Most press brake problems start on the drawing board, not on the machine. A flange that is too short, a hole too close to a bend or a missing relief cut can make a part impossible to bend accurately, however good the equipment is. This CNC press brake bending design guide covers the rules of thumb that help sheet metal parts bend cleanly, repeatably and at a sensible cost.
In air bending, the most common press brake method, the inside radius is set mainly by the width of the V-die opening rather than by the punch tip. As general guidance, the V opening for mild steel is often chosen at around six to eight times the material thickness, and the inside radius that forms is roughly one sixth of that opening. For most mild steel work, designing with an inside radius close to the material thickness is therefore a safe starting point.
Stainless steel springs back more and usually forms a slightly larger radius. Harder aluminium grades can crack if bent too tightly and need a larger radius, often several times the thickness, while softer grades bend easily. Ask your fabricator which radius their tooling produces in your material and use that value on the drawing, instead of a sharp corner that cannot be formed.
Sheet has a rolling direction. Bends made across the grain, with the bend line perpendicular to the rolling direction, are less likely to crack than bends running parallel to it. This matters most for aluminium, thicker hot-rolled steel and tight radii. If a part has bends in two directions, orient the most critical bend across the grain and mark grain direction on the drawing when it matters.
A flange must stay supported across both shoulders of the V-die throughout the bend. If it is too short, it slips into the die, the bend comes out uneven and the part may be marked. A widely used rule of thumb is that the minimum flange length is about four times the material thickness plus the inside bend radius.
If the design needs a shorter flange, the options are to bend a longer flange and trim it afterwards, use a narrower V-die (which tightens the radius and raises the bending force), or rethink the joint. Very short return flanges and hems should be discussed with the fabricator before the design is frozen.
Features placed too close to a bend line are pulled out of shape as the material stretches: round holes turn oval and slots narrow or bulge. A common guideline is to keep the edge of any hole or slot at least two to three times the material thickness plus the bend radius away from the bend line. If a feature must sit closer, it can be cut after bending, or a relief slot can be cut along the bend line to isolate it.
When a bend line runs into an uncut edge, or two bends meet at a corner, the material has nowhere to go and it tears or bulges. A bend relief, a small notch at the end of the bend line, prevents this. As general guidance:
Reliefs are cut into the flat blank during laser cutting, so adding them at the design stage costs almost nothing.
When sheet metal bends, the inside compresses and the outside stretches. Between them lies the neutral axis, which keeps its original length. The K-factor gives the position of this axis as a fraction of thickness: the distance from the inside face to the neutral axis divided by the thickness. Typical values fall between about 0.3 and 0.5, depending on material, radius and bending method.
The K-factor is used to calculate the bend allowance, the length of material taken up by each bend:
Bend allowance = (π / 180) × bend angle in degrees × (inside radius + K × thickness)
The flat blank length is the sum of the straight segments plus the bend allowances. CAD software does this automatically, but only as accurately as the K-factor entered, and a generic value can leave a multi-bend part slightly long or short. It is best to share the 3D model and let the fabricator develop the flat pattern with values proven on their own tooling. Our CAD drafting and sheet metal development service prepares flat patterns from a 3D model, a 2D drawing or a physical sample.
A part that looks fine in CAD may not be bendable in practice. Bends are formed one after another, and each previously bent flange must clear the punch, die and machine frame. Deep U-channels, closed boxes and short flanges between two bends are the usual trouble spots. Check that a channel is wide enough for the punch to enter and that return flanges will not hit the punch or ram.
On the drawing:
Tolerances tighter than the process can hold economically lead to extra inspection, rework or rejections without making the part work any better.
| Design point | General rule of thumb | Effect if ignored |
|---|---|---|
| Inside bend radius | About 1 x thickness for mild steel; larger for stainless steel and hard aluminium | Cracking or inconsistent radius |
| Minimum flange length | About 4 x thickness + inside radius | Flange slips into the die, uneven bend |
| Hole or slot near a bend | Edge at least 2 to 3 x thickness + radius from the bend line | Holes go oval, slots distort |
| Bend relief | Width at least thickness, depth about thickness + radius | Tearing or bulging at corners |
| Grain direction | Bend across the rolling direction where possible | Cracks on the outside of the bend |
| Flat pattern | Developed with the fabricator's own K-factor | Overall size too long or short |
| Dimensioning | Single datum, inside or outside stated | Tolerance stack-up, disputes at inspection |
Vidhee Eng. Works carries out CNC press brake bending, laser cutting and flat-pattern development in-house at New GIDC, Kabilpore, Navsari, under an ISO 9001:2015 certified quality management system, and dispatches parts across India by road. If you are unsure whether a design will bend as drawn, send us your drawing or 3D model and we can review radii, flanges and reliefs with you before production.
Send your drawing, material and quantity to Vidhee Eng. Works, Navsari, and get a clear quotation with a delivery date.
For mild steel, an inside radius close to the material thickness is a safe general starting point in air bending. Stainless steel tends to form a slightly larger radius, and harder aluminium grades need a larger radius to avoid cracking. Because the radius depends on the V-die used, confirm the value with your fabricator and show it on the drawing.
A common rule of thumb is about four times the material thickness plus the inside bend radius. Shorter flanges tend to slip into the V-die, which gives uneven bends and marks on the part. If the design needs a shorter flange, it can sometimes be bent longer and trimmed, or formed with a narrower die, but discuss it with the fabricator first.
K-factor describes where the neutral axis sits within the material thickness during bending, measured as a fraction from the inside face. It is used to calculate the bend allowance and therefore the size of the flat blank. Typical values lie between about 0.3 and 0.5. Using a value that matches the fabricator's tooling gives more accurate flat patterns.
Send the 3D model, ideally as a STEP file, together with a 2D drawing showing critical dimensions and tolerances. The fabricator can then develop the flat pattern using bend values proven on their own tooling. A flat pattern made with a generic K-factor can cause finished dimensions to drift on parts with several bends.
Share your material, thickness and quantity — we’ll review it and come back with a quote and a delivery date, not just a price.
