AnsweredAssumed Answered

K factor and flat pattern length

Question asked by Matthew Theakstone on Jan 17, 2016
Latest reply on Jan 21, 2016 by Bernie Daraz

Like • Show 0 Likes0
Comment • 21

Hi,

Recently at worked we have started in house fabrication, as such our k factors need changing to suit our press brake. However, after doing test pieces the flat pattern length is still not correct. All flat lengths are correct for one bend but not multiple bends.

I modelled a part with 4 bends and the flat length is 4mm too short. To gain this extra 4mm the k factor needs to be set to 0.7, does this seem right? I thought k factor should be 0.25-0.5 due to extending ratio etc etc. I've never needed to calculate k factors, and attempted to use bend deductions but with little sucess, any advice

Dennis Dohogne Jan 18, 2016 4:46 PM

Correct Answer

K-factors can be very accurate, assuming you use good data. The biggest mistake I have seen is assuming values for material thicknesses and bend radii instead of measuring them. The attached pdf explains K-factors and how to calculate them and the attached spreadsheet makes the calcs easy. We went so far as to measure coupons bent with each gauge and bend radius combination and then created a table of K-factors specifically for our shop.

See the reply in context

1 person had this question

Outcomes

21 Replies

Bernie Daraz Jan 17, 2016 5:32 PM
Mark Correct
Correct Answer
I used Bend Deductions most often, simply take a piece of sheet metal of known length, accurately measured of course. Set up your press brake for the bend and keeping notes, top die radius, bottom die width, actual material thickness and grain direction. For the moment lets say you test blank is 5.250 long, again accurately measured. Now place a bend of any convenient length into your test piece.

Measure the sum of your bends and subtract your original flat blank length. The remainder is your bend deduction.
Like • Show 1 Like1
Actions
- Matthew Theakstone @ Bernie Daraz on Jan 18, 2016 12:34 PM
  Mark Correct
  Correct Answer
  Hi Bernie, I've seen some of your previous answers to other
  discussions which were most helpful, and I have indeed done these test
  pieces. in fact I've done them for all our material thicknesses. e.g
  
  99.7 flat pattern length
  90 degree bend
  radius of 2.5
  outside length 1 52.6mm
  outside length 2 52.86mm
  avg length 52.71
  material thickness 3mm
  
  fpl=outside length 1+outside length 2-BD
  BD=outside length 1+outside length 2-fpl
  BD=52.6+52.86-99.7
  BD=5.76
  
  2*outside setback-bend deduction
  (6.03*2)-5.76
  BA=6.3
  
  K factor I get is 0.5
  
  but when on solidworks this one bend comes out 0.5mm too short.
  The bend allowance comes out the same
  But bend deduction gives the length of 52.7mm.
  However, I've now tested this with a piece of 5mm and the bend deduction gives a length that is 6mm too long. The math was done the same, I used 3 test pieces and took averages when calculating the bend deduction.
  
  The tooling remains the same , we only have one set at the moment so that can't be a factor.
  Like • Show 0 Likes0
  Actions
  - Bernie Daraz @ Matthew Theakstone on Jan 18, 2016 8:47 PM
    Mark Correct
    Correct Answer
    Matthew,
    If you're doing the test bends to obtain the actual bend deduction just use them in SolidWorks? I mean you have a tested and proven result to base your blank from. My bend charts are based on tested and reviewed bend deductions, they were sometimes updated when material thickness was lighter or heavier. I would never use the term 'average' is describing a sheet metal function. I am of course referring to precision sheet metal. Ii seems as you're doing plate but everything should work the same.
    Like • Show 0 Likes0
    Actions
Anna Wood Jan 18, 2016 1:37 AM
Mark Correct
Correct Answer
You need to reverse engineer (calculate) your bend deductions. Material type, thickness, grain direction, air or coined form, tooling, etc will affect your bend deductions.

Google Olaf Diegel BendWorks

He has a great little program call BendWorks to help with calculating bend deductions and a pdf that explains sheet metal forming.

His original website is no longer active, but his material has been shared on a few other sites.

