Bend Allowance and Flat Patterns

A sheet metal part starts flat, and bending changes its length. If you cut a blank to the finished dimensions added together, the part comes out too long. The flat pattern is the blank size that bends into the right part. Anyone who lays out sheet metal or runs a press brake needs this math, even when software does most of it, because you have to be able to spot a wrong number.

What You Will Be Able to Do

• Explain the neutral axis and the K-factor.
• Calculate bend allowance for a bend.
• Calculate setback and bend deduction.
• Work out the flat length of a part with two legs.
• Check a calculation with a test bend.

What Happens in a Bend

When sheet bends, the outside surface stretches and the inside surface compresses. Somewhere between them is a layer that does neither. That layer is the neutral axis, and its length stays the same before and after bending. All flat pattern math is based on measuring along it.

The neutral axis does not sit at the center of the thickness. It moves toward the inside of the bend.

The K-factor tells you where the neutral axis sits. It is the ratio of the neutral axis location to the material thickness, measured from the inside surface. A K-factor of 0.33 means the neutral axis is one-third of the way through the metal.

These are starting values. Actual K-factors change with material, thickness, radius and tooling, so a shop's own bend chart or test bends beat a textbook number.

Key Terms

• Inside radius (R): The radius of the inside surface of the bend.
• Thickness (T): The metal's thickness.
• Bend angle (A): How far the metal has bent from flat. A right-angle bend is a 90 degree bend.
• Bend allowance (BA): The arc length of the neutral axis through the bend. It is the flat length that goes into the bend zone.
• Setback (SB): The distance from the tangent point of the bend to the outside corner, or mold line.
• Bend deduction (BD): How much you subtract from the outside dimensions to get the flat length.
• Mold line: The line where the flat outside surfaces would meet if there were no radius.

The Formulas

Bend allowance:

BA = (pi / 180) x A x (R + K x T)

Setback:

SB = tan(A / 2) x (R + T)

For a 90 degree bend, tan(45) equals 1, so SB = R + T.

Bend deduction:

BD = 2 x SB - BA

Flat length, when the drawing gives outside dimensions:

Flat = sum of outside dimensions - BD for each bend

Worked Example: One 90 Degree Bend

You need an L-shaped bracket with outside legs of 2.000 inches and 3.000 inches, made from 16-gauge steel (0.060 inch), with a 0.0625 inch inside radius. Use K = 0.33.

Step 1: Bend allowance

• BA = 0.01745 x 90 x (0.0625 + 0.33 x 0.060)
• BA = 1.5708 x (0.0625 + 0.0198)
• BA = 1.5708 x 0.0823
• BA = 0.129 inch

Step 2: Setback

• SB = 0.0625 + 0.060 = 0.1225 inch

Step 3: Bend deduction

• BD = 2 x 0.1225 - 0.129
• BD = 0.245 - 0.129 = 0.116 inch

Step 4: Flat length

• Flat = 2.000 + 3.000 - 0.116 = 4.884 inches

You can check that with bend allowance. Each flat leg, without its part of the bend, is its outside dimension minus the setback: 2.000 - 0.1225 = 1.8775 inches, and 3.000 - 0.1225 = 2.8775 inches. Add the allowance: 1.8775 + 2.8775 + 0.129 = 4.884 inches. Both methods agree.

Worked Example: A Channel With Two Bends

A U-channel has outside dimensions of 1 inch, 4 inches and 1 inch, with the same material and radius. There are two 90 degree bends.

• Sum of outside dimensions: 1 + 4 + 1 = 6.000 inches
• Two bend deductions: 2 x 0.116 = 0.232 inch
• Flat length: 6.000 - 0.232 = 5.768 inches

A common mistake is to subtract only one deduction. Every bend gets its own.

Bends Other Than 90 Degrees

The angle in the formulas is the bend angle, how far the metal moved from flat. If a drawing shows the included angle between the flanges, convert it first. A 135 degree included angle means a 45 degree bend.

For a 45 degree bend in the same material:

• BA = 0.01745 x 45 x 0.0823 = 0.065 inch
• SB = tan(22.5) x 0.1225 = 0.414 x 0.1225 = 0.051 inch
• BD = 2 x 0.051 - 0.065 = 0.037 inch

Small bends use smaller deductions.

Inside Radius in Air Bending

In air bending, the punch does not set the radius. The die opening does. On mild steel, the inside radius comes out at about 15 to 20 percent of the V-die opening, or roughly the opening divided by 6. If you use the wrong radius in your math, your flat length will be off. So find out what die the brake will actually use, or ask the operator, before you finalize the blank.

For a simple check, a 1/2 inch V-die on mild steel gives an inside radius of about 0.083 inch.

Checking Your Numbers With a Test Bend

Software, charts and formulas are only as good as their inputs. A test bend tells you what your material and tooling really do.

1. Shear a strip of the same material, thickness and grain direction.
2. Measure its length exactly. Say it is 6.000 inches.
3. Bend it at the middle with the actual tooling, to a 90 degree angle.
4. Measure both outside legs. Say they are 3.060 inches and 3.058 inches.
5. Add the legs: 6.118 inches.
6. Subtract the original length. Your bend deduction is 0.118 inch.

Write that value down for that material, thickness and tooling. Many shops keep a bend chart posted at the brake with these numbers, and that chart should win over a general rule.

Other Things That Affect the Blank

• Material lot: Two batches of the same grade can spring back and stretch differently.
• Grain direction: Bending across the grain lets you bend tighter. Bending along it may crack on tight radii.
• Hems: A hem folds metal back on itself. It has its own allowance, so use a chart or a test.
• Holes near a bend: Metal near the bend moves, and holes can distort. Keep them clear of the bend zone, or add them after bending.
• Relief cuts: Where two bends meet, a small notch keeps the corner from tearing.

Using Software

CAD packages unfold a part automatically, using a K-factor or bend table. That is fast and reliable if the inputs are right. Always check that the software has the correct thickness, radius and K-factor, and check one bend by hand. If the first part comes off the brake long or short, the fix is usually in the table.

Common Mistakes

• Adding outside dimensions and stopping. The part comes out too long by one deduction per bend.
• Using the included angle in the formula. A 135 degree corner is a 45 degree bend.
• Assuming the punch radius is the part radius. In air bending, the die opening sets it.
• Using thickness from a gauge chart without measuring. Actual sheet can vary, and small errors add up over many bends.
• Cutting a full batch off an untested number. One test bend protects the whole lot.

Check Your Understanding

A drawing shows a part with outside legs of 4 inches and 2 inches and one 90 degree bend. Your chart gives a bend deduction of 0.130 inch. What is the flat length?

4 + 2 - 0.130 = 5.870 inches.

You used K = 0.33 from a textbook, but your parts keep coming out 0.010 inch long. What should you do?

Run a test bend with the real tooling and material, then update the deduction from the measurement. Actual results beat a general number.

A brake operator swaps a 1/2 inch V-die for a 1 inch V-die. Does your flat pattern change?

Yes. A wider die gives a larger inside radius in air bending, so the bend allowance and deduction change.

A corner on a drawing has a 120 degree included angle. What bend angle goes in the formula?

60 degrees, because 180 minus 120 equals 60.

Key Takeaways

• The neutral axis stays the same length, and all flat pattern math follows it.
• K-factor locates the neutral axis. About 0.33 is typical for air bending mild steel.
• Bend allowance is the arc length of the neutral axis through the bend.
• Subtract one bend deduction for each bend from the sum of the outside dimensions.
• In air bending, the die opening sets the inside radius.
• Test bends and shop charts beat general numbers.