This issue comes up at work fairly frequently. I usually just grin and
bear it, but thought I might save myself a great deal of time and
frustration by summarizing some of the more common issues I deal with
in taking customer models and designs.
Just a couple notes on these files.
When specifying feature locations in the flat, you are opening
yourself up to a lot of potetial problems. The material allowance you
use would have to match ours or the finished part will not meet your
requirements. Material allowance is determined by a combination of
factors: Material type, thickness and inside bend radius(IBR) are a
few of the main factors. Any deviation in the model from what will
actually occur with the part will translate into problems with the
finished part. It is far safer to dimension the finished part, rather
than the flat pattern. If we were fabricating the blanks for your shop
to bend, flats would be no problem. In short, convey what you want,
not how to fabricate it.
Ordinate dimensions are fast, clean and easy, but you can't convey
design intent with them. Parts that are made to print and are within
tolerance can actually be bad be bad parts. I'd be happy to provide
some examples of this if you like. Any deviation in any of the factors
determining material allowance will result in a tolerance stack-up
Locating features in the flat with ordinate dimensions compounds the
potential for producing parts that will not work as intended. Parts
dimensioned in such a way that mate to other parts dimensioned in the
same manner is almost assuring that there will be problems.
Inside bend radii should be as near to or greater than material
thickness in aluminum. The specified .030 IBR in .100 material you
have request will likely result in stress cracks. Standard IBR for
aluminum are: .030, .060, .090, .125, .25. We can achieve virtually
any IBR if we 'cap' our punch, but bend consitency can become an
issue, so it is best to use these standard IBR.
When conveying profile dimensions, the most practical approach is to
dimension legs from outside intersecting faces. These dimensions are
clear and will not change if the IBR should deviate from nominal. It
provides an abslolute dimension without the abiguity that can result
from dimensioning tangency, flat run or radius centers.
I'll forward copies of the drawings after I modify them for your
appoval and as a means of illustrating what I'm attempting to convey
here. If I can be of assistance or answer any questions, don't
hesitate to call.
I guess I might mention that my intent in posting this to the group is
to solicit comments regarding validity of the above as well as to spew
my slant on the topic. Comments/corrections are welcome, but no fair
hammering for typos/grammar.... It was a first draft!
I can't resist amidst many heary laughs.
First of all grammar.
I percieve many cases of participles that be dangling there.
No, but really.
Fabricators: Need flat blanks to build anything.
Designers: Don't really care about flat blanks.
Fabricators: Must pay people to program laser/turret.
Designers: Need a better price.
Fabricators: Must pass on cost of programming.
Designers: Always get bothered about the cost of NREs.
Fabricators: Should be smart about getting data when it is available.
Designers: Should share their best data with fabricators.
Fabricators: Know that you should form small tabs against the grain.
Designers: Think the grain is some sort of malt beverage or new rock
Fabricators: Are responsible for the final parts.
Designers: Are responsible for the ideas that create the product.
Fabricators: Are insane if they work to a designers flat without a
Both: Cannot achieve good anything from bad documentation
But seriously - definitely put a shear angle on the cutoff station,
and also keep the heat out of the die block during sharpening or we
might get those micro cracks again, maybe you need to wet grind this
one . . .
Oh yes and also don't forget to alway use solidworks to design your
parts. And if you fabricate parts designed with solidworks, you need
to get a license too so you can control your own form radii and
developements - remember the flat is free if you have the model . . .
If solidworks is not available just get out your t-square (don't
forget to spin you pencil so the lines are even) and do a 100x blow up
of the form radius drawing the neutral axis (use radians they are
"neater")in and then use one of those map wheel tracers to determine
the length . . .
email@example.com (d) wrote in
If you listen to Sean A you'll be in good shape. I just wanted to stress
one point. Don't fall prey to the people who tell you that the flat
pattern has no value. It's true that if you don't use the right numbers
for allowances, you get so much scrap, so get the fab folks to give you the
numbers they work with and do a couple of tests. In the end it will save
the designer money and the fabber time. And you just might learn
something, I know I did.
I work with a bunch of guys that are in the happy situation of having all
the design and fab under the same roof. They use the SW flat pattern daily
with very good results.
Another way to look at it is to provide the formed views showing the
critical formed dimensions. The flat pattern can then be ordinate
dimensioned and used to show details that don't change with the forming. Be
sure to keep tolerance stackups in mind.
Another advantage to providing the flat pattern is that if you are working
with a particular fabricator, and your flat pattern generation is
consistent, then they can determine what allowances to make for material and
bends based on your flat. This helps them in that they don't have to figure
everything, just mostly consistently modify as necessary.
Another advantage to providing the flat is that you, the designer, get to
look at it, and a lot of the time you realize that a small design change can
make the flat simpler & cheaper to make. Keep in mind, laser time is
generally charged by the number of pierces and by the inches (or mm) of
travel. Take a good look at the flat to see if it can be optimized.
That's the situation we are in, design and fabrication are under the same
roof. We worked closely with the Sheet Metal department to get the correct
k-factor nailed down for the tooling and material gages we use. I'd say on
average our sheet metal fabrication can be held to +/-.015 across bends most
of the time (16-10ga).
We just shoot them a flat-pattern DXF for the laser, and 2D drawing for
forming. The parts can get programmed in about 5mins, and within a few
hours (if production is slow) I can have my parts in hand.