Sheet Metal Bending Guidelines: Design Rules for Press Brake Parts
Release time: 2026-08-05
Key Design Considerations for Press Brake Parts
These sheet metal bending guidelines explain the minimum flange lengths, hole-to-bend clearances, bend reliefs, Z-bend limits, inside radii, acute bends, hems, and tooling restrictions that should be checked before press brake production. Use the tables as practical design references and confirm final values against the selected material, sheet thickness, tooling, and machine capacity.
Minimum Flange Length
Tooling imposes minimum dimensional limits that must be considered to ensure that a bent part can be manufactured. If a flange is too short for the required lower die, the specified bend cannot be produced. Actual limits may vary depending on the part geometry and bend length.
For an initial estimate of the required bending force and V-die opening, use the press brake bending calculator.
| Sheet Thickness (s) | x for Bend Angle ≥ 90° (w) | x for Bend Angle < 90° (w) |
|---|---|---|
| 0.5 mm | 5 mm | 8 mm |
| 0.8 mm | 5 mm | 10 mm |
| 1 mm | 5.5 mm | 10 mm |
| 1.5 mm | 9 mm | 10.5 mm |
| 2 mm | 9.5 mm | 13 mm |
| 2.5 mm | 12 mm | 15.5 mm |
| 3 mm | 14 mm | 22 mm |
| 4 mm | 18.5 mm | 23 mm |
| 5 mm | 24 mm | 30 mm |
| 6 mm | 30 mm | 38 mm |
| 8 mm | 38 mm | 45 mm |
| 10 mm | 45 mm | 59 mm |
| 12 mm | 59 mm | 88 mm |
| 15 mm | 88 mm |
| Sheet Thickness (s) | x for Bend Angle ≥ 90° (w) | x for Bend Angle < 90° (w) |
|---|---|---|
| 0.5 mm | 5 mm | 8 mm |
| 0.8 mm | 5 mm | 10 mm |
| 1 mm | 5.5 mm | 10 mm |
| 1.5 mm | 9 mm | 10.5 mm |
| 2 mm | 9.5 mm | 13 mm |
| 2.5 mm | 12 mm | 15.5 mm |
| 3 mm | 15.5 mm | 22 mm |
| 4 mm | 22.5 mm | 27 mm |
| 5 mm | 30 mm | 38 mm |
| 6 mm | 38 mm | 43 mm |
| 8 mm | 43 mm | 57 mm |
| 10 mm | 57 mm | 72 mm |
| 12 mm | 72 mm | |
| 15 mm | 104 mm |
Minimum Distance Between Internal Contours and the Bend Line
Holes or cut-outs positioned too close to a bend line may distort during forming. A sufficient clearance must therefore be maintained.
The minimum distance to the bend is the same as the minimum flange length specified above. In the minimum-flange diagram, dimension x represents the distance from the bend line to the nearest edge of the contour.
If holes or contours must remain close to the bend for functional reasons, bend reliefs can be incorporated into the design as described in the following section. Distortion caused by an insufficient design clearance cannot be controlled reliably.
Bend Reliefs
If the minimum hole-to-bend distance cannot be maintained, bend reliefs can be added to prevent holes or cut-outs near the forming zone from distorting. The following points should be considered when designing bend reliefs:
- Sufficient material must remain in the bend zone to maintain the structural stability of the part.
- Sharp-edged cut-outs, such as rectangles with square internal corners, can initiate cracking because the material is locally weakened at the corners.
- The preferred bend-relief geometry is a rectangular cut-out with rounded corners.
Minimum Distance Between External Contours and the Bend Line
If a part contains tapered flanges or other external contours close to the bend line, the same rules used for minimum flange length apply.
Where the external contour reduces the available flange below the minimum length, the material is no longer fully supported by the lower die. This area may distort during bending or may not be formed completely.
There are three ways to prevent this condition:
- Remove the bend from the critical area.
- Extend the critical area to meet the minimum flange-length requirement.
- Add a relief cut so the critical area is excluded from the bend.
