unfolding sheet metal part

We are messing around with unfolding sheet metal parts. One problem we are
encountering is that the unfolded parts are not workable. The stretch that
happen during bending is different from what Solidworks calculates. we
have used different bend allowance table and k facters ... but still the
bend allowance/ stretch are off. Usually when we calculate stretch at the
shop for stainless steel we use 1.6 X thickness and that give us a very
accurate stretch. Where can we find info on how to get Solidworks to unfold
with the correct stretch/bend allowance?

 

SolidWorks Help, look into K-Factor.

If you do a lot of in-house sheet metal fab, you might want to experiment
with 12"x2" strips bent into C or Z shapes, adjusting the K-factor until it
matches your processes and tooling.

 

Have you tried bend allowance. If you start with a bend allowance of 0 and
your parts are .25 short change the bend allowance to .25 and if you have to
go the other way use bend deduction. You have allot more flexibility
because you aren't using percentages with the limit of 0 to 1 I think if
you want to do it right you have to set up a bend allowance or bend
deduction table to adjust for different angles.

Corey

Look up "bend allowance" in the SW help it shows a diagram of how it is
calculated.

 

the only way to be sure is to set up solidworks to exactly replicate the
beding process you use. Air bending, coining, bottoming all produce
different results, so be sure to use the exact same process for these
tests as you will on the real parts

set up the press with the same bottom V and the same top tool as you will
for the real parts. Take a say, 100mm piece of strip and VERY carefully
measure the exact external dimesion, note it down. Now, Bend it roughly
in the middle. Measure the two external faces and not them down.

Now you should have two figures for the external surfaces of the 100mm
piece you bent .. say 54.2 and 51.5mm ... make up a solidworks
sheetmetal part with those exact same external dimensions .. unfold it to a flat
pattern and add a dimension to the overall length .. it *should* be 100mm
.... but it wont be just yet.


be sure to set up both the bend radius AND the K factor in the part, they
will be wrong by defualt, and the solidowrks documents are wrong about
how to set it up too. teh radius is NOT the radius of the top tool in air
bending (the most common form of bending these days) it is (roughly)
1/6th of the V width you use for the bend.

So ... you should now neasure the inner bend radius of your part ... but
if you start with a K factor of say 0.4 and a bend radius of 1/6th of
the V width you used to bend it, you should be close. You may find for
stainless you get a K factor closer to 0.3

I recommend you read:
http://www.massey.ac.nz/~odiegel/bendworks/bending.pdf

a most excellent treatment of the subject.

Once you do get solidowrks
set up right (I have macros that run through an assembly, find the
sheetparts and set the K factor and bend radius based on the material, to
save me the trouble) it produces very accurate bends. I can usually
expect to be +-0.2mm on 3~6mm mild steel plate.