best kfactor

I have started work for a small company producing sheet metal products, and
have talked them round to getting a solidworks seat. I will be doing most of
the drawing and in the past I have had at my disposal tried and tested bend
tables etc, but now we will have nothing other than what I have in my head
and my rule of thumb type stuff. anyway what I ask is what is the best
kfactor for use on LVD press. at the mo I am using .445 and that sort of
matches some of my old bend data but I am not 100% confident when issuing
jobs to be cut and folded. I have also used inside sizes + 1/3rd of the
gauge but seems pointless with the 3d systems

Thanks in advance

 

Hi Julian
we used amada here, all we did was contct them and they provoded us
with the bend deduction data which we feed straight into solidworks.
You could try for a 10mm V on mild steel.
0.8 thk 1.8 bend deduction
1.0 thk 2.05 bend deduction
1.2 thk 2.3 bend deduction
1.5 thk 2.65 bend deduction

I'd also suggest you contact LVD http://www.lvdgroup.com/ and get them
to tell you the correct bend deductions for their machines.
regards
Ken
http://kenneth.carpenter.googlepages.com/solidworksusersuk

 

thanks Ken will look them up

 

We use a k factor of .445 for press brake work, whether bottom bending
or air bending. For a folding machine you need to get some more data as
the results of bending differ slightly.

For press brakes, you do need to know whether you are bottoming or air
bending to set the inside radius you are modelling. Bottoming should
match the top punch radius, down to a minimum of 63% of the material
thickness. Air bending we figure .156 times the width of the bottom
die, in mild steel. Aluminum and other soft metal follows the punch a
little closer.

Stamping bend radii and k-factors are a different animal again.

Diego

 

We've found that .446 works great for ferrous steels (cold & hot rolled) and
3000-5000 series aluminum. We use .365 for stainless steels. But it all
depends on what the 'finish' bend radius is. If you model with a .060 bend
radius and the brake operators actually get a .090 bend radius on the part
then your part will not be correct depending on available tolerance. We use
Trumpf press brakes here and we only have tools with 2 radii which makes it
easier but you have to remember that when you are air bending the bottom
die opening has as much to do with the 'finish' bend radius as the radius on
the punch. It gets complicated when you are trying to hold +/- .005 on a
sheet metal parts with 8 bends!

Hope this helps,
Jeff