1. Home
  2. Solidworks CAD Design software
  3. best kfactor

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

Reply to
Julian
Loading thread data ...

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 c> I have started work for a small company producing sheet metal products, and

Reply to
Ken Carpenter

thanks Ken will look them up

Reply to
Julian

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

Reply to
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

Reply to
Not Necessarily Me

=D1=87=D0=B5=D1=82=D0=B2=D0=B5=D1=80=D0=B3, 24 =D0=B0=D0=B2=D0=B3=D1=83=D1= =81=D1=82=D0=B0 2006=C2=A0=D0=B3., 14:59:33 UTC+4 =D0=BF=D0=BE=D0=BB=D1=8C= =D0=B7=D0=BE=D0=B2=D0=B0=D1=82=D0=B5=D0=BB=D1=8C Julian =D0=BD=D0=B0=D0=BF= =D0=B8=D1=81=D0=B0=D0=BB:

The best way is to use Cadman b3d LVD software. It "knows" K-factor and Ben= d deduction for all condition (tools, materials etc). Or you can use my own little XLS file that can calculate right K-factor fro= m know BA \BD. Also it can calculate theoretical k-factor from formula from= putted data (V size, thinkness, radius of punch, etc). snipped-for-privacy@gmail.com

Reply to
timur123

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.