Sheetmetal Bending & k-Factor

Quite often I hear Inventor users saying: “the folded part didn’t come out like it was in the model, I even gave them a flat pattern!” The flat pattern feature in Inventor is near useless if you don’t have the sheetmetal style set correctly to suit material, tooling and processes used to form the part. k-Factor is a useful number that when used along with a correct bend radius can give sheetmetal flat patterns that will fold up very accurately. “So how do I work out this magic k-Factor?” you ask. The easiest and most accurate way to do this is:

  1. Cut out a rectangle of material that you want to fold, say 100mm x 50mm. Measure accurately, and record, length and thickness.
  2. Mark a bendline across the centre of the rectangle and form a 90 degree fold with a press-brake or whatever you are using to do your folding.
  3. Measure, with a vernier caliper, the length of each side and record these (I’ve called them “Leg 1 Length” and “Leg 2 Length”
  4. Measure and record, using a radius gauge, the Inside bend radius.
  5. Plug these numbers into the calculator I’ve created here, and voilĂ , you have your k-Factor to put into your sheetmetal style in inventor.

To check your result, create a sheetmetal style in inventor that has the measured bend radius, k-Factor (from the calculator), and measured thickness, and create a sheetmetal part using this style. Sketch a rectangle, create a face from it, put another sketch line across it in the center, create a 90 degree bend and using the measure command, compare it with your real sample. They should be pretty close. If not, maybe your bend radius is not quite right as it’s a very difficult thing to measure accurately. You can fine tune the k-Factor if necessary.

Note that you will need to repeat this process any time you change material, thickness, tooling etc.

8 Responses to “Sheetmetal Bending & k-Factor”

  1. David Colbourne says:

    You can also work backwards from your spread sheet.

    The fabricator will know the bend allowance ( or deduction) that works for them

    The fabricators I use will give me a bend allowance (deduction) for a given material / thickness – i.e. No bend allowance for Stainless Steel & 0.6mm for a 90 deg bend in 2.0mm Mild Steel. I set the Radius to be equal to the thickness.

    The 2.0mm Stainless Steel Blank will be 96mm to give 50mm legs and a 0.27K factor ( I use 0.27324)

    The 2.0mm Mild Steel Blak will be 96.6mm to give 50mm legs & 0.46 K factor ( I use 0.46425)

    I’ve been using these K factors & bend radi like this since Inventor 10 and have not had a problem.

  2. Muikku says:

    thank you this is handy

  3. Doug says:

    Do you mind sharing the actual algebra that the calculator uses?

  4. Lyle Swartout says:

    Ok I calculated a bend factor using knac a excel tool and by hand all using the same input did this a half dozen times Knacs kfactor = .81 my other excel tool=.40 and by hand=.41 Whats the deal?
    Here is my input
    12ga .1046 thk
    75 deg bend
    My tooling =.1376 bend radius
    leg 1 = 1.067419
    leg 2 = 1.567419
    2.5 blank length
    These are imperial units not metric
    could it be this is metric

  5. admin says:

    Hi Lyle,

    Sorry, it is a metric calculator. I’ll have a look at the code again sometime and see if I can Americanize it.

  6. admin says:

    Sure, I’ll try and find the same reference I used.

  7. admin says:

    Hi Doug,

    The formula I used for the bend allowance is: L= 2 Pi A (R+KT) / 360
    Where L is the arc length of the bend on the neutral axis (bend allowance)
    T is the material thickness
    A is the angle of bend (I used 90 degrees)
    R is the inside bend radius
    K is the k-factor (re-arrange the formula to solve for K)

    You can calculate the bend allowance from the blank length, leg lengths and inside bend radius (from test sample) and then use that data to plug into your rearranged formula to get K.

  8. admin says:

    Hi David,

    Yes, lots of Inventor users use these “rule of thumb” type methods and get the k-factor by trial and error to match the specified bend allowance, but the point here is if you need to be really precise (we would often work to +/- 0.1mm on the width of a folded channel for example), then you can use this method to calculate the k-factor very accurately from a bend sample.

Leave a Reply