# Choosing the right bend radius and minimum flange Quelle: > Why a flange cannot be as short as you like, which inside radius actually forms during bending, and how to read both for each sheet thickness. Design & manufacturing Why a flange cannot be as short as you like, which inside radius actually forms during bending, and how to read both for each sheet thickness. MVG editorial team · Values from our production and the material standards Published on 3 October 2026 · 4 min read The most frequent block in the bent part configurator is a flange that is too short. The second most frequent question concerns the inside radius. Both follow from the same tool: the die. If you know its width, you can read the flange and the radius yourself. Problem ## The problem: the flange slips, the radius does not fit An angle with a 6 mm flange made from 3 mm sheet looks fine in the CAD drawing. On the press brake, the flange drops into the groove of the die, and the bend comes out crooked or cannot be made at all. The radius is similar: the drawing shows a sharp inside edge or a radius equal to the sheet thickness. In air bending, however, the radius is set by the die, the material and the sheet thickness, and on thin sheet it is usually larger. The outside dimensions and the flat pattern then deviate. Cause ## The cause: the opening width of the die Bending takes place between the punch and the die. The die is a rail with a groove; its width is called the die opening (W value). The thicker the sheet, the wider the groove. We bend mainly on CDW dies (Consistent Die Width, 28°); which die a sheet gets depends on the material and the sheet thickness. This results in two limits. First, the flange must rest on both edges of the groove: the minimum flange of the die measured on our press brake applies, at least 8 mm. Second, in air bending the inside radius results from the die, the material and the sheet thickness. We measured it on our press brake for each die; on thin sheet it is usually larger than the sheet thickness. For 1 to 2.5 mm sheet it lies between 2 and 3.8 mm. | Sheet thickness | Steel | Stainless steel | Aluminium | |---|---|---|---| | 0.5 mm | 1 mm | 1 mm | 1 mm | | 0.8 mm | 1.6 mm | 1.6 mm | 1 mm | | 1 mm | 2.8 mm | 3.5 mm | 3.4 mm | | 1.5 mm | 3.3 mm | 3.7 mm | 3.4 mm | | 2 mm | 2 mm | 3.8 mm | 3.8 mm | | 2.5 mm | 2.5 mm | 3.8 mm | 3.8 mm | | 3 mm | 4.9 mm | 5.7 mm | 3.7 mm | | 4 mm | 4 mm | 6.7 mm | 4 mm | | 5 mm | 8 mm | 10.4 mm | 6.5 mm | | 6 mm | 9 mm | 9 mm | 9 mm | | 8 mm | Cut-to-size | Cut-to-size | 12 mm | Inside radius at 90° with the standard tool, measured on our press brake. “Cut-to-size”: in this thickness we supply the material as a cut-to-size part. Solution ## The solution: three rules for your design Three rules help you avoid almost all questions about bent parts: - Make each flange at least as long as the minimum flange in the table below, never less than 8 mm. 3 mm steel runs over the W 24 die; its minimum flange on our press brake is 17.9 mm. - Design with the inside radius from the table above. The outside dimensions and the flat pattern are then correct; the check shows you the expected actual radius. - Keep holes at least as far from the bend line as stated in the design guidelines for each material (column “Hole to bend edge”, at least 2 × sheet thickness + inside radius). The hole then stays round. | Sheet thickness | Steel | Stainless steel | Aluminium | |---|---|---|---| | 0.5 mm | 8 mm | 8 mm | 8 mm | | 0.8 mm | 11.7 mm | 11.7 mm | 8 mm | | 1 mm | 11.7 mm | 11.7 mm | 11.7 mm | | 1.5 mm | 11.9 mm | 11.9 mm | 11.9 mm | | 2 mm | 9.4 mm | 12.1 mm | 12.1 mm | | 2.5 mm | 12.3 mm | 12.3 mm | 12.3 mm | | 3 mm | 17.9 mm | 17.9 mm | 12.5 mm | | 4 mm | 17.9 mm | 20.7 mm | 20.7 mm | | 5 mm | 39.1 mm | 39.1 mm | 20.7 mm | | 6 mm | 39.1 mm | 39.1 mm | 20.7 mm | | 8 mm | Cut-to-size | Cut-to-size | 39.1 mm | Minimum flange (outside dimension) at 90°, measured on our press