GD&T for sheet metal: profile and position on formed parts

A bracket drawing carries a general tolerance of ±0.5 mm and a 90° bend with no angle call-out. The part arrives square, the bend is right, and the assembly still will not close, because the flange tip is 1.75 mm out of position from a one-degree angle error on a 100 mm flange. The tolerance on the drawing never controlled the feature that mattered.

GD&T for sheet metal changes what the drawing measures, not how tightly the part is made. Profile of a surface holds the formed shape inside a band. Position holds the hole pattern to the datums. Together they describe a bent part the way it actually behaves — errors that rotate, not errors that shift.

The arithmetic is simple enough to settle most arguments at quotation: tan(1°) × 100 mm = 1.75 mm. Angle tolerance multiplies by flange length. That number, not the ±0.5 mm, is what a formed part is really controlled to.

Why does ±0.5 mm not control a formed part?

Because a bent part's error is angular, and a linear tolerance does not know about distance. A flange held to ±1° at the tip of a 100 mm flange has moved 1.75 mm; at 200 mm it has moved 3.49 mm; at 300 mm, 5.24 mm. The same part can pass the general tolerance at the bend and fail at the edge.

There is a second reason the general tolerance misses: it is applied to dimensions, not to surfaces. A flange that twists 0.4 mm across its width has no dimension out of tolerance, and it still will not seat on the mating part. Profile of a surface catches it, because the tolerance zone is a band around the whole face.

ISO 2768-2 covers geometrical tolerances for features that carry no individual tolerance indication, which is the fallback when nothing is called out. It is a floor, not a specification: a bracket that has to bolt to a machined mating face needs the datum and the zone stated, because the default class was never chosen for that fit.

What a GD&T for sheet metal drawing should call out

Read the table as a checklist, not a wish list. Every GD&T call-out on a formed part should be one a CMM or a fixture can evaluate, and should point at a feature the assembly actually uses.

Profile and position answer two different questions

Position answers "where is this feature relative to the datums". Profile answers "is this surface where the shape says it should be". A formed bracket usually needs both, and mixing them up produces drawings that cannot be inspected.

Position applies to features of size — holes, slots, bosses — and its tolerance zone is a cylinder at true position. The call-out Ø0.5 means the axis of the hole must sit inside a 0.5 mm diameter cylinder. At MMC, the zone grows as the hole grows, which is the bonus tolerance that lets a clearance hole drift further when it is larger.

Profile applies to surfaces, and its zone is a band centred on the nominal surface unless unequal distribution is stated. A call-out of 0.5 on a flange means the entire face must lie between two surfaces 0.5 mm apart, straddling nominal. With unequal distribution, written as 0.4 outside and 0.1 inside, the band shifts to protect the mating side — useful where a flange must not grow into a gap but may move into clearance.

ISO 1101 defines the symbols, the tolerance zones and the rules for both. The practical difference on the shop floor is which instrument proves it: position is a hole centre, measured with a pin, a CMM or a functional gauge. Profile is a surface, measured by scanning or by seating the part in a fixture with the mating features built in.

Datum strategy on a bent part

Three datums, in the order they constrain the part.

Datum A is the face that mounts. On a bracket, that is the largest flat face that seats against the parent structure, not the flange and never the radius. Datum B fixes translation and one rotation; on sheet metal the usual choice is a hole that also takes a fastener. Datum C fixes the last rotation, either a second hole or a formed edge.

Two holes are better than a hole and an edge because a laser-cut edge is a straight line with a burr and a break, while a hole has a defined centre. Two holes also survive coating better: a hole centre does not move by 70 µm when powder is applied, even though its diameter shrinks.

Where the holes are in the flat pattern rather than in the formed part, say so. A hole pierced before forming moves with the bend deduction, so the hole position in the formed part carries the bend error. That is why the position call-out has to be evaluated on the formed part, in the fixture, after bending.

Composite position and the two tiers

A hole pattern that mates with a fixed set of studs has two requirements at once: the holes must be right relative to each other, and the pattern must be in the right place on the part.

Composite position writes both. The upper segment, for example Ø0.5 to A|B|C, locates the pattern as a group within 0.5 mm of the datums. The lower segment, Ø0.2 to A|B|C, controls each hole relative to the others, and is evaluated without datum shift. The pattern can sit anywhere inside the upper zone, and each hole must still be within 0.2 mm of its true position within the group.

That distinction matters when the mating part has clearance. A 0.5 mm group position with 0.2 mm hole-to-hole holds the assembly together even if the whole pattern is 0.4 mm off, because the studs move with it. Without the lower segment, a pattern that is 0.5 mm off in one direction and 0.5 mm off in the other can still pass each hole individually while the studs bind.

Angle tolerance turns into millimetres

The conversion is worth memorising, because it ends the "just hold the angle" conversation.

For a flange of length L and an angle error θ, the tip displacement is L × tan θ. At 0.5° and 100 mm, that is 0.87 mm. At 1° and 100 mm, 1.75 mm. At 1° and 300 mm, 5.24 mm.

