sheetmetal, flat patterns, bend allowances

We are having a heck of a time getting flat patterns to come out correct. It
seems like everyone in the shop has some kind of different formula to
achievee a correct part. When the guy does the programming thru metalsoft
manually, we have few patterns. But when we use a flat pattern from
solidworks (created by sheetmetal, flanges, etc.) everything comes out way
off. It isnt even close to what it should be. We tried the tables right out
of the machinest manual for the material and size. BAD PARTS. We tried
punching in the numbers the guys in the shop use. BAD PARTS. We tried using
what the Metalsoft programmer uses. BAD PARTS. We need to get this flat
pattern to the point where we dont have to go thru the extra steps of
another person redrawing it in a nother program. Any ideas where we are
failing. I had a part today with 13 90 degree bends. It came out over 1" off
from the machine???? Thanks for all the help anyone can give. Jake Barron

 

o.k., good ol' bob z. has no actual sheet metal experience, but your post
has bob z. troubled. very troubled.
is/was there any consistency between all of the parts coming off of the
machine that were designed to the different formulae? for example, if you
created the part in swx using the machinery's handbook and then created
the same part using the shop dude's criteria, did these two finished
off-the-machine parts have the same error? bob z. knows this sounds a
little obvious, but it sounds like the problem really needs to be
simplified. ya know? take out some of the variables. pick a formula and
stick with it till you get it to work.
bob z. would probably pick the formula that the shop dudes use. why? ya
gotta be friendly with them guys!

o.k., bob z.'s post sure didn't help you in anyway, but maybe... maybe...
it'll help somebody.

bob z.
p.s. curse this dreaded alcohol addiction!

 

what method bend table, k-factor, bend allowance or bend deduction are you
using to calculate the flat?

bend table & bend deduction work well, results are very predictable. bend
tables are nothing more than a list of bend deductions for varing radii &
material thicknesses. the table will interpolate for angles other than 90.
hth

 

When the guy does the programming thru metalsoft
Do you mean few "problems' ? Or he just doesnt get much work done?

I've done my flat patterns both (and more) ways; including using
MetalSoft (Fabriwin)

I soon discovered that to allow my Solidworks Flats to come out the
way they
they were being done manually, I had to change my K-Factor to .28.

Why? Because a .28 K Factor, using a bend radius equal to the stock
thickness, returns the same valuse as the Bend Radius on 90 degree
bends! Somehow they thought/think that doing a second equation of
adding a fudge factor to the
pseudo-bend allowance was saving time.

Example: .125 stock. .125 Bend radius, 90 degree bend,
..28 K Factor = .125 bend allowance

If this is what's being done on your shop floor, and there is no
chance of
convincing them to do it correctly, then update your models
accordingly :/

Another thing you may want to check is that the correct SIDE of the
base face is checked. Inside vs outside allowance can make all the
difference.

Thirdly, I dont use the OLE in Fabriwin to import a Flat Pattern from
an open SolidWorks model.... 'things' happen to it. I export my flats
from a SWX drawing.. either to DXF, or directly to metalSoft .prt
format.

MetalSoft uses a low precision internally... and while 6 decimal
places may seem fine in sheet metal, thats also only 6 decimal places
using 'Pi' and any trig...
Round off errors show up often in arcs and non-orthagonal lines.

 

I use the OLE in fabriwin all the time, sometimes I have had problems with
lines that were smaller than .001 modeling errors. I have also had problems
with parts that have both new and old sheetmetal features. It supressed
everything between the new flatpatern feature and the old features. I
remedy this by making a mirrored part since the mirror of a flatpattern is
just cutting from the other side. I tried to submit that to their
development team and they always say it will be fixed in the next release
but it never happens. SW has a much better system of getting releases fixed
beleive it or not than any other software I have dealt with.

We always use close to .5 K factor but in our shop they say if it is within
..25" it is good. So I never know how close it actually is.

Corey

 

All we do here is sheet metal for pizza ovens. Stainless steel 20 thru 12
gage. Darn tough stuff to work with. The material properties vary from
middle of the sheet to one edge, etc. We had to 'discover' the inside radii
and K factors based on our tools. For instance we use K = .41 and inside
radii = 1/16" for our Safan (dang nice machine) press brake loaded with
Wilson Euro tooling (also nice) for the 18 gage stock. It took a little
trial and error to get this, and we usually can hold +/- 0.015" or better.
Operator, machine setup, and technique probably has more to do with holding
close tolerances. There are a million variables besides the software.
Solidworks has been a real time saver for me, and its sheetmetal
capabilities was the primary reason I bought it to begin with.

Gary

 

You need to have your sheetmetal guys do some 90 degree test bends to
determine what the bend deduction of the material is that you are
working with. For example, where I used to work, #4 SS 16 Ga. had a
bend deduction of .110. We determined this number by bending up some
test pieces and finding out how much the material stretched. This
number will change depending on material, dies and even the brake. So
a 1"x1" L-shaped part needs to have a flat length of 1.89. You
subtract .110 for every bend in the part.

So we simply put that .110 into a bend table and the parts came out
nails. We had different bend tables for each different material. We
only had one brake, so we didn't have to account for different tools.
The use of a bend table allows SolidWorks to calculate angle other
than 90 degrees

 

WE DO A LOT OF SHEET METAL WORK!
And have only recently discovered that the bend radius has nothing to do
with the top tooling, but the bottom v block!
If you send me your email address, I will send you our formulas for 1mm to
4mm sheets.
this ensures that the notching is also correct when using the bend deduction
option.