Sheet Metal K-Factor: Chart, Formula & Bend Allowance

Sheet metal K-factor locates the neutral axis as a fraction of material thickness. It lets you calculate bend allowance, bend deduction and the flat length; common starting values fall around 0.33-0.50, but the correct production value depends on material, thickness, inside radius and tooling.

Use the charts and formulas below to build a first flat pattern, then replace the assumed value with a measured test bend. This page covers the general method and starting tables for steel, stainless and aluminum. Looking specifically for K-factor for copper? Use the dedicated copper K-factor and bend allowance guide for C101/C110 temper-specific starting values because temper changes copper bending behavior. For production review, see our press brake bending capabilities.

Why K-Factor Matters

When you bend a piece of sheet metal, here’s what physically happens:

1. Inside fiber (closer to the punch) gets compressed — its length decreases
2. Outside fiber (farther from the punch) gets stretched — its length increases
3. Somewhere between them, there’s a fiber whose length doesn’t change. This is the neutral axis.

The position of the neutral axis depends on:

• Material thickness
• Inside bend radius
• Material properties (yield strength, work hardening)
• Bend method (air bend, bottom bend, coining)
• Bend angle

K-factor = distance from inside surface to neutral axis ÷ material thickness

For most sheet metal bends, the neutral axis sits closer to the inside (compressed) surface — typically at 33-50% of material thickness, so K ≈ 0.33-0.5.

The Core Formulas

Bend Allowance (BA)

BA is the length of the neutral axis through the bend. This is what you add to the flat sides to get the total flat pattern length.

BA = (π/180) × A × (R + K × T)

Where:

• A = bend angle (degrees)
• R = inside bend radius
• K = K-factor
• T = material thickness

Bend Deduction (BD)

BD is what you subtract from the sum of “outside dimensions” to get the flat pattern length. Many designers find BD easier to work with than BA.

BD = 2 × (R + T) × tan(A/2) − BA

For a 90° bend:

BD = 2 × (R + T) − BA

Flat Length using BA

If you have flange lengths measured to the bend tangent line:

Flat Length = Flange A + Flange B + BA

Flat Length using BD

If you have outside dimensions (to the apex):

Flat Length = Outside A + Outside B − BD

The Three Most Common Mistakes

Mistake 1: Using the CAD default K-factor for everything

SolidWorks defaults to K = 0.5. Inventor defaults to 0.44. Neither is accurate for most real bends — and using the same K across materials and bend radii produces consistently wrong flat patterns.

Mistake 2: Ignoring inside bend radius

K-factor changes with the R/T ratio (inside radius ÷ material thickness):

R/T Ratio	Approximate K (Mild Steel)
0.5	0.30
1.0	0.33
1.5	0.40
2.0	0.44
3.0+	0.47
5.0+	0.50

Small R/T = neutral axis closer to inside = smaller K. Use a single K for all bends and you’ll be wrong on small-radius bends.

Mistake 3: Not validating empirically

Published K-factor tables are estimates. Your actual K depends on your material, your tooling, your machine, and your bend technique. The only way to get an accurate K is to bend a test piece and measure.

K-Factor Charts (Starting Points)

These are typical starting values. Always validate with a test piece for production work.

Mild steel (cold-rolled, 60-80 ksi)

Inside Radius (R)	Material Thickness (T)	R/T	Recommended K
0.8 mm	1.5 mm	0.5	0.30
1.5 mm	1.5 mm	1.0	0.33
2.0 mm	2.0 mm	1.0	0.33
3.0 mm	2.0 mm	1.5	0.40
6.0 mm	3.0 mm	2.0	0.44
10 mm	3.0 mm	3.3	0.47

Stainless steel (304, 316 — work hardens more)

Add ~0.02-0.03 to the mild steel K for same R/T ratio. Stainless’s higher work hardening shifts the neutral axis slightly outward.

Aluminum (5052, 6061 — more elastic)

Subtract ~0.02-0.03 from the mild steel K. Aluminum’s lower yield strength means more compression on the inside, shifting the neutral axis inward.

R/T Ratio	Steel K	Stainless K	Aluminum K
0.5	0.30	0.33	0.28
1.0	0.33	0.36	0.31
1.5	0.40	0.43	0.38
2.0	0.44	0.46	0.42
3.0+	0.47	0.49	0.45

For material-specific properties, see our 304 vs 316 stainless guide, 6061 vs 6063 aluminum comparison, and carbon vs stainless steel comparison.

Bend Allowance Calculation Example

Problem: 2.0 mm mild steel, 90° bend, 2.0 mm inside radius (R/T = 1.0, K = 0.33). Outside-to-outside dimensions: 50 mm × 30 mm.