There are also all kinds of info on brake press forming to be found searching on Google.
Like • Show 0 Likes0
Actions
- Matthew Theakstone @ Anna Wood on Jan 18, 2016 12:34 PM
  Mark Correct
  Correct Answer
  Thanks Anna, very useful pdf, its nice to have all the info in one place and in metric.
  Like • Show 0 Likes0
  Actions
Tateos Tvapanyan Jan 18, 2016 4:04 AM
Mark Correct
Correct Answer
Hi Matthew,

Sometimes such a big difference come from the radius. Check the bend radius. Does it match designed radius?
Like • Show 0 Likes0
Actions
- Matthew Theakstone @ Tateos Tvapanyan on Jan 18, 2016 12:34 PM
  Mark Correct
  Correct Answer
  Tateos, the radius was wrong, though by about 0.5mm, I had been using the chart on the press brake rather than measuring as we had no radius gauges thanks for the tip, I had heard it could be considered (relatively) negligible.
  
  Thankyou all very much for your advice so far.
  Like • Show 0 Likes0
  Actions
  - Tateos Tvapanyan @ Matthew Theakstone on Jan 19, 2016 4:02 AM
    Mark Correct
    Correct Answer
    Matthew,
    It depends on sheet thickness.
    
    BA=pi(R + KT) A/180
    
    BA = bend allowance
    R = inside bend radius
    K = K-Factor, which is t / T
    T = material thickness
    t = distance from inside face to neutral sheet
    A = bend angle in degrees (the angle through which the material is bent)
    
    If the design radius is 5mm and produced is 5.5mm, sheet thickness is 5mm, and the K factor is 0.35, the difference for one 90deg. bend will be rough 0.8mm.
    
    For four bends it will be 3.2mm.
    
    So it's not negligible.
    Like • Show 0 Likes0
    Actions
Dennis Dohogne Jan 18, 2016 4:46 PM
Unmark Correct
Correct Answer
K-factors can be very accurate, assuming you use good data. The biggest mistake I have seen is assuming values for material thicknesses and bend radii instead of measuring them. The attached pdf explains K-factors and how to calculate them and the attached spreadsheet makes the calcs easy. We went so far as to measure coupons bent with each gauge and bend radius combination and then created a table of K-factors specifically for our shop.
Attachments
- K-Factor Development.xls38.0 KB
- K-Factor Development.PDF49.1 KB
Like • Show 1 Like1
Actions
- Matthew Theakstone @ Dennis Dohogne on Jan 19, 2016 4:29 PM
  Mark Correct
  Correct Answer
  If the sheets aren't the correct gauge (which i know they're not always) does this mean you check when a new delivery of sheet metal enters the workshop, or do you simply order metal from the same company which brings some more consistency to the quality.
  Radius gauge is being delivered tomorrow so i think that will have been my downfall.
  Like • Show 0 Likes0
  Actions
  - Dennis Dohogne @ Matthew Theakstone on Jan 19, 2016 5:27 PM
    Mark Correct
    Correct Answer
    The sheet thickness was the biggest wrong assumption we had been making. We usually only used one supplier, but if there was a change we would recheck. We also checked all the thicknesses every six months just so we weren't caught with our pants down. The supplier might change their source and not tell us. Also, the thickness was so important that the thickness was one of the first things we'd check if a problem arose (and it or a wrong tool was usually the problem). Your SWX parts have to be modeled with the actual sheet thickness so you have to know what that is.
    
    We setup spreadsheets in SWX with the decimal value of the materials. Dropdown selections are nice. If you get it really well setup you can select the material thickness and the inside bend radius and have it show the K-factor for that combination. Depending on how precise you want to be you could even specify the grain direction as this does have a very small effect on the bending. (We did some coupons of the same thickness and bend radius bent with the grain and across the grain. The difference in the K-factor was on the order of <=.01 so we didn't bother with grain direction.) We'd list the material thickness on the drawing in decimal form, but only reference the gauge in parentheses.
    
    Our sheet metal designs in SWX got pretty involved, with some parts having as many as ten bends. We used SWX for developing all the flat patterns and bend locations and were never happier. Since we had SWX and had learned how to use it for making accurate sheet metal and flat patterns we didn't need any third-party software.
    Like • Show 1 Like1
    Actions
  - Pete Peters @ Matthew Theakstone on Jan 20, 2016 8:41 AM
    Mark Correct
    Correct Answer
    Matt,
    
