Minimum Bending Radius for a given thickness of sheet metal

Hi, seem to be a lot of knowledgeable people here re: sheet metal
bending.
Can somebody please give me a formula that will give a minimum inside
bend radius for a given thickness of sheet metal and a given K factor?

Sorry if I am covering "done" material but I have searched google and
nobody seem to have asked this question.


thanks

Steve

 

For the sheet metal we do here, mostly around 1mm thickness, we use inside
radius of 0, and k factor of 0. It makes it easier to deal with on corners.

Otherwise, I have often heard of a default inside radius equal to the
thickness. No idea of the k factor, but it sure depends on your bending
method and tooling.

HIH
JM

 

I found that most of the specs I examined for HSLA steel include a
specification for minimum bend radius, in terms of thickness.

Most mild steels, minimum bend is 1x thickness. HSLA's (high-strength
low alloy) typically are 1.5x thickness. There are some exceptions,
depending on your application. Thin gage work tends to go to near-zero
creases.

Also, there is some dependence on processes. If you are bending with a
prog die vs. brake press, you have the option of coining bends and
getting tighter and more accurate bends.

K-factors are sometimes published in steel specs, but most die-builders
I've known have their own secret recipies based on alloys, press force,
bend radii, etc. Good guesstimate values typically around 0.35 for
mild steel and 0.45 for harder grades.

 

Seems to largely depend on the material being bent. The .100" 4130N
that I use tends to crack and weaken at anything sharper than a .100"
radius, however the same thickness domex material ( both have very similar
mechanical properties but differ in chemistry ), bends just fine at a .030"
radius. The sheet metal shop that we use was more than happy to share their
bending information with us, so that I could integrate the information into
flat pattern generation. The files that I've given them recently have
required no re-work on their part. They cut the solidworks generated flat
pattern and bend on its bend lines. Parts have been suprisingly accurate on
first articles and almost none have needed adjustment.

One thing to watch, however, is that different software seems to have
different compensation values. If I use bend deduction/allowance SW applies
them differently than the sheet metal shops software. They have two
packages that generate numbers that are different than each other. Using
K-factor have generated the same compensation values across all three
platforms so is what I use.

 

Do a web search for

"minimum bend radius" & sheetmetal | "sheet metal"

For some general info try searching for

"sheet metal fabrication" or some such.

One that sticks in my memory - www.sheetmetaldesign.com

 

Thankyou very much for your replies. You solved my problem.
I am doing some picture card holders and I decided to use sheet metal
with @1mm thickness. From your answers, it seems that getting a fold
with near zero inside radius should be no problem.

Thanks again Steve

 

Last place I was at did alot of sheet metal bending with brake press.
Material was mostly mild steel 1.5 to 6 mm

Generally we found that it was quite dependent on what V die the press brake
operator was using.
If he forgot to change V die to a narrower size when going down to a thinner
plate, things would turn to custard!

From memory 3mm plate used 25 wide V die - that gave an internal radius of
about 1.5mm.
If operator used the correct minimum width V die, called up by brake press
manufacturer, we found that about 0.5 thickness for inside radius used to be
a rule of thumb.
K factor we used for this was about 0.1.
Our flat patterns used to fold up quite nicely with these settings.