Key takeaways
- Minimum outside flange is V/2 + t, so the die opening, not the flange, is the variable to choose: 3 mm sheet on a 12 mm V needs 9 mm of flange and on a 24 mm V needs 15 mm.
- Keep V between 4t and 12t. Below 4t the punch load and die marking become the limit; above 12t the inside radius grows and the angle gets harder to hold.
- On 3 mm mild steel an 8 mm V needs 559 kN/m of bend force, which limits a 200 T brake to 3.58 m of bend; a 16 mm V halves the force and lets the full 4,450 mm bed work.
- Dropping from a 16 mm to an 8 mm V on 3 mm sheet grows the flat pattern by 0.56 mm per bend, so a die change at quotation is a drawing change.
A 3 mm bracket with an 8 mm return flange is a common drawing. The flange is formable only on a 10 mm V die, which on 3 mm sheet is 3.3 times the thickness — inside the range where punch load and die marking, not geometry, decide whether the part can be made.
Minimum flange for sheet metal follows one rule, V/2 + t, where V is the die opening and t the thickness. The rule is easy. The decision behind it is not, because the die opening also sets the inside radius, the force per metre, the flat length and the maximum bend length the press can run. Choose V for the flange and four other numbers move.
This page is about choosing the opening. The general flange rule, punch clearance and tall-flange limits are covered in minimum flange length for press brake parts; here the question is which V to put in the machine.
What sets the minimum flange for sheet metal, and which V can you run?
The geometric minimum is V/2 + t: the flange edge must reach the far die shoulder while the bend line sits over the centre of the opening. On 3 mm sheet a 16 mm V gives 11 mm minimum outside flange; a 12 mm V gives 9 mm; a 24 mm V gives 15 mm.
The usable range is narrower than the geometry suggests. Production practice keeps V between about 4t and 12t. Below 4t the force per metre climbs steeply, the die shoulders mark the outside of the bend, and the inside radius falls below one thickness, which is where cracking starts in mild steel. Above 12t the inside radius grows faster than the bend allowance models assume, the angle becomes harder to hold, and the flange has to be longer anyway.
So the flange question reduces to: what is the narrowest V at or above 4t, and does the part's force fit inside the press? On 3 mm sheet that floor is a 12 mm opening, which sets 9 mm as the shortest flange available from standard tooling.
Choosing the opening in four steps
- Set the floor: V must be at least 4t. For 3 mm sheet that is 12 mm; for 2 mm sheet, 8 mm.
- Set the ceiling: V should stay under about 12t unless the drawing wants a large radius. For 3 mm sheet that is 36 mm.
- Check the flange: the shortest outside flange on the part must be at least V/2 + t for the chosen opening.
- Check the force: force per metre multiplied by the bend length must stay inside both the press rating and the tool's rated load per metre.
Steps 1 and 3 pull in opposite directions, and step 4 usually decides. A part that fails step 3 needs a wider flange or a different feature; a part that fails step 4 needs a shorter bend, a wider opening or a second pass.
Die opening, flange and force on 3 mm mild steel
The table is calculated for 350 MPa tensile strength, air bending, 90° bends, using F = 1.42 × σb × t² / (1,000 × V) in kN per metre and a 200 T press with a 4,450 mm bed. Inside radius follows the air-bend approximation Ri ≈ 0.16V.
| Die opening V | V/t | Minimum outside flange | Inside radius | Force per metre | Maximum bend length at 200 T | Ganesh note |
|---|---|---|---|---|---|---|
| 8 mm | 2.7 | 7 mm | 1.3 mm | 559 kN/m | 3.58 m | Below the 4t floor; tool rating and marking risk |
| 10 mm | 3.3 | 8 mm | 1.6 mm | 447 kN/m | 4.47 m | Bed limit is 4,450 mm, so no force margin at full length |
| 12 mm | 4.0 | 9 mm | 1.9 mm | 373 kN/m | 4,450 mm bed | Narrowest standard opening for 3 mm |
| 16 mm | 5.3 | 11 mm | 2.6 mm | 280 kN/m | 4,450 mm bed | Usual choice for 3 mm brackets |
| 24 mm | 8.0 | 15 mm | 3.8 mm | 186 kN/m | 4,450 mm bed | Better angle control, longer flange |
| 32 mm | 10.7 | 19 mm | 5.1 mm | 140 kN/m | 4,450 mm bed | Radius may be too large for the design |
| 48 mm | 16.0 | 27 mm | 7.7 mm | 93 kN/m | 4,450 mm bed | Outside the 12t range; angle drift |
Two readings matter. The flange column answers the drawing question, and the force column answers the production question: at 8 mm the brake cannot run a full 4,450 mm bend, and at 10 mm it can only just, with no margin for ram deflection. The length limit is not a machine setting — it is arithmetic on the tool.