    My company was working with a ~1/4 tolerance when I came on board.
    They do not do high tolerance sheetmetal.
    We buy mostly from the same vendor.
    Once the time is spent creating a sheetmetal part, we move on and don't invest any more major time.
    I've got them working down into the 1/16 to 1/32 tolerance range now.
    We don't worry about actual sheet thickness and only use nominals in our K-Factor calcs.
    I don't even want to think of the nightmare a variable thickness would cause for drawing iteration.
    Our biggest problem is supplying a 0.000 tolerance Folder with 0.00 tolerance burned flats.
    Our Fasti spits out the Flat Length after programming and our Go / No Go range is +- 0.040.
    We really need a laser or waterjet, but only have high-def plasma tables.
    Like • Show 0 Likes0
    Actions
Bob Van Dick Jan 18, 2016 6:26 PM
Mark Correct
Correct Answer
Matthew,

If you cannot get bend deductions to work, you are doing something wrong. Is it perhaps your flat pattern calculation is off? At our shop, we have a standard bend deduction table we use that works for most parts. There are always exceptions to the rule and after awhile you get to know when it is a good idea to get a bend sample when creating a flat pattern for a new part. If you are the designer/engineer, you really need not worry about figuring the flat pattern length. Whether in house or subcontracted, typically the NC programmer will develop the flat pattern because he knows what bend deductions need to be used for a give material, thickness, and bend radius at their particular shop with their brake tooling.

Bob
Like • Show 0 Likes0
Actions
- Matthew Theakstone @ Bob Van Dick on Jan 19, 2016 7:47 AM
  Mark Correct
  Correct Answer
  Well in this instance I am the designer, engineer, as well as the plasma operator and press brake user. Although I have experience of sheet metal, I've never (or my boss) had to link the drawings to get the flat pattern length. The subcontractors gave us k-factors to use and that was it. If the NC programmer develops the flat pattern do you mean he simply changes these bend deduction values using solidworks, or is it more common to have a separate software package, like Autopol?
  AutoPOL - Software solutions for the Sheet Metal industry
  Like • Show 0 Likes0
  Actions
  - Bob Van Dick @ Matthew Theakstone on Jan 19, 2016 9:48 AM
    Mark Correct
    Correct Answer
    Matthew,
    
    No, I use SolidWorks. Perhaps the problem you are having is changing the bend radius on the actual flanges in SolidWorks to match the tooling you are going to use at the press brake. That isn't really necessary. You just need to use the correct bend deduction you will see at the brakes. If you start changing the bend radiuses on the flanges themselves in SolidWorks after the fact, it could (depending on the flange position used) change the length of the flanges and perhaps that is where your problem could be. When modeling a formed part in SolidWorks, I typically use a .0005 radius for the flanges. Many of our parts are welded and this allows for tight corners. The bend deduction I will end up using will be based on the material, thickness, and radius of the brake tooling used. What I am trying to say is that the radius in the model doesn't have to match the radius of the formed part for the bend deduction to give you a correct flat size. When unfolding a customers model, I don't change any bend radiuses in their models, I just plug in the bend deduction that I know our brake area will require to get the part to form to the correct dimensions. Some engineers will use the "bend outside" flange position, if you change the bend radius, the flange length will change. Maybe that is what was your original problem was.
    
    Bob
    Like • Show 2 Likes2
    Actions
  - Tateos Tvapanyan @ Matthew Theakstone on Jan 19, 2016 10:34 AM
    Mark Correct
    Correct Answer
    I think that will be helpful.
    
    SheetMetal.Me
    Like • Show 0 Likes0
    Actions
  - Pete Peters @ Matthew Theakstone on Jan 19, 2016 11:20 AM
    Mark Correct
    Correct Answer
    This was our month+ long process setting up a Fasti Folding Machine using SW2012:
    
    * Record data directly to plate with sharpie.
    
    1. Cut six K-Factor Plates per gauge, per material, per IR: Inside Radius. (20140107... attachment, pay attention to yellow sticky notes on pages 1 & 2)
    2. * Measure EACH K-Factor Plate in the FLAT (Granite Surface Block & Digital Height Gauge)
    3. Fold K-Factor Plates (90 Deg)
    4. * Measure EACH IR with Radius Gauges OR BETTER preferred method.
    
    Note: we only have ONE IR per gauge with our folder tooling. A bottom X Die, on a Brake Press, will give you multiple IR's.
    All this data gathering must be performed on each INDIVIDUAL IR per gauge.
    Having a single IR per gauge makes our data set quite small.
    
