Design and Manufacturing solutions through Digital Prototyping and Interoperability

Sheet Metal | K-factor

K-factor; what is it, and why does it matter to me? Design & Motion is all about digital prototyping. For digital prototypes to be most effective, what we produce digitally (in the form of models and drawings) needs to represent the finished product as closely as possible. In my experience, the area of manufacturing where this need for accuracy seems to be most neglected, is in sheet metal design. For applications where sheet metal components do require tight dimensional tolerances, too often I hear the blame game where the fabricator tells me the designer always gets the blanks wrong, and the designer tells me that the fabricator can’t fold his parts accurately. In a lot of these situations, neither the fabricator nor the designer has a good understanding of where the error comes from.

Folded

With modern CAD tools, the ability to unfold a complex sheet metal shape to produce a blank is all too easy. The problem with it, is because the blank looks correct, many designers assume that it is, without taking into account the fact that software has been set with a default value that is used to calculate how the material changes in length when it is folded. The folded component will only be dimensionally correct if the blank is also correct. There are many methods for quantifying the amount of material to allow for a fold, but in my opinion, the easiest and most efficient one to use relates to a magic number called K-factor.

You’ll remember from Mechanics 101, that when a material is placed in a “bending” scenario, the top surface of the material goes into compression, and the bottom surface is stressed under tension. Between the two extreme surfaces, there is a gradual change from compression to tension, with a plane right in the centre that is neither in tension or compression. This is often called the neutral axis. When we take this bending to the extreme and actually push the material beyond elastic limit, like we do when folding sheet metal, the plane that is under the least amount of stress is not actually always in the center of the thickness of the material. Exactly where it lies depends on a number of factors such as the type of material, how “tightly” you are folding it etc. For any given bending scenario, the neutral axis of the material will lie somewhere between the inner surface of the bend and exactly half of the thickness of the material. We can quantify exactly where it lies by expressing it as a percentage of the thickness of the material. We call this the K-factor. So for a very large radius bend where the neutral axis lies right in the center of the material, the K-factor would be exactly 0.5, or half the thickness.

kFactor

Most CAD systems that have sheet metal design tools will allow you to input a K-factor that the software uses to calculate the unfolding to give an accurate blank, or flat pattern. This is all well and good, but how do you know what K-factor to put into the software? Well the easiest and best way to do this, is to perform a bend test for a particular scenario, and then back-calculate the K-factor from measurement data. To make this easier, we have come up with a handy K-factor calculator for you to use. Just follow these simple steps and it will spit out a K-factor for you to input into your CAD tool.

Angle

1. Cut a blank to a specific length (say 100mm) and measure it as accurately as possible.

2. Mark a fold line exactly in the center.

3. Configure the press or other folding tool with your desired tooling and make a 90 degree fold on the bend line.

4. Measure the outside lengths of both legs of the fold and input them into the calculator as well as the inside bend radius (this can be measured with a radius gauge.)

5. The calculator will give you the K-factor. Make sure you record the details of the tooling used, material thickness, and material type that correspond with this particular K-factor.

Flat Pattern

If this method is used, you will find that your CAD software will produce incredibly accurate blanks and your folded components should turn out spot on.

For Autodesk Inventor users, I recommend that you set up multiple sheet metal styles for each bending scenario and name them to include the tooling and material details (eg 1.5mm Aluminium – 16mm Vee) and set the K-factor for each one after performing a bend test and calculation. This way, when you create a new part, you can simply select the style that you want and know that your K-factor is set correctly.

K-factor calculator

Here’s to accurate blanks!

update:

Multi-body sheet metal enhancements in Autodesk Inventor 2016

  • aaktas

    Great solution for k factor problem! thanks a lot. I have tried it and works great. However if there’s 2 folds (please check attached picture). how should I dimension the second fold. The reason that I ask that question is the dimensions of folds in an unfolding draw are between the bend axises. So, after the operator makes the first fold, how is he going to position the machine for the second fold? (The thickness of metarial should be added the dimension of second fold?)

  • erazorzedge

    @ aaktas

    When setting up the machine for two bends, you first have to figure out the difference between the dimension from edge of part to first bend line and edge of part to the inside bend intersection after forming. The difference plus (or minus) the thickness, plus the dimension between the two bend lines (in the flat) is what the backgauge should be set at on a press brake.

    For instance, I have a two 90° bends in a piece of 14ga S.S. (thickness = 0.075″) using a 0.500″ v-die opening. From edge of part to the first bend line is 0.931″. The calculated I.D. should be equal to 0.925″ (based on results from bend tests). The difference between these two values is equal to 0.006″. Now add that to the thickness and you get 0.081″. In the flat pattern, the distance from the first bend line to the second bend line is 1.838″. We now add 0.081″ to 1.838″ and 1.919″ is the dimension to set the backgauge to on the press brake.

  • Gavin Bath

    The point here, is that if the software is calibrated to give accurate flat patterns and bend positioning, based on real-world geometry that you used to do the calcs, then you can simply measure and mark the bend lines on the flat pattern and fold on those lines.

Join the Community