Every sheet metal part starts as a flat blank. Getting from a dimensioned 3D part back to that flat blank requires understanding how metal behaves during bending. The geometry is straightforward; the variables that trip people up are the K-factor, the difference between bend deduction and bend allowance, and knowing when the textbook numbers do not match the press brake.
This guide covers the theory behind flat pattern development, explains K-factor in practical terms, walks through the math for bend deduction and bend allowance, and addresses the real-world variables that make test bends necessary. If you have ever had a flat blank come out 1/16 inch too long or too short after bending, this guide explains why and how to fix it.
The Neutral Axis and K-Factor
When sheet metal bends, the outside surface stretches and the inside surface compresses. Somewhere between those two surfaces is a plane that neither stretches nor compresses. That plane is the neutral axis, and its location determines everything about flat pattern development.
K-factor is the ratio of the neutral axis location to the material thickness, measured from the inside of the bend. If the neutral axis is at 40 percent of the material thickness from the inside surface, K = 0.40. If it is at 50 percent (the center), K = 0.50. In practice, the neutral axis shifts toward the inside of the bend because the inner material compresses more easily than the outer material stretches.
For air bending mild steel with a standard V-die opening of 6 to 8 times the material thickness, K = 0.44 is the most widely used default. Stainless steel runs slightly higher at 0.45. Soft aluminum (3003, 5052) runs lower at 0.38-0.42. Hard aluminum (6061-T6) runs around 0.42-0.45. Copper and brass are in the 0.35-0.40 range.
These are starting points, not absolutes. K-factor varies with tooling (die opening, punch radius), bending method (air bend vs bottom vs coining), material temper, grain direction, and even the specific lot of material. The only way to get a K-factor that is accurate to within 0.005 is to bend a test coupon and measure the result.
K = t / T
Where t = distance from inside surface to neutral axis, T = material thickness.
Typical values: Mild steel 0.44, Stainless 0.45, Aluminum (soft) 0.40, Copper 0.38.
Bend Deduction & K-Factor Calculator
Calculate bend allowance, bend deduction, K-factor, and flat pattern length for sheet metal bending. Supports air bending, bottoming, and coining with common materials.
Bend Allowance: The Arc Length Method
Bend allowance (BA) is the length of the neutral axis arc through the bend zone. It represents the physical amount of material consumed by the bend. The formula is:
BA = (pi / 180) x angle x (inside_radius + K x thickness)
For a 90-degree bend in 16-gauge mild steel (0.060 inch) with a 0.060-inch inside radius and K = 0.44: BA = (3.14159 / 180) x 90 x (0.060 + 0.44 x 0.060) = 1.5708 x 0.0864 = 0.1357 inches.
The bend allowance method calculates flat pattern length by summing the inside dimensions (flat lengths between bend tangent lines) and adding the bend allowance for each bend. This method is used by most CAD systems and is the standard in European fabrication.
The advantage of bend allowance is that it works directly from inside dimensions, which is how most engineering drawings are dimensioned. The disadvantage is that you need to identify the bend tangent lines on the drawing, which requires knowing the inside radius and doing some geometry.
BA = (π / 180) × θ × (R + K × T)
Where θ = bend angle (degrees), R = inside radius, K = K-factor, T = material thickness.
Flat Pattern (BA method):
L = sum of inside flat lengths + sum of bend allowances
Bend Deduction: The Shop Floor Method
Bend deduction (BD) is the amount subtracted from the sum of the outside mold line dimensions to get the flat pattern length. Most American fabrication shops and many press brake operators work in bend deduction because it maps directly to the way parts are dimensioned on shop drawings: outside dimensions from bend line to edge.
The formula connects bend deduction to bend allowance through outside setback (OSSB):
OSSB = (inside_radius + thickness) x tan(angle / 2)
BD = 2 x OSSB - BA
For the same 90-degree bend: OSSB = (0.060 + 0.060) x tan(45) = 0.120 x 1.0 = 0.120 inches. BD = 2 x 0.120 - 0.1357 = 0.1043 inches.
To use the bend deduction method, add up all the outside dimensions (flange lengths measured to the outside mold line at each bend), then subtract the bend deduction for each bend. The result is the flat blank length.
