Design Rules for Fabricated Metal Parts

If you need a metal part, cutting a blank and then bending it is often one of the most cost-effective manufacturing methods to make it.  OSH Cut offers both blank cutting and bending to make fabricated metal parts.

As with any manufacturing method, sheet metal bending has some limitations that should inform your design.  You should understand both how air bending works, and how your part should be designed to avoid problems during fab

 Our material catalog contains design rules for each bending material that we offer.  Below, we walk through how bending works, and how to understand the design rules published in our catalog.

1. What is Air Bending?

2. What is Minimum Flange Length?

3. What is the K-Factor?

4. What is the Bend Radius?

5. What are Bend Deductions?

6. What is Bend Allowance and Outside Setback?

7. What is the Maximum Box Depth?

8. What is the back gauge, and how does it affect bending capabilities?

1. What is Air Bending?

Air bending is a method of forming sheet metal using a punch and die.  In a part produced using air bending, the metal is placed between a punch and a V-die as shown below:

Punch, Die, and Bent Sheet Metal Part

As the press brake forces the punch and the die together, the metal folds where the punch makes contact with the part.  The part itself only touches the punch on the bend line, and the v-die on the edges.

 

2. What is Minimum Flange Length?

In a bent sheet-metal part, minimum flange length is the minimum distance from where the punch contacts the metal, to the edge of the part.  Because the part is bent as the punch compresses the part into the V-die, the V-die must remain in contact with the part for the duration of the bend.  If the V-die loses contact with the part, it will not bend properly, if at all.

Sheet metal minimum flange length

If there are internal cutouts that overlap the region where the punch or die meets the metal, it can cause the part to deform, as shown below:

sheet metal part with min flange length violation

Because the material does not make contact with the v-die in the above part, the metal does not bend properly.

 

3. What is the K-factor?

K-factor is the ratio between the "neutral axis" of a bent part and the thickness of the material.  The "neutral axis" is where the material doesn't elongate or compress during the bend.

For example, when you bend a metal part, the outside of the bend has to elongate, and the inside of the bend compresses.  Somewhere in the middle, the metal does neither.  This is what the k-factor defines.

Usually, you don't use k-factor directly.  If you use CAD software to model your bent part and create your flat pattern for manufacturing, you'll usually tell it the k-factor so that it knows how to unfold your part to create the flat pattern.  Combined with the material bend radius, the k-factor allows the computer to figure out exactly how your part will stretch during bending.  It will compensate for that when unfolding your part, so that the finished part is as close as possible to your design.

You can calculate deductions and offsets yourself, if you'd rather not use CAD.  But if the finished size of your part is important, we highly recommend that you use CAD software so that you are certain that your flat pattern and bend locations produce the part that you need.

Explanation of sheet metal bending parameters
 

4. What is the Bend Radius?

In a bent sheet-metal part, the Bend Radius is the radius of the bent metal where the punch meets the part.  In an air-bending process, exact 90 degree angles are not possible to manufacture.  There will always be a radius on the bend, as shown below:

Formed sheet metal parts require a bend radius

The bend radius depends on material properties and the size of the V-die gap used to bend the part.  Bend radius is smaller if a more narrow v-gap is used, at the expense of higher tonnage requirements to perform the bend, increased risk of stress cracks on the bend surface, and surface marking where the punch and die makes contact with the part.

At OSH Cut, we publish the bend radius that will be formed using our material and tooling in our material catalog.  We do not support customizable bend radii, but we selected common and optimal tooling so that if you design around our bend radii, you should be able to have your parts manufactured anywhere.

When you design your part in CAD, you can configure both the bend radius and k-factor to match our manufacturing processes, so that your finished part is as close as possible to the size you intend.

 

5. What are Bend Deductions?

In a bent sheet-metal part, the Bend Deduction is the amount the material will stretch when bending your part.  Because the material will stretch during the bend, the total length of the part - including the radiused area where the bend takes place - will be larger than the original flat pattern defined.

If you are creating your bent part in CAD, you usually do not have to worry about bend deductions: you can tell your software what k-factor and bend radius to use for the material, and it will automatically create the correct flat pattern size and bend locations so that the finished part size after bending matches your design.

If you are creating a flat pattern manually, you will either need to compute bend deductions, or use our app to obtain bend deduction and other information for your bend.  Bend deductions depend on the angle of the bend, but our app will tell you exactly what to use for a bend, like below:

Automatically compute bend parameters

For selected bends, our system will report the bend radius, bend allowance, bend deduction, outside setback, and k-factor.  You can use this data to manually modify your flat-pattern if you need to do so.  But again, sheet metal CAD is the best solution to ensure that your part is the correct size.

 

6. What is Bend Allowance and Outside Setback?

Bend Allowance is the length of the arc formed by the "neutral axis" of a bend.  During a bend, the outside of the material stretches, and the inside compresses.  Somewhere in the middle, the material does neither: the length of that region is the bend allowance length.  See the picture below.

When your bend angle is 90 degrees, Outside Setback is the distance between the start of the bend radius, and the edge of the flange (see the picture below).  If the bend angle is not 90 degrees, it is the distance from the start of the bend radius, to the tangent point of the outside radius.

Explanation of sheet metal design parameters

Like Bend Deductions, Bend Allowance and Outside Setback can help you manually modify a flat pattern to obtain the correct finished part size.  We again highly recommend that you don't do this manually, and that you use sheet metal-capable CAD software instead.  If you already know how to do it manually and want to do so, you can use the parameters automatically computed by our web app to finalize the size of your flat and the placement of the bend lines.

 

7. What is the Maximum Box Depth?

Maximum box depth (or channel depth) is the deepest channel we can create in a part without causing a collision with the brake or tooling during the bend.

