Datum strategy for sheet metal: what to dimension from

A bracket dimensioned from its sheared edge passes first article at the toolmaker and fails at the customer, because the edge moved 0.4 mm when the blank was nested differently and every hole moved with it. Nothing was out of tolerance on the drawing. The drawing had simply chosen a datum that the process does not control.

Datum strategy for sheet metal is the decision about which features the inspector and the welder are allowed to trust. Get it right and a part with ±0.2 mm feature accuracy assembles every time. Get it wrong and a part made to ±0.1 mm is rejected because the datum it was measured from was never repeatable.

The rules below cover what to use as A, B and C, where the bend error enters, what to leave as reference, and how coating changes a datum that was correct on the flat.

What should a sheet metal drawing use as its datum?

Datum A should be the mounting face, B a round hole and C a slot in the line between the holes. That combination follows the assembly, matches how a fixture would hold the part, and does not over-constrain a laser-cut profile.

The mounting face is almost always obvious: it is the face that sits against the mating part and carries the fastener load. On an enclosure side panel it is the inside face that lands on the frame. On a bracket it is the flat that touches the machine. Making that face datum A means flatness and any bow are measured where they matter, not on the outside face that nobody clamps.

The hole choice is less obvious. A single hole fixes two translations, and a second feature fixes rotation. If both features are round holes, the distance between them has to match the pin spacing exactly, or the part will not seat. Laser cut position is about ±0.2 mm, and hole spacing on a 300 mm part can vary by that much, so two fixed pins will bind on some parts and rattle on others. A slot at C, elongated along the line between the holes, removes that conflict. It is the sheet metal version of the diamond locating pin.

What not to use: a cut edge as a primary datum, a formed flange as A unless it is the seating face, and a bend line as a datum. All three are features the process controls poorly compared with a hole cut in the same setup as the features being measured.

How repeatable is each datum feature?

Feature-to-feature accuracy is better than edge-to-feature accuracy because features cut in one laser setup share an origin. The table gives the values we work to, and the Ganesh column says what we will hold on a drawing that asks.

The edge figure is the one that catches designers out. A laser edge is accurate in position relative to the machine origin, but the blank may be nested with a 0.2 mm gap to the sheet edge, and a sheared edge on a guillotine can be 0.5 mm off over 3 m. Dimensioning a hole pattern from the edge ties a ±0.1 mm feature to a ±0.5 mm reference and loses the accuracy the machine already had.

Where the bend error enters the stack

A bend adds an angular tolerance that grows with distance. At the ±0.5° we hold on the 200 T brake, the positional error on a flange is:

error = L × tan(0.5°) = L × 0.00873

At 100 mm from the bend line that is 0.87 mm. At 300 mm it is 2.62 mm. No amount of hole position accuracy survives that, which is why a hole on a long flange should be dimensioned from the bend line with its own tolerance, and why the flange should not be used as a datum for anything on the other side of the bend.

There is a second bend error that people miss: the bend allowance. The flat pattern is calculated from a K-factor, and if the K-factor is out by 0.02 on a 2 mm part at 90°, the developed length changes by:

ΔBA = θ × t × ΔK = 1.571 × 2 × 0.02 = 0.063 mm

That is small per bend, but it accumulates on a part with four bends, and it changes the position of every feature on the far side of the chain. The bend allowance guide has the arithmetic; the datum consequence is that features either side of a bend should be located from the bend line, not from each other.

A worked example

Take a 3 mm CRCA bracket, 150 mm by 80 mm, with a mounting hole at each end on 120 mm centres and a third hole on a 60 mm flange.

If the two mounting holes are dimensioned from the sheared 150 mm edge, the stack is 0.5 mm of edge position plus 0.2 mm of hole position, giving 0.7 mm worst case between the hole pattern and the mating frame. If they are dimensioned from datum B in the same laser setup, the same distance holds to 0.1 mm.

If the third hole is dimensioned from the mounting holes across the bend, add 0.52 mm of angle error at 60 mm, 0.2 mm of bend line position and 0.06 mm of K-factor error, giving 0.78 mm on top of the pattern. If it is dimensioned from the bend line and the flange is allowed to float, the pattern stays at 0.1 mm and the flange hole carries its own 0.5 mm.

That is the whole strategy in one part: hold the pattern tight because the assembly needs it, and let the flange hole be loose because nothing mates to it except a clip.

