but I did get you a flat pattern. As close as I can tell it's correct. The issue w/ the part is simply [we two things] first of all in SW, it hasn't been converted so its just a 'dummy' part. It has no inteligence built in [it doesn't know that its a sheet metal part, it only knows it's a really thin, curved part. So I had to extrapolate the curve of the part, extruded a new sheet metal pc that matched the curve, then I coverted the edges and cut out the shape, followed by cutting the holes. What I found was that solidworks still didn't know which edge to use for a flat pattern. [Flat pattern works the same way as if you used the 'flatten' function and picked an edge or surface to use as a base point] So I had to add one on the end. I made it 0.010 off the end and used it as my base edge. Flattening it out still gave me some greif [I still have an error] but it did do the flatten. I've attached the dwg of the pattern here.

HTH
Jerry

[DareBee]

Good job Jerry

Been there done that.

Imported items always have to be converted to be of any use.
I have also had the *um* pleasure of figuring out to make a cheater flat on curved parts for flattening.
It has been a few years and I had forgotten - thanks for the reminder.

[JerryFlyGuy]

Aw shucks , it took me a few goes to figure out that the completly curved end's was causing the problem. I could extrude a sheet metal pc which was curved to match the same curve as the part and it would flatten out just fine, cut it to the profile and it just wouldn't work..
twas a moment..

Jerry

[DareBee]

sometimes things click and sometimes they don't.

We can't be possibly be the best at everything - can we?

[JerryFlyGuy]

You said it!

Jerry

[jderou]

I actually attempted to do the same thing. I re-created the curved surface with a flat on one end, then I made trim surfaces from the original leaving a flat tab on the bottom. For some reason by the time I trimmed it, solidworks said it was too complex to unfold. So I went ahead and did it manually, cause I needed it done. I laid my results on top of yours, the results are pretty similar, except for some of the holes (mine is the green lines). I haven't checked which one is right, but hopefully its mine cause the parts are already made!! heh.
What version solidworks are you using BTW? I'm still on '06.

Joe

[JerryFlyGuy]

Strange eh? I looked at the dwg, it would appear that yours is correct and I've got a mirroring error in mine. Good catch. I'd hate to be responsible for you cutting a part w/ a error in it!

Sorry about that!
Jerry