Sheet Metal Bend Allowance and Press Tonnage

Sheet Metal Bending

Sheet Metal Bending: Bend Allowance, Springback, Press Tonnage and Layout Rules

Scope

The tool lays out a straight-bend sheet-metal part (an angle, channel, Z, hat or box side) in the flat: for every bend it gives the setback, bend allowance and bend deduction, for every flange the flat it leaves, and for the part the total developed width to cut. It then estimates the springback of each bend and the die angle to overbend to, checks the inside radius against the minimum for the alloy, works out the press-brake force for air bending (with bottoming and coining multiples), the die opening, the radius an air bend forms, the shortest flange the die can hold, the distance a hole or slot must keep from the bend, the relief hole where two bends meet, and the blanking or punching force with stripping. The methods are those of the FAA airframe handbook and advisory circular, which are U.S. government works, with the closed forms of the press and springback relations; every shop rule is an entered number whose default is stated as illustrative.

Bend geometry

A bend is described by its inside radius R, the sheet thickness t and the angle θ the sheet is bent through (FAA-H-8083-31B: 180° minus the angle between the flanges; 90° for a square corner, less for an open bend, more for a closed one). The outside surfaces of the two flanges, extended, meet at the mold point; a flange's mold line dimension is measured from mold point to mold point, or to the sheet edge. The metal starts to curve at the bend tangent lines, which sit a setback SB back from the mold point: SB = tan(θ/2)(R + t) on the outside mold line (tan(θ/2) R on the inside). The handbook calls tan(θ/2) the K-factor and tabulates it from 1° to 180° (Figure 4-122; 1.000 at 90°, 0.41421 at 45°, 2.4142 at 135°); the tool names it the setback factor to keep it apart from the neutral-axis K below.

Bend allowance and the K-factor

Between the tangent lines the metal follows an arc. The fibres on the inside are compressed and those on the outside stretched; one fibre, the neutral axis, keeps its length, and that length is the bend allowance BA, the material the bend consumes. If the neutral axis sits K t from the inside surface, BA = θ (R + K t) with θ in radians. The handbook gives two forms: formula 1 puts the neutral axis at mid-thickness, BA = 2π(R + t/2)/4 for 90° (its example: R = 1/4 in, t = 0.051 in gives 0.4327 in), and formula 2, the empirical aircraft rule BA = (0.01743 R + 0.0078 T) N for N degrees, which is θ(R + 0.4475 t) with the per-degree constant 0.01743 in place of π/180 = 0.017453 (0.13 percent low); the handbook's Figure 4-128 chart of 90° and per-degree allowances for 19 thicknesses and 14 radii is formula 2 evaluated, and the handbook puts the neutral axis at 0.445 t. The tool offers formula 2 as printed, the mid-thickness value K = 0.5, an entered K, or a piecewise rule table of K against R/t; the default table (0.33 for R/t up to 0.5 rising to 0.5 beyond 4 t) is a common shop rule, not a published table, and should be replaced by measured values for the material and tooling. The bend deduction BD = 2 SB − BA is what the sum of the mold line dimensions exceeds the flat by.

Flat pattern

Each flange's flat is its mold line dimension less the setbacks of the bends at its ends (one setback for the first and last flange, two for the others); the total developed width is the sum of the flats and the bend allowances, equivalently the sum of the flange dimensions less the bend deductions. The handbook's U-channel example (0.040-in 2024-T3, R = 0.16 in, flanges 1, 2 and 1 in, two 90° bends) gives setback 0.2 in, flats 0.8, 1.6 and 0.8 in, bend allowance 0.27 in and a developed width of 3.74 in, less than the 4 in of mold line dimensions, which is the check to make: a flat longer than the sum of the flange dimensions is a sign of an error. The tool reproduces that example, the handbook's 45° and 135° bends and its 60° L-bracket in its test script. The flanges may instead be dimensioned to the inside mold lines, in which case the inside setback tan(θ/2) R is used.

Springback

On unloading the bend recovers elastically: the angle opens and the radius grows. For an elastic-perfectly-plastic sheet bent to an inside radius R_i the recovery follows from the moment carried by the partly yielded section, M = (S_y t²/4)[1 − (1/3)(2 S_y R_i/(E t))²], unloaded elastically, 1/R_f = 1/R_i − M/(E I) with I = t³/12 per unit width, which is Gardiner's relation R_i/R_f = 4x³ − 3x + 1 with x = R_i S_y/(E t). At x = 1/2 the ratio is zero: the sheet is not yielded through and springs back flat. The neutral-axis arc keeps its length, so θ_f (R_f + t/2) = θ_i (R_i + t/2) and the springback factor is K_s = θ_f/θ_i = (2R_i/t + 1)/(2R_f/t + 1); to leave θ the die bends to θ/K_s. The relation uses the inside radius as the thin-sheet form of the neutral-axis radius and ignores strain hardening, which raises the unloading moment, so it understates the springback of a work-hardening alloy; the handbook's cornice-brake rule of thumb, a 90° setting giving 87° to 88° in aluminum, is the order of magnitude. The tool's test script checks the closed form against a fibre-by-fibre integration of the stress distribution.