What to leave free, and how to say so

A drawing that tolerances everything equally tells the inspector nothing. The dimensions that should carry a tight tolerance are the ones the assembly closes on. Everything else should be marked as reference, in parentheses, or left to the general tolerance note.

Leave these free:

• Overall length and width. The mating part usually has clearance, so a 150 mm overall dimension does not need ±0.2 mm. ISO 2768-1 medium gives ±0.5 mm over 120 to 400 mm, and that is enough.
• Non-functional bend angles. A stiffening flange that touches nothing can be ±1°; a flange that seats on a frame cannot.
• Cable and drainage holes. Position to ±1 mm unless a grommet or a connector needs better.
• Edge parallelism and squareness of a laser cut profile. The machine holds it; specifying it adds inspection cost for no assembly benefit.
• Cosmetic features on a hidden face. Note them as cosmetic and keep them off the tolerance chart.

Leave these tight: the datum hole diameters and their position, the hole pattern that carries fasteners, the mounting face flatness, and any feature that sets a sealing gap.

ISO 2768-1 applies only where the drawing does not state a tolerance for that dimension. The moment a dimension carries its own tolerance, the general note no longer covers it. That scoping matters in review: a drawing that says "tolerances to ISO 2768-m" and then dimensions a hole as 10.0 without a tolerance has left the hole diameter on the general note, which is ±0.2 mm at that size, not the ±0.1 mm the designer intended.

How a datum strategy for sheet metal changes after coating

Powder coating at 60 to 90 µm per face adds 0.12 to 0.18 mm to a feature that is coated on both walls. A 10.00 mm datum hole becomes 9.86 mm, and a 10.00 mm locating pin no longer enters without force. The part is dimensionally correct as cut and unusable as coated.

Three options, in order of preference:

1. Mask the datum holes and a 10 mm ring around them before coating. This is what we do on parts where the hole is also a fixture locator.
2. Cut the hole 0.2 mm oversize and accept that the datum is now the coated edge, which is softer and less repeatable.
3. Move the datum to a masked face or a masked slot, and keep the coated holes as clearance only.

The bending tolerance and inspection guide covers how the formed features are checked; the coating point is that the datum has to survive the whole route, not just the laser.

What Ganesh runs

Datum features are cut on the 12 kW fibre laser with the 40 ft × 16 ft bed, so a 3,000 mm part and its hole pattern come off in one setup and hold ±0.2 mm position, with ±0.1 mm feature to feature. Forming runs on the 200 T, 4,450 mm, 5-axis brake with Delem control, holding ±0.5° on bend angle and ±0.5 mm on formed features. Where a part is welded into a frame, fixtures are designed and built in the in-house tool room, and they locate on the same datums the drawing specifies, which is the point of naming them at all.

First article inspection reports the datum features before anything else, and PPAP documentation is available where the programme requires it. Coating runs through seven-tank pretreatment and the 18 ft × 14 ft powder booth, with DFT and cross-hatch adhesion checks, and masking is applied per the drawing note rather than per habit. The bending capability page lists the machine and tool set, and the design and CAD hub collects the related rules on tolerance and flat patterns.

What to put on the drawing

• Datum A identified on the mounting face, with a flatness value if the assembly needs one.
• Datum B as a hole with its diameter and position tolerance, and datum C as a slot with its width and orientation.
• A position tolerance for the fastener pattern referenced to A, B and C, in that order.
• Reference dimensions in parentheses for overall size and non-functional features.
• A general tolerance note that names the standard and the class, for example ISO 2768-1 medium.
• A masking note for every datum feature that is also a locator.
• A bend table with angle and bend line position tolerance per bend, rather than one note for the whole part.
• The assembly datum carried through to the weld drawing, so the fixture and the drawing agree.

When this datum scheme is wrong

If the part is located in a weld fixture by three pins, the drawing datums should be those three holes, even if a different trio would be better for inspection. The datum that matters is the one the process uses.

If the part is a deep drawing with no flat face, the mounting face may be a trimmed edge or a drawn wall, and the scheme has to change. If the part is coated all over and has no masked feature, the coated surface is the datum by default and the tolerance has to widen to cover it.

We do not hold datum position across a weld without a fixture, and we do not certify a datum that is defined on a feature we cannot access after assembly. Send the drawing with A, B and C marked and the assembly interface identified, and the scheme can be checked against the process before the first part is cut. Request a quote with the revision and the mating part, or read the tolerance stack-up guide for how the numbers combine once the datums are set.