Step 1: Calculate BA

BA = (π/180) × 90 × (2.0 + 0.33 × 2.0)
BA = 1.5708 × (2.0 + 0.66)
BA = 1.5708 × 2.66
BA = 4.18 mm

Step 2: Calculate BD

BD = 2 × (R + T) × tan(45°) − BA
BD = 2 × (2.0 + 2.0) × 1.0 − 4.18
BD = 8.0 − 4.18
BD = 3.82 mm

Step 3: Calculate flat length

Using outside dimensions:

Flat = 50 + 30 − 3.82 = 76.18 mm

The flat pattern is 76.18 mm, not 80 mm (sum of outside dimensions) and not 72 mm (sum of inside dimensions). Cutting at either of those wrong values is the typical “my bent part is the wrong size” error.

How to Validate K-Factor Empirically

This is the most important step for production work. Published charts get you in the ballpark; only an empirical test gets you exact.

Test procedure

1. Cut a strip of your exact production material, known flat length (e.g., 100.0 mm)
2. Bend at 90° with your production tooling and machine
3. Measure the resulting outside dimensions (e.g., 51.2 mm and 51.6 mm)
4. Calculate the BD:

   BD = Sum of outsides − Flat length = (51.2 + 51.6) − 100.0 = 2.8 mm

5. Back-calculate K using:

   BD = 2(R + T) tan(A/2) − (π/180) × A × (R + K × T)

   Solve for K.

Or just iterate K in your CAD until the unfold matches your measured flat length.

Why this matters

A K-factor accurate to ±0.02 produces parts accurate to about ±0.3 mm on typical sheet metal sizes. A K-factor wrong by 0.1 produces parts off by 1.5-3 mm — a critical fit problem.

Other Factors That Affect K-Factor

Factor	Effect on K
Bend method (air bend vs bottom bend)	Bottom bend → slightly higher K (more compression)
Coining	Highest K (material flows, neutral axis shifts)
Punch radius	Larger radius → larger K
Material work hardening	More hardening → K shifts outward
Grain direction	Bending across grain → slightly higher K
Multiple bends close together	Interaction can shift K
Sharp bends (R < T)	K becomes unpredictable; avoid

For more on bending issues, see our press brake bending defects guide and hem & seam design patterns.

Common Design Rules

To make K-factor predictable and your flat patterns reliable:

1. Minimum bend radius: R ≥ material thickness (R ≥ T)
2. Avoid sharp bends: R < T causes cracking and unpredictable K
3. Consistent R/T across the part: simplifies K-factor specification
4. Standard radii: use 1×T, 2×T, 3×T whenever possible
5. Allow K variation: don’t tolerance bend dimensions to ±0.05 mm if you haven’t validated K to that precision

Practical Workflow

Here’s how the K-factor question actually plays out in production:

Step 1: Establish K-factor for your standard combinations

Test bend each material × thickness × bend radius combination you commonly use. Record empirical K-factors in a shop table.

Step 2: Set CAD defaults to your tested K

Configure SolidWorks Sheet Metal / Inventor / Solid Edge to use your empirical K, not the software default.

Step 3: Validate first article

For any new design, first-article validation is the final check. If the bent part is off, the K assumption was wrong — not the drawing.

Step 4: Document for your supplier

When sending parts to a fabricator, include either:

• Flat pattern with K-factor noted, OR
• 3D model with bend table specifying K-factor

A capable supplier will validate against their own data; specifying K-factor upfront avoids “my unfold doesn’t match yours” disputes.

For more DFM rigor, see our 17-point DFM checklist and ISO 2768 tolerance guide.

How DRAmetal Handles K-Factor

For OEM customer parts, our process is setup-specific:

1. DFM review checks material, thickness, bend radii, grain direction and problematic R/T ratios.
2. Starting value selection uses the closest validated material, radius and tooling combination rather than an unqualified CAD default.
3. Test bending measures the actual flange and bend deduction when the geometry or tolerance warrants it.
4. First-article validation compares the formed part with the controlled drawing using an inspection method suited to the feature.
5. Production release records the approved flat pattern, tooling assumptions and drawing revision for repeat orders.

For our press brake bending capabilities and DFM review process, see our service pages. To request a sheet metal design review, submit your CAD files. The initial response target is within 24 working hours; K-factor and DFM feedback require material, tooling and bend review.

Bottom Line

K-factor is a small variable with a large impact. Wrong K-factor = wrong flat patterns = bent parts that don’t match drawings. The fix is straightforward: understand the geometry, use realistic K values from charts as starting points, and validate empirically for production work.

The buyers and engineers who get this right are the ones whose first articles come out the size the drawing says. The ones who fight chronic dimensional issues are usually using CAD default K-factors that don’t match their actual material and tooling — fixable in an afternoon of test bending.

Get K-factor right once, document it for your standard material × thickness × radius combinations, and move on. Then your flat patterns just work.