Minimum bend radius

Too sharp a bend cracks the outside fibres. AC 43.13-1B Table 4-6 lists the recommended radii for 90° bends in aluminum alloys as multiples of t for sheet thicknesses from 0.016 to 0.258 in: nothing for annealed tempers, 1.5 t to 3 t for 0.016-in 2024-T3 rising to 5 t to 7 t at 0.258 in, 2 t to 4 t for thin 7075-T6 rising to 6 t to 10 t. The tool takes the band at or above the entered thickness and the upper end of the range as the minimum; Alclad bends slightly tighter and 2024-T3 bends tighter immediately after quenching (the table's notes). For other materials an entered multiple is used (annealed sheet bends to about its thickness, FAA-H-8083-31B p. 4-61).

Press-brake force

Air bending over a V-die of opening V loads the sheet as a strip in three-point bending. The fully plastic moment of a strip of width L is M_p = S_u L t²/4 and the central load that produces it over the span V is F = 4 M_p/V = S_u L t²/V, the plastic hinge; the charted press-brake formula F = k S_u L t²/V with k = 1.33 adds strain hardening and die friction, and the elastic limit (2/3) S_y L t²/V is the load below which the sheet would spring back flat. The die opening follows the shop rule V = 8 t (6 t for thin sheet, 10 to 12 t for thick plate), and an air bend forms an inside radius of about V/6 to V/8 whatever the punch radius, which is why the formed radius is entered as a fraction of V and compared with the radius in the bend table. Bottoming (the sheet pressed to the die angle) and coining (the sheet squeezed between punch and die) take several times the air-bend force; the multiples are entered, the defaults of 3 and 8 being illustrative of press-brake makers' guidance. The tool prints the force in the force unit of the dropdown and in U.S. short tons and metric tonnes, applies an entered capacity factor and reports the margin against the entered press capacity as a plain ratio.

Minimum flange and features

At the bottom of the stroke the two legs are inclined at θ/2 and each must still reach the die shoulder, a half-span V/2 measured along the leg: the shortest flange is L_min = V/(2 cos(θ/2)) plus an allowance for the die shoulder radius, 0.5 V for a shallow bend and 0.707 V at 90°, which is the 0.7 V of the makers' charts. A hole or slot inside the bend zone distorts; the shop rules keep its edge at least 2 t (holes) or 2.5 t (slots) from the bend tangent line on the flat pattern, both entered. Where two bends meet, a relief hole at the intersection of the inside bend tangent lines keeps the corner from tearing: FAA-H-8083-31B p. 4-72 makes its diameter the bend radius, not less than 1/8 in for sheet up to 0.064 in or 3/16 in from 0.072 to 0.128 in, and extends it 1/32 to 1/16 in behind the tangent lines; the tool prints that diameter, a relief-cut width of an entered multiple of t and a cut depth reaching the tangent line plus 1/16 in.

Blanking and punching

The force to shear a blank or a hole is the sheared area times the shear strength, F = L t τ, with L the total cut perimeter; τ is entered or taken as 0.75 S_u, the usual estimate for sheet steels (measured values run from about 0.6 to 0.8 S_u). The punch must then be stripped from the sheet, a force of 5 to 20 percent of the cutting force depending on the clearance and lubrication, entered as a fraction, and the press must carry both with the capacity factor. Shear on the punch face, which spreads the cut over the stroke and lowers the peak force, is not modelled.

Units

Lengths, radii and flanges convert with the unit switch (inches or millimetres), strengths in ksi or MPa, the modulus in Msi or GPa, forces in kip or kN with the tons printed beside, and the force per unit length in lb/in or N/m. The bend angles, the K-factor, the multiples, factors and fractions are plain numbers in both systems.

Limits

Straight bends in flat sheet only: no curved flanges, joggles, hems, curls or flanged holes; the springback is for an elastic-perfectly-plastic material without strain hardening or Bauschinger effect and is not a substitute for a trial bend; the press force is the air-bend estimate with multiples for the other modes, not a die-design calculation; the minimum-radius table covers aluminum sheet alloys only; the feature distances are shop rules.