Why force per metre decides more than tonnage
The formula scales with the square of thickness and inversely with the opening. Double the thickness and the force quadruples; double the opening and it halves. That is why a single short flange on a 3 mm part can force a die change on the whole job.
A 200 T press delivers 2,000 kN. Divide by the force per metre and you get the length that can be bent in one stroke:
- 8 mm V on 3 mm: 2,000 ÷ 559 = 3.58 m.
- 12 mm V on 3 mm: 2,000 ÷ 373 = 5.36 m, capped at the 4,450 mm bed.
- 16 mm V on 3 mm: 2,000 ÷ 280 = 7.14 m, capped at the bed.
The 4,450 mm bed and the 200 T rating cross over at about 449 kN/m, which corresponds to a 10 mm opening on 3 mm mild steel. Narrower than that and the press runs out of force before it runs out of bed. That is the honest constraint on a short flange: it is not only a tooling question, it is a capacity question for long parts.
The tensile strength in the formula is the coil's, not a handbook constant. ISO 6892-1 defines how tensile properties are measured; a 450 MPa HSLA coil needs 1.29 times the force of a 350 MPa CRCA coil at the same opening. On a part already near the limit, the grade decides whether it forms.
The four numbers a narrower V changes at once
Change the opening and the part changes in four places. Work through them before accepting a flange redesign.
The inside radius falls. Ri ≈ 0.16V, so a 16 mm opening gives about 2.6 mm on 3 mm sheet and an 8 mm opening gives about 1.3 mm. The 1.3 mm radius is 0.43t, close to the cracking limit for CRCA and beyond it for some aluminium grades.
The flat pattern grows. With K = 0.44, a 90° bend at 2.6 mm radius has an allowance of π × (2.6 + 1.32) / 2 = 6.16 mm and a deduction of 2 × (2.6 + 3) − 6.16 = 5.04 mm. At 1.3 mm radius the allowance is π × (1.3 + 1.32) / 2 = 4.12 mm and the deduction is 2 × (1.3 + 3) − 4.12 = 4.48 mm. The flat grows by 0.56 mm per bend, so a four-bend part grows 2.2 mm. If the flat pattern was released with the drawing, it is now wrong.
The bend length available falls. The table above shows the 8 mm opening capping the press at 3.58 m, so a 4,000 mm part cannot be formed in one pass on that die.
The face marks. A narrower opening concentrates the same force on a smaller shoulder contact area, which is why a part with a cosmetic face on the die side needs a wider opening, a polished shoulder or a protective film.
Short flanges that standard tooling cannot form
Five options exist, and one of them is usually right.
Take the 8 mm flange on 3 mm CRCA that opened this page. The 4t floor says a 12 mm V, which needs 9 mm of flange, so the drawing misses by 1 mm. A 10 mm opening gets there at 8 mm, but it runs at 447 kN/m, which caps the press at 4.47 m — right at the bed limit, with nothing left for a long part. That is the trade in a single part: 1 mm of flange against the entire force margin of the machine.
An acute tool — a 30° punch and die set — lets a flange sit inside the V rather than on the shoulders, so a 6 mm flange on 3 mm sheet can form without forcing the opening below 4t. The angle needs a matched punch and die pair, and the tonnage is higher than the angle suggests.
A joggle or offset turns the short flange into a step. Two small bends replace one, the flat face stays flat, and the step dimension is easier to hold than a 6 mm return.
A relief notch at the bend line lets the flange form without dragging the adjacent wall, which is the usual reason a short flange tears at its end.
A different bend sequence can make the flange the last operation, so the punch enters an open shape rather than a closed box.
A welded strip replaces the bend entirely. It works, it costs a weld, a fixture and a straightening operation, and it turns a press tolerance into an assembly tolerance.
The bad option is to specify the flange and leave the tool to the supplier without a note. Tryout on an unformable flange consumes a die set and a first batch, and the correction that comes back is the one available at quotation.
