Using ID's on sheetmetal parts

My brake operators prefer to use ALL inside dimensions when forming a
part with no specified radii. I can't figure out how to get solidworks
to recognize this. The closest I've come to achieving my goal is to
specify a .0001 default radius, and a k factor of 0. I run into
problems with this on some thicker parts when solidworks HAS to put a
bend radius in it. My flat layouts always come up with bogus
dimensions (at least according to the brake operators) and creates some
major headaches for me, and them.
Is there a bend table I should be using for A36 ms plate? Am I missing
something? I haven't seen any other threads addressing this problem.

Thank you,
Chad

 

Chad,
Unless you are using some really strange A36, then you have to put in a
realistic bend factor. You should also specify a radius, unless
consistent and repeatable parts are not needed. A 0.4 k factor would be
a good place to start. Your specified bend radius is going to depend on
what size die they are using, assuming they are air bending the part.
1.25*thickness is a good place to start. Once you get your k-factor
dialed in and the radius correct, the flat pattern should be correct.
I have a excel spreadsheet with different material and bend radii that I
could send to you if needed.
Brian

 

I'm a bit confused as all bending operations will involve a radius of some
size, unless you get into coining, which I don't think is your issue. My
suggestion is to determine what the K-factor is of the current operations
and then use those values. To test it, shear out a piece of the material,
measure it accurately, bend it, and the measure it again. That way you will
know what the bending process is producing.

WT

 

I should have been more specific, sorry about that. We have a 500 ton
Cincinatti hydraulic press brake with v bottom dies. The issues I
speak of for example, when I form a Channel shape out of lets say .25
material thickness the brake operators want only Inside dimensions,
i.e. 5" flange with 2" legs (inside dimensions) the brake operators
want exactly 9" of material, no more, no less, and this is the way
we've always done it, and it serves us well. However, solidworks wants
to make it a little more or a little less depending on bend radii and
bend allowance.
I hope this helps clear some things up...

Thank you,
Chad

 

It's just a matter of picking the correct bend radius and k-factor. For
1/4" material, try k-factor = .4, inside radius = .366

 

Chadli,

Use Bend Deduction and set it to 0. This will produce the results you
are looking for.

 

Awesome Brian, that worked great! Is there a bend table allowance I
should be using to get these figures on a consistent basis? Or is is
pretty much a guessing game?

 

Dave I tried this, and yes, it does work, sometimes, with a default
radius to .0001 or somewhere around there, however it has a hard time
bending and unbending some of the thicker metals that require a larger
radius.

 

Chadli,

Please send me one of the parts you are having a problem with.
dherb_ma_n_@ho_tmail.com
^^REMOVE UNDERSCORES^^

I'm guessing the issue is related to bend relief or edges intersecting
the bend region. I double checked by creating a sheet metal angle with
2"x2" legs and setting Bend Deduction to 0, then mucking around with
the variables.

Material Thickness: .375
IBR: .375
Flat pattern= 4"

Material Thickness: .375
IBR: .0001
Flat pattern= 4"


Material Thickness: .5
IBR: .5
Flat pattern= 4"