{"id":14747,"date":"2026-09-20T09:48:57","date_gmt":"2026-09-20T09:48:57","guid":{"rendered":"https:\/\/elitemoldtech.com\/sheet-metal-bend-radius-k-factor\/"},"modified":"2026-10-01T09:55:23","modified_gmt":"2026-10-01T09:55:23","slug":"sheet-metal-bend-radius-k-factor","status":"publish","type":"post","link":"https:\/\/elitemoldtech.com\/ar\/sheet-metal-bend-radius-k-factor\/","title":{"rendered":"Sheet Metal Bend Radius and K-Factor: Charts and How to Calculate Them"},"content":{"rendered":"

The smallest safe sheet metal bend radius depends on material and temper: about 0.5T to 1T for cold-rolled steel and 5052-H32 aluminum, around 1T for annealed 304 stainless, and 2T to 6T for 6061-T6. The K-factor, usually between 0.33 and 0.50, locates the neutral axis so you can calculate flat blank length before cutting.<\/p>\n

What Bend Radius and K-Factor Mean<\/h2>\n

The inside bend radius\u00a0(R) is the radius on the inside of the bend, and the outside radius equals R plus material thickness (T).<\/p>\n

When sheet bends, the outside stretches while the inside compresses. Somewhere between them sits the neutral axis, the one layer that keeps its original length through the bend. It does not stay at mid-thickness; it shifts toward the inside of the bend.<\/p>\n

The K-factor\u00a0describes that shift:<\/p>\n

K = t \u00f7 T<\/p>\n

where t is the distance from the inside surface to the neutral axis. A K-factor of 0.50 means the neutral axis sits at mid-thickness. Real bends usually fall between 0.33 and 0.50. The K-factor matters because the neutral axis length is the length you cut, so it drives every flat pattern.<\/p>\n

Minimum Sheet Metal Bend Radius by Material<\/h2>\n

Bending tighter than the minimum bend radius cracks the outside surface. The ranges below are common guidance for bends across the rolling direction.<\/p>\n\n\n\n\n\n\n\n\n
Material and temper<\/td>\nTypical minimum inside radius<\/td>\n\u0627\u0644\u0645\u0644\u0627\u062d\u0638\u0627\u062a<\/td>\n<\/tr>\n
Cold-rolled low-carbon steel<\/td>\n0.5T\u20131T<\/td>\nVery formable in thin gauges<\/td>\n<\/tr>\n
304 \/ 316 stainless, annealed<\/td>\nAbout 1T, up to 2T in thicker gauges<\/td>\nWork hardens; more springback<\/td>\n<\/tr>\n
5052-H32 aluminum<\/td>\nAbout 1T, 0.5T in thin gauges<\/td>\nThe easy-bending aluminum<\/td>\n<\/tr>\n
6061-T6 aluminum<\/td>\n2T\u20133T thin, up to 4T\u20136T heavier<\/td>\nLow ductility; cracks easily<\/td>\n<\/tr>\n
Annealed copper and brass<\/td>\nTight, often below 1T<\/td>\nSoft; mark easily<\/td>\n<\/tr>\n<\/tbody>\n<\/table>\n

Two factors shift these numbers. Grain direction\u00a0matters: bending parallel to the rolling direction cracks more easily, so rotate the blank on the sheet when a bend is critical. Temper\u00a0matters too: 6061 bent in the O or T4 temper and aged afterward can take far tighter radii than T6. Mill specifications such as ASTM B209\u00a0set bend requirements for aluminum sheet by alloy and temper, and are the reference to check for critical parts.<\/p>\n

Our advice is simple. If a design needs tight bends in aluminum, use 5052-H32 rather than fighting 6061-T6.<\/p>\n

K-Factor Chart by Material and R\/T Ratio<\/h2>\n

K-factor depends mostly on the ratio of inside radius to thickness (R\/T). Tight bends pull the neutral axis further inward.<\/p>\n\n\n\n\n\n\n
\u0627\u0644\u0645\u0648\u0627\u062f<\/td>\nR\/T below 1<\/td>\nR\/T 1 to 3<\/td>\nR\/T above 3<\/td>\n<\/tr>\n
\u0623\u0644\u0648\u0645\u0646\u064a\u0648\u0645<\/td>\n0.33<\/td>\n0.40<\/td>\n0.50<\/td>\n<\/tr>\n
\u0627\u0644\u0641\u0648\u0644\u0627\u0630 \u0627\u0644\u0637\u0631\u064a<\/td>\n0.38\u20130.42<\/td>\n0.42\u20130.46<\/td>\n0.50<\/td>\n<\/tr>\n
\u0627\u0644\u0641\u0648\u0644\u0627\u0630 \u0627\u0644\u0645\u0642\u0627\u0648\u0645 \u0644\u0644\u0635\u062f\u0623<\/td>\n0.40\u20130.44<\/td>\n0.44\u20130.48<\/td>\n0.50<\/td>\n<\/tr>\n<\/tbody>\n<\/table>\n

Bending method shifts it as well. Protolabs cites about 0.33 for an air bend and 0.42 for a bottom bend when R is below T. Treat every chart value as a starting point, then confirm with a test bend on your actual material and tooling.<\/p>\n

How to Calculate Bend Allowance and Bend Deduction<\/h2>\n

Follow these steps for a single bend:<\/p>\n

    \n
  1. Collect the inputs:\u00a0thickness T, inside radius R, bend angle A in degrees, and K-factor K.<\/li>\n
  2. Bend allowance\u00a0(BA), the arc length of the neutral axis: BA = (\u03c0 \u00f7 180) \u00d7 A \u00d7 (R + K \u00d7 T)<\/li>\n
  3. Outside setback\u00a0(OSSB): OSSB = tan(A \u00f7 2) \u00d7 (R + T)<\/li>\n
  4. Bend deduction\u00a0(BD): BD = 2 \u00d7 OSSB \u2212 BA<\/li>\n
  5. Flat length\u00a0from outside flange dimensions: flat = flange 1 + flange 2 \u2212 BD<\/li>\n<\/ol>\n

    Worked example.\u00a0A 2 mm cold-rolled steel bracket has a 90\u00b0 bend, a 2 mm inside radius and flanges of 50 mm and 30 mm measured to the outside. Using K = 0.42:<\/p>\n