How Ganesh bends a short flange
Bending runs on a 200 T, 5-axis CNC press brake with a 4,450 mm bed and Delem control, working to 10 mm thickness. The 5-axis control compensates the ram and the back gauge along the bed, which is what keeps the angle on a long part when the die opening has been chosen tight.
Special punches and dies for a short flange come from the in-house tool room, which also builds press tools, progressive dies, welding fixtures and checking fixtures. That matters when the answer is an acute tool rather than a standard one: the tool is designed against the part, not selected from a catalogue and hoped for.
Custom parts run from 0.8 mm to 40 mm at ±0.5 mm typical sheet metal tolerance, with tighter features agreed against the drawing. Manufacturing has run since 1992 across five units in Mumbai (Vasai) and Nagpur, under ISO 9001:2015 and ISO 14001:2015, with first article inspection standard and PPAP available.
What to put on the drawing
- Outside or inside flange dimensions, stated once, with the convention named.
- Inside radius, or a note that the radius follows the tool. A radius below one thickness in mild steel is a material decision, not a tooling one.
- Bend line position from a datum edge, so the flat can be derived consistently.
- The flange that must not move, marked, so the supplier knows which bend is critical when the die is chosen.
- Grade and thickness, because the force calculation depends on both.
- The cosmetic face, so the die shoulder does not mark it.
- The flat pattern, marked reference only, since the die opening governs the deduction.
The press brake tool selection page covers how the punch and die pair is chosen once the opening is fixed, and minimum bend radius by material covers the radius limit that a narrow V approaches. Both sit alongside the bending capability page, which lists the brake, the bed and the thickness range, and the design and CAD hub indexes the drawing guides.
When a short flange should not be a bend at all
Below about 2t there is no standard tooling that will form the flange on a production basis, and below 1.5t even acute tools struggle. At that point the geometry has to change: a joggle, a hem, a folded edge or a welded strip.
A hem is a different process with a different tool, and it is not a bend with a tight radius. Ganesh does not run a dedicated hemming line, so a hemmed edge is a design decision to confirm before quotation rather than a note on a bend.
Above 10 mm the brake is outside its range here, and heavy plate is cut and welded instead. A short flange on 12 mm plate is a machining or welding problem.
If the flange is the only feature that does not fit, request a quote with the bend lines marked. The engineering team will say whether the die, the tool or the geometry has to change, and what each option does to the flat pattern.
Frequently asked questions
What is the minimum flange for 3 mm sheet metal?
About 9 mm outside on a 12 mm V die, which is 4t and the narrowest opening normally used on 3 mm. A 24 mm V needs 15 mm. A shorter flange needs an acute tool, a joggle or a welded strip rather than a narrower die.
Can I use a 6 mm die opening on 3 mm sheet?
Geometrically yes, and it allows a 6 mm flange, but it needs 746 kN/m of bend force on mild steel and it is below the 4t floor where die marking and punch loading become the constraint. Standard tooling is not rated for that combination on a production basis.
Does a narrower die opening change the flat pattern?
Yes. A narrower V produces a smaller inside radius, which lowers the bend deduction and lengthens the flat. On 3 mm sheet, moving from a 16 mm to an 8 mm V adds about 0.56 mm of flat length per 90° bend.
How does die opening affect the bend length I can run?
Through force. F = 1.42 x tensile strength x t squared / (1000 x V) kN per metre. On a 200 T brake that gives 3.58 m at an 8 mm V on 3 mm steel and the full 4,450 mm bed at 16 mm. Narrow dies cost length as well as tonnage.
What is the difference between minimum flange and minimum bend radius?
The flange is a die-shoulder constraint measured from the bend line to the free edge; the radius is a material constraint on the inside of the bend. A flange of 9 mm on 3 mm sheet can still fail if the drawing asks for a 1 mm inside radius.
Sources and further reading
- ISO 2768-1 — General tolerances for linear and angular dimensions where the drawing gives no individual tolerance · reviewed 3 Nov 2026
- IS 513 Part 1 — Cold reduced carbon steel sheets and strips, the grade and property basis for the bend force calculation · reviewed 3 Nov 2026
- ISO 6892-1:2019 — Metallic materials: tensile testing at room temperature, which gives the tensile strength used in the tonnage formula · reviewed 3 Nov 2026
Have a flange that is too short for the tool?
Send the drawing with the bend lines and the flange heights. We check each bend against the die set and the punch load, and tell you whether the answer is a different die, an acute tool or a design change.
Request a quote