Just checking - lofted bends

Just wanted to confirm what I am seeing - can we only have one lofted
bend per sheetmetal part? Nothing about that limitation in the help
(or in the nesgroup search I just skimmed), but lofted bends is greyed
out in both 2006 and 2007 after I start a part with lofted bends.

 

To the best of my knowledge, you are correct. One lofted bend per part,
which is crap if you ask me...

 

Also be aware that any flat patterns derived from a lofted bend are
probably wrong.

 

Well that sucks big time.
We requested lofted bend development because we use it all the time in the
aerospace industry, there aren't many straight lines in an aircraft.

Unfortunately most parts in a wing have 2 lofted bends ie an upper and lower
wing surface to mate up with.

Looks like we will be moving over to Catia a lot quicker than envisaged.

 

because we use it all the time

But you are just now becoming aware of this limitation?

It would be cool to see the flat pattern process for a one piece rib, joggles
fore and aft. I've always wondered how the real people do it.

 

What about the F-117? ;-)

 

No they're not. I've been using the lofted bend in a quite a few sheet metal
parts and it's worked out perfect everytime for me.

 

I've ehard htat lofted bends weren't that accurate, but everything I
was going to do was flats and cones so it should unfold withotu having
to do any apporximations. I might try to loft it and then add bends
(old sheetmetal), but as you know it can take quite a bit of setup for
a loft to make a true cone - you can't be off the slightest bit (or
take the slightest shortcut) or the deals off.

 

The amount of error depends on the amount of non-Gaussian (compound)
curvature in the bend. If your bends do not have a lot of non-gaussian
curvature, then the amount of introduced error will be less, perhaps
not enough to matter.

One die maker I worked with simply does not accept flat patterns for
compound-curved parts. He insists on developing his own, since
CAD-developed (SW and Pro/E) flats for compund curvature are invariably
flawed.

 

You've heard all the words and are getting close. Gaussian curvature greater
than 0 indicates compound curvature. The analysis necessary to predict the
exact behavior of the material is outside the scope of a mechanical CAD
software.

What is that supposed to mean? What's the process and application? Is it going
to bother you if the length of a contoured flange on a bag pressed rib or frame
isn't created to machine part tolerances? How far off will a SW or ProE flat
pattern be for that part?

 

Is creating the part outside the sheet metal environment then converting to sm
an option?

 

Yes - that's my next avenue.
But as I understand it you have to be very careful on how the lofts are
set up so the resultant model is all cones, cylinders, or planes. The
way to check if you actually made a cone or cylinder (vs an algorithmic
face) is to select the face as a reference for an axis. To check if a
face is planar, click on it and see if you the sketch icon is greyed
out or if it is available.

 

But as I understand it you have to be

Is that the criteria or can it be expanded to include all developable surfaces;
i.e. an extruded conic arc or spline?

Is a Gaussian curvature analysis available to help determine if a surface is
developable if the criteria can be expanded?

I'm not a SW user, or a brandX shill. Just a curious net nerd, so please excuse
me if the questions are irrelevent to the topic.

 

SolidWorks does not have a check for Gaussian curvature. Unigraphics
has had Gaussian curvature analysis since at least 1996. This was very
useful, as I used to have the task of putting decals on odd surfaces.

 

As far as I know, the criteria for unfolding a model to which
sheetmetal is applied are as I posted.

Thanks for being frank - that's appreciated. I don't think the
question is irrelevant because it speaks to the wider need to flatten
complex shapes. Swx is still not able to do any of the things youb
rought up (at least as far as I know - I try not to say SWx can't do
soemthing because it will suprise you at times. I just doubt that it
will surpise us in this case)

Ed

 

Thanks for the info, folks.

 

We do a lot of conical sheet metal and use the usual sheet metal tools
to generate the flat patterns and this works just fine. Occasionally
we have to generate a flat pattern for an offset cone and need to use
the lofted bend feature for this. We found the flat patterns for the
lofted bend cones were not accurate at all so we tried a little test.
We made a standard sheet metal cone and the same part with a lofted
bend. The two flat patterns are not even close! What we found is that
the "k" value for lofted bends are not used. If you model the lofted
bend with the outer surface the flat pattern reflects the geometry of
the outer surface rather than the neutral axis (i.e. k=0.5). Same
thing if you create your model using the inner surface, the flat
pattern reflects the geometry of the inner surface, not the neutral
axis. The work around for us was to model the part using the neutral
axis and this gave the correct flat pattern. Unfortunetly the part
itself is not correct as you can not do a "mid plane" lofted bend so we
ended up with two configurations of the part, one for the correct part
geometry and one for the correct flat pattern. Our parts use
relatively thick steel plate such as 3/8" or 1/2" which can create a
considerable error in the lofted bend flat pattern unless we create the
geometry on the neutral axis. Try a flat pattern of a simple sheet
metal cone with both tools and a relatively thick wall thickness and
you will see the problem. Has any of this changed in SW2007, we are
still on SW2005 SP5.

Ed