GD&T for sheet metal: scope, limits and what to ask for

A bracket drawing that says ±0.2 on two hole locations and a bracket that says ⌀0.4 at MMC are not the same requirement, even though both look like twenty-hundredths on the page. The first fixes a 0.4 mm × 0.4 mm box around each hole. The second fixes a 0.4 mm circle that widens as the hole is cut oversize. On a ⌀6.0 +0.2/0 hole, the second callout accepts a 0.3 mm axis shift at the top of the size band, where the first allowed 0.2 mm.

That difference is what geometric tolerancing buys, and it is also why the language is worth learning. It does not make parts more accurate. It aligns the tolerance on the drawing with the way the part actually assembles.

Geometric tolerancing is the ISO 1101 system of symbols and feature control frames that defines form, orientation, location, profile and run-out zones. This page sets out what the standard covers, where it stops and hands over to four other standards, which zones a 1–4 mm sheet metal part can hold, and the four fields to add to a drawing. The standards and compliance hub covers the rest of the cluster.

What does ISO 1101 cover, and where does it stop?

ISO 1101 defines the symbols, the feature control frame and the shape of the tolerance zone. It covers fourteen characteristics: four for form (straightness, flatness, circularity, cylindricity), three for orientation (parallelism, perpendicularity, angularity), three for location (position, concentricity, symmetry), two for profile (line, surface) and two for run-out (circular, total).

That is the whole of its remit. It tells you how to write a requirement and what shape the zone takes. It does not tell you which datum to use, how much extra tolerance a loose hole earns, whether size and form are independent, how many parts to inspect, or what to do when the measurement is close to the limit. Those sit in other documents, and a drawing that cites ISO 1101 alone is under-specified in exactly the places that cause arguments at first article.

The practical consequence is simple. A buyer who receives a drawing with a feature control frame and no datum note, no material modifier and no statement of tolerance principle has received a symbol, not a specification. Ask which system applies before the drawing goes to quotation, because the answer changes the inspection method and the scrap rate.

Which zones can a sheet metal part actually hold?

The table below is the working set for 1–4 mm CRCA, stainless and aluminium parts made on a fibre laser, a press brake and a welded fixture. The values assume a flat part inspected on a surface plate or a checking fixture, not a CMM programme written from the model without a datum review.

Two entries in that table explain most of the disputes we see. The first is position across a bend. A hole placed 20 mm from the bend line on a 2 mm CRCA flange moves when the bend angle varies, and a 0.5° error at 20 mm is 0.17 mm. Combine that with ±0.2 mm of cut position and the ⌀0.5 zone is already spent. The second is flatness after welding, where a 0.3 mm callout on a 300 mm frame face is achievable with a fixture and a balanced weld sequence, and not achievable without them.

Tolerance stack explains a third family of failures, where every individual callout passes and the part does not fit. Take a three-flange channel with three flange heights at ±0.3 mm and two bend angles at ±0.5° on 40 mm flanges. Worst case, the flange heights contribute 0.9 mm and the angles 0.7 mm, for 1.6 mm at the far hole. Root-sum-square, the same inputs give √(0.52² + 0.49²) = 0.71 mm. Neither number fits a ⌀0.4 zone, which is why a position callout on the third flange has to be set from the stack and not from what the laser can do in the flat.

ISO and ASME are two systems, and the default differs

The same feature control frame means two different parts depending on which system the drawing follows. ISO 8015 sets out the independency principle: every dimension and geometric requirement is met separately, so a ⌀6.0 shaft that measures ⌀5.98 at every section may still be bowed, and the size callout is satisfied. ASME Y14.5 applies an envelope by default, so the same shaft must also fit inside a perfect ⌀6.0 cylinder.

ISO handles the gap with the Ⓔ envelope symbol, which is written after the size tolerance when form has to be controlled by the size dimension. If the drawing is silent, ISO gives you independency and the part may be straighter or more bent than the buyer assumed.

This is not a theoretical distinction on thin sheet. A 1.5 mm panel cut on a 40 ft × 16 ft bed can be flat to 0.2 mm, but a 300 mm strip 1.5 mm thick that has been sheared and stacked can bow 1 mm and still measure 1.5 mm on a micrometer. Under ISO 8015 with no Ⓔ, that strip conforms. Under ASME Y14.5 it does not.

There is a parallel split inside the welding standard family, where ISO 2553:2019 carries two symbol systems, one aligned with ISO practice and one aligned with the ASME approach. The lesson is the same in both cases: state the system on the drawing, in the general notes, on the same sheet as the title block. A note that says "interpret per ISO 8015 and ISO 1101" removes a week of first-article correspondence.