Both methods produce the same flat pattern length. The difference is which dimensions you start with: inside dimensions for bend allowance, outside dimensions for bend deduction. Use whichever matches how your drawings are dimensioned and how your shop thinks about parts.
Bend Deduction & K-Factor Calculator
Calculate bend allowance, bend deduction, K-factor, and flat pattern length for sheet metal bending. Supports air bending, bottoming, and coining with common materials.
How Tooling Affects the Result
The V-die opening is the single biggest variable after material type. A wider die opening produces a larger inside radius and shifts the K-factor. The general rule for air bending: inside radius equals approximately the die opening divided by 6. An 8-times die opening (8T, where T is material thickness) produces a radius slightly larger than the material thickness. A 12-times die opening produces a radius roughly twice the material thickness.
Punch tip radius matters for bottoming and coining but has little effect on air bending because the material does not contact the punch tip at full depth. In air bending, the inside radius is controlled by the die, not the punch.
Springback is the other tooling variable. After the ram retracts, the material springs back toward its original flat state. Mild steel springs back 2-4 degrees on a 90-degree air bend. Stainless springs back 4-7 degrees. Aluminum varies from 2-10 degrees depending on temper. CNC press brakes compensate automatically with angle measurement and crowning. Manual brakes require overbending by the springback amount.
The practical impact: if your K-factor tables were developed on a specific die opening and your shop switches to a different die, the flat patterns will be off. Always document which die was used when establishing K-factor values for a given material and thickness.
Air bend inside radius ≈ die opening / 6
8T die opening: inside radius ≈ 1.3 x thickness
12T die opening: inside radius ≈ 2 x thickness
Always verify with a test bend. The 1/6 rule is approximate.
Minimum Bend Radius and Cracking
Every material has a minimum inside bend radius below which the outer surface cracks. The minimum radius depends on the material, temper, grain direction, and thickness. Bending across the grain (perpendicular to the rolling direction) allows tighter radii than bending along the grain.
General minimums for 90-degree bends across the grain: Mild steel (A36, 1018): 1T (radius equals thickness). Stainless 304: 1T. Aluminum 3003-H14: 0.5T. Aluminum 5052-H32: 1T. Aluminum 6061-T6: 2T. Copper (half-hard): 1T. Brass (half-hard): 1T.
For bends along the grain, increase the minimum radius by 50-100 percent. For aged or work-hardened material, increase further. For material thicker than 0.125 inch, the minimum radius often increases faster than a simple multiple of thickness.
When a drawing specifies a radius tighter than the material minimum, you have three options: change the material or temper, change the grain direction, or negotiate a larger radius with the designer. Trying to force a tight bend will result in cracking, and the crack may not be visible until the part is in service and fails under load.
Test Bends: Why They Are Not Optional
Theoretical calculations get you within 0.010-0.020 inches of the correct flat pattern for a single bend on familiar material with well-characterized tooling. For a part with four or five bends, the cumulative error can reach 0.050-0.100 inches, which is unacceptable for most precision work.
The solution is test bends. Cut a coupon from the production material, bend it on the production die, measure the result, and back-calculate the actual K-factor. Use that empirical K-factor for all flat patterns on that job. This takes 15 minutes and saves hours of scrap and rework.
The test bend procedure: Cut a strip at least 4 inches wide by 8 inches long. Mark two lines 2 inches from each end. Bend a 90-degree angle at one mark. Measure the resulting flange lengths (inside dimensions). Back-calculate: K = (BA / (pi / 180 x angle) - inside_radius) / thickness. Compare this K to your assumed value and adjust.
For production runs, make the test bend part of your setup procedure. For prototype and one-off work, use a conservative flat pattern (slightly long) and trim to final dimension after bending. Adding material is easy; removing too much is not.
1. Bend a 90° test coupon
2. Measure inside flat lengths (F1, F2)
3. BA = Total flat blank length - F1 - F2
4. K = (BA / (1.5708 × T) - R) / T
Where T = thickness, R = measured inside radius.
Bend Deduction & K-Factor Calculator
Calculate bend allowance, bend deduction, K-factor, and flat pattern length for sheet metal bending. Supports air bending, bottoming, and coining with common materials.