    5. * Measure EACH K-Factor Plate in the FOLD (Granite Surface Block & Digital Height Gauge)
    6. Capture each gauge group in a photograph. (20140410... attachment)
    7. Transfer & crunch all photo data into an Excel spreadsheet. (20150326... attachment)
    8. Copy and rename this file: C:\Program Files\SolidWorks Corp 2013\SolidWorks\lang\english\Sheet Metal Gauge Tables\k-factor inches sample.xls
    
    I suggest a format like BIA_K-Factor_HRPO_Steel_Rev-D.XLS. (BIA: Blast-it-all, HRPO: Hot Rolled Pickled in Oil)
    Store it in a custom folder like D:\UserPete\Documents\000_SW13Custom\SheetMetalGaugeTablesBIA.
    Delete, replace, add, subtract data in this XLS file with the data you crunched in step 7. (BIA-K-Factor... attachment)
    Note: in your parts add a -D14G suffix to your Sheet-Metal feature. (D: Gauge Table Rev, 14G: 14 Gauge)
    This is the only way I have come up with to keep track of the Gauge Table Revision and material gauge.
    
    You've got to do hands-on K-factor testing on the specific piece of shop equipment.
    Then use the resulting crunched data in Excel to calibrate SolidWorks to that machine.
    
    This is what finally worked for us, but my gut tells me you should instead be calibrating your machine to SW.
    I don't have ANY clue how to accomplish this in that reverse way.
    
    Note: This "data" will not work for any other machine but mine, so don't even try to use it.
    
    Pete
    Attachments
    BIA_K-Factor_HRPO_Steel_Rev-D.xls34.0 KB
    20150326_BendWorks_K-Factor_Rev-C-D.xlsx24.1 KB
    20140410_K-FactorPlatePictures_18GThru7G.pdf671.7 KB
    20140107_FastiKFactor90180_V02_DownRez.pdf1.4 MB
    Like • Show 0 Likes0
    Actions
    - Matthew Theakstone @ Pete Peters on Jan 19, 2016 4:29 PM
      Mark Correct
      Correct Answer
      Thanks very much for this step by step approach.
      A month! boss expects this done by tomorrow however, i am down to just 1mm error over 4 bends, and radius gauges will be here tomorrow which i hope will eliminate that error. The sheet metal gauge tables will just fill out the boxes for radius and k factor rather than me having to look at the list or try to remember them, yes?
      Like • Show 0 Likes0
      Actions
      - Pete Peters @ Matthew Theakstone on Jan 19, 2016 4:53 PM
        Mark Correct
        Correct Answer
        The Fasti has a graphical programming interface where you draw the profile section view of the part.
        You then add the leg length and angle values into the table below the graphic.
        It then spits out the OALL length of the flat.
        None of the drawings I put out of SW would be anywhere close to that number, so it was worthless to even try and fold it.
        It was an exhaustive quest for knowledge and then self teaching through fire.
        My equipment manufacturer could only teach his equipment and my VAR could only teach SW.
        I had to learn the middle and it was just like a baby learning to speak.
        My brain had to fill up with all that data until it flashed over and understood what I needed to do.
        It will take what it takes and you can't shortcut or rush it.
        
        Yes you will get a drop-list with all your radii to choose from.
        SW will then open up Excel to extract the required K-Factor data from the gauge table.
        K-factor droplist will say something like "Table Values" I think.
        Hard to recall without actually looking at it live.
        Make sure to add the suffix to your Sheet Metal feature.
        In your case it will be -A"GaugeNum"G.
        Like • Show 0 Likes0
        Actions
        Matthew Theakstone @ Pete Peters on Jan 21, 2016 11:39 AM
        Mark Correct
        Correct Answer
        Ok, I am now getting my bends for 3mm plate to within 0.5 mm from 20 to 90 degrees. However, my 50 degree bend seems to want a negative bend deduction (e.g an addition). part is attached what bend deduction would you guys use for this?
        Attachments
        50 degree 3mm.SLDPRT.zip127.4 KB
        Like • Show 0 Likes0
        Actions
Bernie Daraz Jan 21, 2016 8:04 PM
Mark Correct
Correct Answer
Matthew,
I used your numbers and my Excel sheet popped up with this.
Like • Show 1 Like1
Actions

Incoming Links

Re: Sheet metal bend deduction tables for flat development.

K factor and flat pattern length

Outcomes

Attachments

Attachments

Attachments

Related Content

Recommended Content

Incoming Links