The "bend stackup" on our press brake looks like the following:

Sheet metal bending stackup

Depending on the geometry of your bent part, it could collide with the punch or V-die, die holder, brake, punch holder, or ram during the bend. 

The profiles for our available punches currently match what is shown above.  We do not currently have gooseneck punches or extensions to allow for deep, narrow channels, although we will expand our tooling options over time.  

When you upload your part and select bend lines, our online system will automatically simulate the bends and let you know whether it can be bent without collisions.  You can also use the tables below as a guide to determine maximum box/channel depth based on channel width and flange height.  These should be used as general guidelines, and may not cover all cases.

Channel width and max flange heights in the table below are measured from the inside of the part.

Materials between 0.024" and 0.08" thick

110 Copper

260 Brass

Maximum flange heights for the above materials are given below:

Channel Width (in)
Max Flange Height (in)
0.25"
N/A
0.5"
N/A
0.75"
0.4"
1.0"
0.8"
1.25"
1.2"
1.5"
1.45"
1.75"
1.7"
2.0"
1.85"
2.25"
1.95"
2.5"
2.05"
2.75"
2.25"
3.0"
2.55"
3.25"
2.3"
3.5"
2.1"
3.75"
2.0"
4"
2.1"
4.25"
2.2"
4.5"
2.45"
4.75"
2.7"
5"
2.9"
5.25"
3.2"
5.5"
3.45"
5.75"
3.7"
6.0"
4.6"
6.25"
4.85"
6.5"
5.1"
6.75"
5.35"
7.0"
5.6"
7.25"
5.85"
7.5"
6.1"
7.75"
6.1"
8.0"
6.25"
8.25"
6.5"
8.5"
6.75"
8.75"
7.0"
9.0"
7.25"
9.25"
7.5"
9.5"
7.75"
9.75"
8.0"
10.0"
8.25"
11.0"
9.25"
12.0"
10.25"
13.0"
11.25"
Minimum flange height diagram

Materials between 0.09" and 0.135" thick

A36 Steel, HR P&O

 

5052 H32 Aluminum: 

 

A1008 Steel, CR

304 Stainless Steel, #4

 

304 Stainless Steel #2B

316 Stainless Steel #2B

110 Copper

260 Brass

Maximum flange heights for the above materials are given below:

Channel Width
Max Flange Height
0.25"
N/A
0.5"
N/A
0.75"
N/A
1.0"
0.9"
1.25"
1.2"
1.5"
1.45"
1.75"
1.6"
2.0"
1.75"
2.25"
1.85"
2.5"
2.0"
2.75"
2.25"
3.0"
2.25"
3.25"
2.1"
3.5"
1.9"
3.75"
1.9"
4.0"
1.9"
4.25"
2.1"
4.5"
2.3"
4.75"
2.5"
5.0"
2.7"
5.25"
3.0"
5.5"
3.2"
5.75"
3.4"
6.0"
4.5"
6.25"
4.7"
6.5"
4.9"
6.75"
5.2"
7.0"
5.4"
7.25"
5.6"
7.50"
5.9"
7.75"
6.1"
8.0"
6.3"
8.25"
6.5"
8.5"
6.7"
8.75"
6.9"
9.0"
7.2"
9.25"
7.4"
9.5"
7.6"
9.75"
8.0"
10.0"
8.25"
11.0"
9.25"
12.0"
10.25"
13.0"
11.25"
Maximum flange height diagram

Materials between 3/14" and 1/4" thick

A36 Steel, HR P&O

5052 H32 Aluminum: 

304 Stainless Steel, #1

316 Stainless Steel, #1

260 Brass

Maximum flange heights for the above materials are given below:

Channel Width
Max Flange Height
0.25"
N/A
0.5"
N/A
0.75"
N/A
1.0"
N/A
1.25"
N/A
1.5"
N/A
1.75"
1.5"
2.0"
1.6"
2.25"
1.7"
2.5"
1.8"
2.75"
2"
3.0"
1.9"
3.25"
1.8"
3.5"
1.7"
3.75"
1.7"
4.0"
1.8"
4.25"
2"
4.5"
2.2"
4.75"
2.4"
5.0"
2.6"
5.25"
2.9"
5.5"
3.1"
5.75"
3.3"
6.0"
4.4"
6.25"
4.6"
6.5"
4.8"
6.75"
5.1"
7.0"
5.3"
7.25"
5.5"
7.5"
5.7"
7.75"
5.9"
8.0"
6.2"
8.25"
6.4"
8.5"
6.6"
8.75"
6.8"
9.0"
7.1"
9.25"
7.3"
9.5"
7.5"
9.75"
7.9"
10.0"
8.125"
11.0"
9.125"
12.0"
10.125"
13.0"
11.125"
Maximum flange height diagram
 
fixed bends2.png
fixed bends1.png

To fix this, you can add a tabbed bend-surface to the edge of your part, like the one below:

bad bends2.png
bad bends1.png

However, the part below does not work, because it lacks a reference edge for the press brake backgauge:

valid bends (1).png
valid bends2 (1).png

Our press brake a a CNC back gauge that allows us to place parts in exactly the right spot so that bends take place on the bend line.  In order to make your part, we must have a "gauging" surface on the part so that it can be aligned on the back gauge to perform the bend.

We are working on tools to remove this requirement, but for now, all bend lines must be parallel to a straight part edge, so that we have a reference surface to position the part for bending.

For example, the following part works because every bend line is parallel to a part edge:

8. What is the back-gauge, and does it affect bending capabilities?

We are working on tools to make bends like this easier for you to request, but for now, bends lines must have a parallel gauging surface.

 

READY TO GET STARTED?