Sheet Metal Bending DFM Guide: K-Factor, Bend Radius and Hole-to-Bend Distance

Start with the correct process: press-brake bending, not stamping

In fabrication, a laser or punch cuts the blank and a press brake forms one bend at a time. The setup must support the part, avoid collisions and place each bend in a workable sequence. Flexible tooling makes this route suitable for prototypes, enclosures and low-to-medium volumes.

A stamped bend is developed inside a dedicated die, often with piercing or other forming stations. Strip layout, carriers, station sequence and die clearances introduce different constraints. Do not transfer a progressive-die bend allowance or tolerance directly to a press-brake flat. Name the expected route and volume in the RFQ, or ask the supplier to compare both routes.

Neutral axis and K-factor: what the flat pattern is modeling

During bending, the outside surface stretches and the inside surface compresses. Between them is a neutral axis whose length is treated as unchanged. It normally shifts toward the inside rather than staying at mid-thickness.

K-factor equals the neutral-axis distance from the inside surface divided by sheet thickness. CAD uses it, a bend table or bend deduction to develop the blank. It is not a permanent material constant: radius-to-thickness ratio, material condition, grain direction, bend method and tooling all influence it.

A generic CAD default can support an early concept, but critical flange locations need the fabricator's bend data and, when necessary, a coupon or first-article correlation. Record any approved value with its material, thickness, radius, angle and tooling context.

Bend allowance, bend deduction and flat length

Bend allowance is the developed neutral-axis length through a bend. A common expression is BA = A × (π/180) × (R + K × T), where A is the bend angle, R the inside radius and T the thickness. Confirm whether CAD defines A as the angle formed through or the included angle; mixing conventions gives a wrong flat.

Bend deduction reaches flat length from outside flange dimensions: flat length equals their sum minus the applicable deduction. Shops often calibrate deductions from coupons. Setback is related geometry, not a replacement for process data.

Use one controlled method and do not combine a K-factor calculation with a separate shop deduction. Apply it to every bend and define whether dimensions reference theoretical corners, tangencies or real surfaces. Small errors can accumulate across a multi-bend chassis.

Choose inside bend radius with material and tooling

Call out inside radius where it affects fit, strength or appearance. A radius near one thickness is a common early concept for some ductile mild steels, not a universal minimum. Harder grades, stainless steel and some aluminum conditions may need more radius, especially when bent parallel to grain. Burrs or scratches on the tensile side can also initiate cracks.

In air bending, achieved radius depends strongly on V-die opening, material and thickness; it may not equal the punch-tip radius. Bottoming and special forming behave differently. Unnecessary radius variety can add tool changes, so standardize non-critical bends where possible.

Ask the supplier to confirm achieved radius with the intended tool set. For a crack-sensitive or mating profile, define verification and approve samples made from the intended material condition.

Minimum flange length and press-brake access

A flange must remain supported by the die as the blank rotates. Its practical minimum depends on V-opening, tool profile, angle, radius and measurement convention. A rule such as four times thickness may flag risk, but it cannot confirm every shop's tooling.

A narrower die or special tool may form a shorter flange at the cost of force, marks, setup or radius risk. Return flanges, hems and deep boxes also need clearance from punch, die, ram and backgauge. An earlier wall can block a later bend.

Send the fully formed model and bend directions for sequence review. When a short flange is functional, identify why and allow a proposed tool radius or relief.

Hole-to-bend distance and feature distortion

Material near a bend stretches, compresses and slides. A nearby hole or slot may become oval, pull toward the bend or shift from its datum. Measure clearance from the feature edge to the bend tangent, not only from its center to a drawn bend line.

For early screening, an ordinary hole edge is often kept roughly R + 2T or more from the tangent; some shops or features use R + 2.5T or more. This is a review trigger, not an acceptance limit. Large slots, countersinks, lances, inserts and position-critical holes may need more space because material, V-opening and orientation change distortion.

If the feature cannot move, consider relief, post-bend cutting or a validated pre-bend shape. State whether diameter, position, edge distance or assembly clearance is critical so the supplier can assess the right risk.

Bend relief, corner relief and tear prevention

Where a bend ends inside a blank, material at the end may tear, bulge or pull the adjacent edge. Bend relief lets the flange rotate; corner relief manages the meeting point of multiple walls.

A concept check often starts near one thickness wide and extends about inside radius plus thickness beyond the tangent. This is not a fixed minimum: kerf, material, radius, finish and corner-gap needs control the final shape. Radiused relief ends can reduce stress concentration, while an oversized relief may expose or weaken the corner.

Show whether the corner stays open, is welded, receives a cover or carries a gasket. Include weld access and finishing rather than assuming welding removes all relief distortion.

Plan for springback, grain direction and bend sequence

Springback is elastic recovery after force is removed. Material strength, radius-to-thickness ratio and tooling influence it. The fabricator may compensate with over-bend, tool selection or trial correction. Specify the finished angle and tolerance; do not pre-distort nominal CAD unless that correction is agreed and controlled.

Bending across the rolling grain is generally less crack-prone than bending parallel to it, especially for harder stock. Mark grain direction only when functional because it can reduce nesting efficiency and raise material cost.

Sequence controls access and accumulated error. A tall wall formed early may block another tool, while several bends can stack variation. Identify assembly datums and critical formed dimensions, then let the supplier select a stable forming and inspection sequence.

Drawings, STEP models and flat-pattern control

Send a formed STEP/STP model and controlled 2D drawing. The model communicates finished shape; the drawing states material, thickness, bend directions, critical radii, datums, formed dimensions, tolerances, grain, finish and cosmetic faces. Dimension function after forming instead of over-defining conflicting flat and formed states.

A flat DXF/DWG helps nesting and estimating only when its revision and bend basis are clear. Label it reference-only or buyer-controlled and state its K-factor, bend table or deduction. The fabricator may regenerate it using validated shop data.

Avoid one tight tolerance across cut edges, angles and formed locations. Tighten connector positions, mating flanges, cover gaps or mounting datums where needed, and agree on normal process tolerances elsewhere. Inspection should use stable datums and the product's assembly condition.

RFQ and DFM checklist before first articles

Give engineering enough context to select tooling and flag risky features before price and lead time are fixed. Quantity can change the preferred route, and visible faces may need special handling for press-brake contact marks.

Request written DFM feedback instead of silent changes to radius, flat or hole location. Update both model and drawing, then verify assembly-critical formed dimensions on the first article.

• Provide formed STEP/STP, controlled PDF and a labelled flat DXF/DWG when available.
• State material grade, thickness, condition, finish, grain constraint and acceptable alternatives.
• Mark bend direction, finished angle, critical radius, datums and critical formed dimensions.
• Identify short flanges, close features, reliefs, hems, inserts and collision-prone walls.
• Define visible faces, tooling-mark limits, deburring, masking and prefinished material constraints.
• List prototype and annual quantities plus first-article measurements and assembly checks.
• Ask the supplier to confirm method, tooling, bend data, sequence and proposed changes.