Jump to content

Properly Setting Up K-factor In Sheet-metal


ramsay

Recommended Posts

Does anyone know how to set-up k-factor for sheet-metal every time i draw a sheet-metal component in solidworks the flat-development always come out to big when i form it on a press-brake.

Iam using the de-fault setting k-factor 0.50

BOX.jpg

Link to comment
Share on other sites

A bend table setup is ideal, but K-factor is what we use here.

 

In our case, we used a known bend allowance to figure out what the blank *should* be, and did some trial and error to get the K-factor that gave us that blank size.

 

You'll have a K-factor for each material/bend radius.

 

For example, our 14-13ga parts are formed w/a 3/32" radius. The bend allowance we use for 14ga is .156. We ended up w/a K-factor of .291.

 

I have an Excel spreadsheet that I put together w/the gauge, K-factor, our standard radius and bend allowance as well as distance(s) to bend lines from either an edge or another bend line. If your allowance for 14ga is close and you'd like a copy as a place to start, PM me an email addy and I'd be happy to send you a copy.

 

If you need an aluminum reference, we bend .125 w/a .125 radius and a bend allowance of .22. That gives us a K-factor of .44.

 

Basically, the initial setup is something of a hassle and takes some time but once you've got it figured out it's handy. Someday, when I have lots of time and many minions, I'll have time to actually hash out a good, working bend table that we can use automatically. But till then, the K-factor calculations have served us well.

Link to comment
Share on other sites

one thing you can also do(if you are using SW09) is draw your part as a solid block then you can convert it to sheet metal selecting your base and bends. it will let you compensate to the inside or outside.

 

You do this by going to Insert>Sheet Metal>Convert To Sheetmetal.

 

Select your base, your 4 bend edges and enter the rest of your parameters.

 

Here is a screen shot. I set my materail thickness to 5mm, bend radius to 5mm and i set the auto relief to Tear and the Gap to .1mm. When I flatten the sheet i get 285.71 with a 2.5mm radius and 283.56 with a 5mm radius. Playing around with kfactor on sheet metal pieces i couldnt really tell a difference in the model. I just setup my bend radius and my flange position where they need to be and roll with it.

 

I would like to figure out a more accurate way of modeling sheet pieces but the tolerances for my pieces just dont warrant it(yet).

sheethelp.jpg

Link to comment
Share on other sites

You can do the same with older versions actually- I'm not sure the rip functionality is there or as good as I don't use it often, but when sheet metal was first added you had to create the solid first and then convert to sheet metal. It's something I still use, in particular when I have an existing part with a known good blank that needs to go into SolidWorks. It's another way to model, but it does not solve the issue of getting a good blank, because SW only has the information it is given to do the calculation. Even if you don't enter the bend data when you rip it, you'd most likely have to edit it afterward.

 

I did a quick build with my usual settings out of .190 aluminum. We form it w/a .125 radius (3mm and change), and use a K-factor of .4814 for a bend allowance of .29".

 

I got a blank width of 283.906mm, and a notch that measured 25.9589. With your larger radius, your blank would be slightly smaller and it would put you close, I think, to your expected blank size of 280mm. This assumes: your *overall* size was 250mm, all 4 flanges created at the same time, with outer virtual sharp and material inside selected, length of 25mm.

 

Is any of this the kind of information you're looking for? :)

Link to comment
Share on other sites

Thanks for all the input guys yeah a k-factor spread sheet would be brillaint if possible in metric please.

ramsay458@hotmail.co.uk

With our press-brake in work for that box to fold to the dimenshions i drew it up with 250mm outside with 25mm outside flanges the development should only be around 280mm.

All my sheet-metal parts always come out to big just now so i need to try to find a solution to solve this just now iam manually adjusting it in our cad / cam software when programing it for the machines.

Link to comment
Share on other sites

Something interesting. I was working in Inventor 09 saturday morning doing some sheet metal design. I was working with .125 thick 3003 aluminum. Inventors preloaded kfactor for that material was .44. I havent had the chance to play around with other materials but that was the first sheet metal part i had done in inventor 09.

Link to comment
Share on other sites

Fixed the problem for some reason when drawing parts in sheet-metal if i use a bend allowance of 1.5 for various thickness the flat part development comes out pefect every time.

Link to comment
Share on other sites

Glad to hear it. :) I've gotten about halfway through the conversion of that table but we are less than half staffed this week so I haven't yet gotten to finish it. As soon as I do I will send it your way.

Link to comment
Share on other sites

  • 2 months later...
  • 3 weeks later...

I did a table for Solidworks' bend deduction settings by comparing the blanking size from Trumpf Tru Bend program and Solidworks ... The values i get seem to only apply if the item has less than 4 bends. I'm quite new with sheet metal, and the more senior guys in my office uses autocad.. having a pretty tough time getting the solidworks sheet metal parameters.

 

Also, we've got a Salvagnini machine in our factory, through observation, it seems like the bending allowances for this method of bending is different from press break's.

Link to comment
Share on other sites

  • 4 months later...
  • 2 weeks later...

im having the same problem, im drawing standard stuff in inventor and my blank size is just coming out big everytime, is there an easy fix or away to work out the k factor??

Link to comment
Share on other sites

  • 3 weeks later...
im having the same problem, im drawing standard stuff in inventor and my blank size is just coming out big everytime, is there an easy fix or away to work out the k factor??

 

 

i have the best solution.

We have a pressbrake from baykal, i make my flat pattern as follow:

 

1. draw sheet metal part in inventor.

2. in our pressbrake, make an 100x100 profile with desire thickness.

3. choose tooling in the program

4. read total flat length and bendradius, write them down.

5. using software "bendworks"(Free, google it). Use "reverse engineer k-factor

6. enter thickness, kfactor and bendradius on the part in inventor.

 

Now inventor and our pressbrake calculates flatlength equal. Now i just export the flat part to a dxf file, make cnc code for our waterjet and BAM..

 

It Works very very well, final part is always 0.3-0.1mm wrong. thats pretty good for me ;)

 

You could get flatlength and bendradius without the pressbrake, but for me its faster to "sync" the values i get from the pressbrake.

 

Enjoy

Link to comment
Share on other sites

btw, now when i program the same profile in the pressbrake, the gauges is always correct. no need to manually program it. This is very usefull on complex parts

Link to comment
Share on other sites

  • 10 months later...
  • 2 weeks later...

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.
Note: Your post will require moderator approval before it will be visible.

Guest
Unfortunately, your content contains terms that we do not allow. Please edit your content to remove the highlighted words below.
Reply to this topic...

×   Pasted as rich text.   Restore formatting

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

×
×
  • Create New...