The 200 T, 5-axis brake with a 4,450 mm bed and Delem control holds about ±0.5° per bend on a 2 mm part, with the 5-axis compensation correcting ram deflection along the bed. That is 0.87 mm at the tip of a 100 mm flange and 2.6 mm at the tip of a 300 mm flange. If the assembly needs the tip within 0.5 mm, the drawing cannot rely on the angle — it needs a profile call-out that the fixture can hold, or it needs a shorter flange.

There is a second order effect that catches designers: the flange length itself. The flat length depends on the bend deduction, which depends on the die opening and the K-factor. Change from a 16 mm to a 12 mm V die on 2 mm CRCA and the inside radius drops, the deduction changes by roughly 0.2-0.4 mm, and every hole that was positioned from the bend line moves with it. The bend allowance guide works through that arithmetic, and it is the most common reason a GD&T drawing and a first article disagree.

Inspection: CMM, fixture or gauge

An inspectable drawing names the state and the method. Three options cover sheet metal work.

A CMM with a fixture mounts the part on its datums and scans the surfaces and hole centres. It returns a number for every call-out and it is the right tool for first article inspection and PPAP submissions. It is slow, so it is not a production check.

A checking fixture built to the datums seats the part on datum A and pins B and C. It answers pass or fail on the features that matter, in seconds, at the line. Fixtures are designed and built in-house here, which is why they are the usual choice for repeat orders: the fixture and the weld or bend setup come from the same datum scheme.

A functional gauge — a pin, a go/no-go plate — answers one question only. It is cheap and it is definitive for that question, and it is useless for diagnosing why a part failed.

Whichever is used, the coating question has to be settled on the drawing. A powder film of 60–80 µm adds at least 0.06 mm to a measured surface per side, so a 0.3 mm flatness call-out on a coated face is being measured against a film as thick as a fifth of the tolerance. State "dimensions apply before coating" or "after coating, coated surfaces excluded", and do not leave it to interpretation.

How Ganesh works to a GD&T drawing

Drawings and models are accepted as PDF, DXF, DWG and STEP, and the datum scheme is reviewed before the route is quoted. A call-out that cannot be measured is queried at that point rather than discovered at first-off.

Forming runs on the 200 T, 5-axis CNC press brake with a 4,450 mm bed, working to 10 mm, with a Delem control that holds the angle and compensates the ram across long parts. Cutting runs on a 12 kW fibre laser with a 40 ft × 16 ft bed on mild steel, CRCA, stainless, aluminium, brass and copper, which is where hole position and edge quality come from. Welded assemblies go to three CLOOS robotic MIG cells or to more than 30 manual MIG, MAG, spot and SPM stations, with fixtures designed in-house.

Custom parts run from 0.8 mm to 40 mm at ±0.5 mm typical sheet metal tolerance, tighter on critical features by agreement. Coating is supported by a seven-tank pretreatment line, a 16 ft × 16 ft shot blast chamber, an 18 ft × 14 ft electrostatic powder booth and a wet paint booth, with DFT gauge and cross-hatch adhesion testing as the check on the film. About the coating, the coated assemblies capability page covers what the line does to a dimension.

First article inspection is standard and PPAP is available where the programme needs it. The bending tolerances and inspection page covers what the brake holds feature by feature, and welded assembly tolerances covers how bend error and weld distortion add on an assembly.

What to put on a GD&T drawing for a formed part

• Datum A on the mounting face, B and C on two holes. State that they are evaluated after forming.
• One profile of a surface call-out for the formed shape, with the zone width and the datum reference frame.
• Position on every hole that takes a fastener, at MMC where clearance allows.
• Angle and tolerance per bend where the angle is functional, and a note that the angle is measured on the formed part.
• The inspection state for coating, and whether coated surfaces are excluded from dimensional checks.
• A note on which features are checked on first article only and which are checked on every part.
• The model revision, because a GD&T drawing that does not match the STEP file produces two different first articles.

The design and CAD hub collects the drawing-side guides, including the STEP model handover rules that decide whether the model and the drawing describe the same part, and the laser cutting tolerance page gives the feature-level numbers behind the position call-outs.

When GD&T is the wrong tool on a formed part

GD&T does not fix a design that cannot be made. A 0.3 mm profile across a 1,200 mm welded panel is a distortion problem, and the answer is a fixture and a weld sequence, not a tighter zone. A position call-out on a hole placed too close to a bend line will be met on some parts and missed on others, because the material stretches as it forms.

It is also the wrong tool when nobody can measure it. A call-out on a 3-point datum frame that does not appear on any fixture or CMM program will be "verified" by a tick box. If the part is inspected at the customer's plant against a scheme the drawing does not show, send that scheme with the drawing.

And it is the wrong tool for a part where the fit is genuinely loose. A cover panel with 2 mm of clearance all round needs an envelope and a flatness limit, not a full frame. Adding precision that the assembly does not use raises the inspection cost without changing the fit.

Send the drawing, the model and the datum scheme, and request a quote with the call-outs you are unsure of marked. The engineering team will say which of them the brake, the laser and the fixture can hold, and which need a design change before the tool is set.