Minimum Z-Bend Height
For two consecutive bends forming a Z-profile, the tooling requires the following minimum step heights.
| Sheet Thickness (s) | x for Bend Angle ≥ 90° (w) | x for Bend Angle < 90° (w) |
|---|---|---|
| 1 mm | 11.5 mm | 18.5 mm |
| 1.5 mm | 12.5 mm | 19.5 mm |
| 2 mm | 15 mm | 20.5 mm |
| 2.5 mm | 20 mm | 26 mm |
| 3 mm | 24.5 mm | 35 mm |
| 4 mm | 30 mm | 35.5 mm |
| 5 mm | 36 mm | 44 mm |
| 6 mm | 46 mm | 58 mm |
| 8 mm | 59 mm | 72 mm |
| 10 mm | 70 mm | 86 mm |
| 12 mm | 98 mm | |
| 15 mm | 128 mm |
| Sheet Thickness (s) | x for Bend Angle ≥ 90° (w) | x for Bend Angle < 90° (w) |
|---|---|---|
| 1 mm | 11.5 mm | 19 mm |
| 1.5 mm | 13.5 mm | 20 mm |
| 2 mm | 18 mm | 26.5 mm |
| 2.5 mm | 24 mm | 32.5 mm |
| 3 mm | 26 mm | 36 mm |
| 4 mm | 36 mm | 53 mm |
| 5 mm | 43.5 mm | 53 mm |
| 6 mm | 53.5 mm | 63.5 mm |
| 8 mm | 65.5 mm | 78 mm |
| 10 mm | 92 mm | |
| 12 mm | 109 mm | |
| 15 mm | 181 mm |
Maximum Flange Length
Tool Collision with U-Profiles
If the flanges are too long or the designed U-profile is too narrow, the workpiece may collide with the upper tool or upper beam. The achievable dimensions for U-profiles depend on the available tool and beam clearances.
For material thicknesses of 6 mm and above, part size and geometry may require a straight punch instead of a gooseneck punch.
Available working lengths, control configurations, and tooling options can be reviewed on the CNC press brake machine page.
Horn Tools
Tools with lateral horn extensions make it possible to form concealed bend lines in closed-frame components. The concealed section of the bend must not exceed 32 mm, and sufficient vertical clearance must be provided for the horn.
Press Brake Bend Radius
- The stated values may vary significantly depending on the tooling used.
- The resulting inside bend radius is determined primarily by the selected lower die. The punch radius normally has only a limited influence.
- The inside bend radius may vary with the material batch, tooling condition, and part geometry.
- Unless specifically agreed before production, modelled radii may be adjusted automatically to a radius within the achievable range shown below.
Bend Radii for 90° Bends
| Sheet Thickness (t) | Upper-Tool Radius | V-Die Opening | Inside Bend Radius |
|---|---|---|---|
| 0.5 | 0.5-1 | 4-8 | Approx. 0.5-1.7 |
| 0.8 | 0.5-1 | 4-12 | Approx. 0.8-2.5 |
| 1 | 1 | 6-12 | Approx. 1.0-2.5 |
| 1.5 | 1 | 6-16 | Approx. 1.5-3.4 |
| 2 | 1-2 | 10-20 | Approx. 2.0-4.2 |
| 2.5 | 1-2.5 | 12-24 | Approx. 2.5-5.0 |
| 3 | 1-3 | 16-30 | Approx. 3.0-6.3 |
| 4 | 1-4 | 20-40 | Approx. 4.0-8.0 |
| 5 | 1-5 | 30-50 | Approx. 5.0-10.1 |
| 6 | 1-6 | 30-60 | Approx. 6.0-11.8 |
| 8 | 4-8 | 50-90 | Approx. 10.2-18.1 |
| 10 | 4-10 | 70-120 | Approx. 14.0-24.2 |
| 12 | 5-10 | 80-120 | Approx. 15.8-24.4 |
| 15 | 6-10 | 90-120 | Approx. 17.9-24.1 |
| Sheet Thickness (t) | Upper-Tool Radius | V-Die Opening | Inside Bend Radius |
|---|---|---|---|
| 0.5 | 0.5-1 | 4-8 | Approx. 0.5-1.8 |
| 0.8 | 0.5-1 | 4-12 | Approx. 0.8-2.6 |
| 1 | 1 | 6-12 | Approx. 1.0-2.7 |
| 1.5 | 1 | 6-16 | Approx. 1.5-3.7 |
| 2 | 1-2 | 10-20 | Approx. 2.0-4.6 |
| 2.5 | 1-2.5 | 12-24 | Approx. 2.5-5.7 |
| 3 | 1-3 | 16-30 | Approx. 3.0-7.0 |
| 4 | 1-4 | 20-40 | Approx. 4.0-9.0 |
| 5 | 1-5 | 30-50 | Approx. 7.3-11.2 |
| 6 | 1-6 | 30-60 | Approx. 7.2-13.6 |
| 8 | 4-8 | 50-90 | Approx. 12.2-19.9 |
| 10 | 4-10 | 70-120 | Approx. 16.1-26.6 |