brake for each die. **Remember:** Need a short flange? Then choose a thinner sheet – the die becomes narrower and the minimum flange shorter. In practice ## Further limits of bending The die is not the only limit. We bend steel S235JR and stainless steel 1.4301 up to 6 mm, aluminium AlMg3 up to 8 mm. Bent parts can be ordered up to 3,000 mm long; less depending on material and sheet thickness, because thick sheet needs more press force (table “Bend length per sheet thickness” in the design guidelines). The smallest opening angle between the flanges is 30°. A hem (180°) is possible up to 2 mm sheet thickness. The angle tolerance is ± 0.5°; the press measures the angle during bending (ACB), typically ± 0.3°. Please request tighter tolerances in the order notes. ## At a glance - Read the minimum flange for each sheet thickness from the table - Design with the measured inside radius from the table - Holes at the table distance from the bend line - Check the bending limit of the material and the maximum bend length [Configure a bent part now →](https://mvg-frankfurt.de/en/bent-parts) ## Matching products [configurator **Bent angle aluminium AlMg3, 2 mm** Flanges 50 × 50 mm, 1,000 mm long – adjust the dimensions, instant price. *Configure a bent part →*](https://mvg-frankfurt.de/en/configurator/bent-parts?form=L&a=50&b=50&t=2&mat=aluminium-almg3&tiefe=1000) · [configurator **Bent angle stainless steel 1.4301, 1.5 mm** Flanges 100 × 40 mm, 200 mm long. *Configure a bent part →*](https://mvg-frankfurt.de/en/configurator/bent-parts?form=L&a=100&b=40&t=1.5&mat=edelstahl-1.4301&tiefe=200) · [Calculators **Bend radius calculator** Inside radius, die and minimum flange per sheet thickness. *Open the calculator →*](https://mvg-frankfurt.de/en/calculators/bend-radius) · [Guidelines **Design guidelines** All check values for holes, webs, flanges and sizes. *Read the guidelines →*](https://mvg-frankfurt.de/en/design-rules#richtlinien) ## Frequently asked questions **How short can a flange be on 3 mm steel?** 3 mm steel runs over the W 24 die; its minimum flange on our press brake is 17.9 mm. **Which inside radius should I design with?** The inside radius from the table: we measured it for each material, sheet thickness and die on our press brake. For 1 to 2.5 mm sheet it lies between 2 and 3.8 mm. The check in the configurator shows the expected value. **Up to which thickness do you bend?** Steel S235JR and stainless steel 1.4301 up to 6 mm, aluminium AlMg3 up to 8 mm. We cut thicker sheets to size but do not bend them. **What happens if a hole is too close to the bend?** It deforms during bending. The check then shows a note that you confirm before ordering. A relief cut into the bend zone is the usual solution. ## Questions about your part? Our sales team advises you on material, manufacturing and delivery time. [Call: (069) 94 21 30 - 0](tel:+496994213000) · [Email info@mvg-frankfurt.de](mailto:info@mvg-frankfurt.de?subject=Question%20about%3A%20Choosing%20the%20right%20bend%20radius%20and%20minimum%20flange) ## Related articles - [Design Preparing bent parts: dimensions, flanges and cut-outs The key questions before configuring an L, U or Z profile. 1 min read Read the article →](https://mvg-frankfurt.de/en/magazine/preparing-bent-parts) - [Design Planning sheet metal trays: clarify shape, corners and use A bent tray can cover, frame or hold. For a suitable design, the corners and the intended use must also be clear. 1 min read Read the article →](https://mvg-frankfurt.de/en/magazine/planning-sheet-metal-trays) - [Design & manufacturing Upload a CAD file, get a price in seconds: no more waiting three days Drawing by email, three days waiting for the quotation, chasing it up: this is still how many people buy sheet metal parts. Why we have done away with it, and what the route from file to part looks like today. 2 min read Read the article →](https://mvg-frankfurt.de/en/magazine/cad-file-instant-price)