How do you check a position callout without a CMM?

You calculate true position from two measured offsets. True position is twice the radial distance from the true location, so with the hole 0.12 mm out in X and 0.09 mm out in Y, the true position is 2 × √(0.12² + 0.09²) = 2 × 0.15 = 0.30 mm. That is inside a ⌀0.4 zone. The same two offsets under a ±0.2 coordinate callout are also inside, and the two methods agree on the axes.

The difference appears at the corners and with the modifier. Take a ⌀6.0 +0.2/0 hole with a ⌀0.4 zone at MMC. The hole measures ⌀6.18. Bonus tolerance is 0.18 mm, so the allowable zone is ⌀0.58. At true position 0.30 mm the part passes with margin, where the flat ⌀0.4 callout would have used three-quarters of the zone on a hole that is functionally better than nominal, because a larger hole clears the bolt more easily.

Inspection follows the same logic. A checking fixture with two pins at the virtual condition size — for the example above, ⌀6.0 − 0.4 = ⌀5.6 body and a ⌀6.2 hole in the plate — tests the assembly condition directly and takes seconds per part. A CMM programme gives richer data and costs minutes per part. On a 5,000-piece order, the fixture is the right instrument for production and the CMM is the right instrument for the first article and the annual layout.

Practical calibration of the fixture matters more than the CMM's accuracy statement. Pins wear, and a pin worn by 0.05 mm accepts parts the drawing rejects. Check the fixture against its own drawing on a fixed interval, not only when a customer rejects a part.

What Ganesh runs, and what it changes

Ganesh cuts on a 12 kW fibre laser with a 40 ft × 16 ft bed, supported by two 6 kW and two 3 kW machines, and forms on a 200 T, 5-axis brake with a 4,450 mm bed and Delem control to 10 mm. The working tolerance for a custom part is ±0.5 mm, with tighter features by agreement on a feature-by-feature basis.

The checking fixtures used on repeat parts are designed and built in the in-house tool room, which is the same shop that builds press tools, progressive dies and welding fixtures. That matters for geometric tolerancing because a fixture built from the model, without a datum review, will confirm the model and not the drawing. The bending and inspection guide covers how a formed feature is measured against its datum.

Welded frames from three CLOOS robotic MIG cells and more than 30 manual MIG/MAG, spot and SPM stations behave differently from a cut blank. Distortion moves the datum, and a profile callout of 0.5 mm on a welded frame is a fixture-and-sequence requirement, not a cutting one. The welded assembly tolerance guide sets out the numbers that survive the weld; the bending capability describes the brake and its tooling.

Pressed parts have a different set of limits again, because a progressive die holds position from the tool rather than from the machine. The stamping tolerance guide covers those figures, and first article inspection and PPAP are available where the OEM programme requires them.

What to put on the drawing

1. Datum scheme. Three datums, A as the primary face, B and C as two holes or two edges, in the order that matches how the part is located at assembly.
2. Feature control frames on the features that locate the part. Two holes and one face on a bracket; add profile only where a visible surface or a gasket face matters.
3. Material modifier. Ⓜ on clearance holes that take a fastener, Ⓛ on features where minimum wall matters.
4. Tolerance principle. A general note naming ISO 8015 and ISO 1101, plus Ⓔ on any size callout that must also control form.
5. General tolerance class. ISO 2768-m for linear and angular dimensions and ISO 2768-2 class K for form and position, so the uncalled features have a default.
6. Inspection extent. Which features are checked on every part, which on first article, and whether a checking fixture is expected to ship with the tooling.

The DXF and RFQ checklist covers the file side. The datum scheme is the field most often missing from the pack that arrives with a drawing.

When geometric tolerancing is the wrong tool

Three cases. A one-off fabricated frame with no mating part is better served by a diagonal dimension and a flatness note than by nine feature control frames, because nobody will inspect nine and the fitter will adjust the frame on site anyway. A part whose real requirement is "fits the mating pressing" is better served by a functional gauge specification, which tests the condition directly and needs no interpretation. And a part that is already at the process limit gains nothing from a tighter symbol: a ⌀0.2 zone on a hole across a bend is not a request, it is a rejection waiting to happen.

Ganesh does not machine datums onto a laser-cut part, and we do not hold machined-surface flatness on a formed flange. Where a drawing needs a ground face, a bored hole or a turned bore, that operation sits outside this route and belongs with a machining supplier. Saying so at quotation is cheaper than discovering it at first article.

Send the drawing with the datum scheme, the material and the features that decide assembly. The engineering team will return the zones the route can hold and the ones it cannot, and the quotation request takes the file in PDF, DXF, DWG or STEP.