| 12 | 4-10 | 80-120 | Approx. 18.5-27.3 |
| 15 | 4-10 | 90-120 | Approx. 21.0-27.8 |
| Sheet Thickness (t) | Upper-Tool Radius | V-Die Opening | Inside Bend Radius |
|---|---|---|---|
| 0.5 | 0.5-1 | 4-8 | Approx. 1.3-2.1 |
| 0.8 | 0.5-1 | 4-12 | Approx. 1.2-3.0 |
| 1 | 1 | 6-12 | Approx. 1.6-3.0 |
| 1.5 | 1 | 6-16 | Approx. 1.6-4.0 |
| 2 | 1-2 | 10-20 | Approx. 2.6-5.0 |
| 2.5 | 1-2.5 | 12-24 | Approx. 2.8-5.9 |
| 3 | 1-3 | 16-30 | Approx. 3.8-7.5 |
| 4 | 1-4 | 20-40 | Approx. 4.6-19.6 |
| 5 | 1-5 | 30-50 | Approx. 6.9-12.0 |
| 6 | 1-6 | 30-60 | Approx. 6.9-14.1 |
| 8 | 4-8 | 50-90 | Approx. 12.0-21.6 |
| 10 | 4-10 | 70-120 | Approx. 16.1-29.6 |
| 12 | 5-10 | 80-120 | Approx. 21.9-29.1 |
| 15 | 6-10 | 90-120 | Approx. 20.4-28.5 |
Bend Angles Below 90°
The following processing requirements apply to sheet metal bends with an included angle below 90°:
- For sheet thicknesses up to 5 mm, a bending die with a maximum included opening angle of 30° is recommended.
- For sheet thicknesses of 6 mm and above, bending dies with an included opening angle of 60-80° should be used.
- Acute cracking may occur in material 3 mm thick and above, particularly at smaller bend angles.
- Narrow bend tabs increase the risk of cracking.
- This problem can occur in aluminium at even lower material thicknesses.
| Bend Angle < 90° | Carbon Steel Thickness | Stainless Steel Thickness | Aluminium Thickness |
|---|---|---|---|
| < 30° | – | – | – |
| 30-35° | Up to 2.0 mm | Up to 2.0 mm | – |
| 35-40° | Up to 4.0 mm | Up to 4.0 mm | Up to 2.0 mm |
| 40-45° | Up to 6.0 mm | Up to 6.0 mm | Up to 2.5 mm |
| 45-60° | Up to 8.0 mm | Up to 8.0 mm | Up to 2.5 mm |
| 60-80° | No specified limit | No specified limit | Up to 5.0 mm |
Sheet Metal Hems (180°)
The following requirements apply to 180° hems:
- The maximum material thickness for this type of bend is 2 mm.
- The hem must be designed with a 0.2 mm gap. However, this gap will be closed during the manufacturing process.
Minimum Hem Lengths for Different Sheet Thicknesses
| Sheet Thickness (s) | x for Bend Angle < 90° (w) |
|---|---|
| 0.5 mm | 10 mm |
| 0.8 mm | 10 mm |
| 1 mm | 10 mm |
| 1.5 mm | 10.5 mm |
| 2 mm | 13 mm |
The maximum hem width is limited to 1500 mm.
Sheet Metal Bend Relief Cuts
Laser-cut features have a minimum achievable width and must be represented correctly in the CAD file. Cut lines at the end of a bend should be designed as bend reliefs. A small cut-out can be added to the drawing, or a corner-relief option can be specified. Without sufficient separation between adjacent bend zones, the material may continue tearing along the cut.
Reliefs Adjacent to Bends
Reliefs next to a bend must have a minimum width and depth equal to the material thickness. Sufficient clearance must be maintained around the bend to permit accurate forming while preserving part stability.
Corner Reliefs
Corner reliefs must extend at least 1 mm beyond the bend zone in each direction. This additional length provides sufficient forming clearance and may need to be increased for thicker material.
Minimum Clearance Between Overlapping Tabs
A minimum clearance of 0.2 mm must be provided between two overlapping tabs to ensure correct calculation and reliable manufacturing.
If existing equipment cannot meet the required tooling clearance, bending accuracy, or automation level, review the available press brake upgrade solutions before changing the component design.
