Tight tolerances on a laser-cut part are usually free in CAD and expensive on the shop floor. Here is where they actually matter — and where they quietly add cost.
A tolerance is a purchasing decision written in a drawing. Every time a designer types ±0.1 mm out of habit, somebody downstream decides whether to add an operation, slow a machine, or gauge a batch that would otherwise have shipped. On laser-cut sheet metal that decision gets made dozens of times per drawing.
What the process gives you for free
A well-maintained fibre laser holds roughly ±0.1 mm on profile within a single sheet, and that is genuinely free — it falls out of the process. What is not free is holding that same tolerance across a bend, across a weld, or across a batch cut from different coil.
- .01Cut profile within one sheet: ±0.1 mm, no cost
- .02Hole position within one sheet: ±0.1 mm, no cost
- .03Across a single bend: ±0.3 mm realistically, before springback correction
- .04Across two or more bends: stack the tolerances, do not repeat the tight one
- .05After welding: assume ±1 mm unless the part is fixtured and stress-relieved
Where the money leaks
The expensive pattern is a tight linear tolerance measured from a folded edge. The fold is the least repeatable feature on the part, so a ±0.1 mm callout from that datum forces either a secondary machining operation or a fixture that nobody quoted for. Reference the flat, not the fold, and the cost disappears without any loss of function.
The second leak is uniform tolerancing — the same block tolerance applied to all 40 dimensions on a sheet. Mating features usually account for four or five of those. The rest can sit on a general tolerance to ISO 2768-m and nobody will ever notice.
RULE OF THUMB — IF A DIMENSION DOES NOT TOUCH ANOTHER PART, IT DOES NOT NEED A SPECIFIC TOLERANCE.
K-factor is not a constant
Flat patterns generated with a default K-factor of 0.44 will be wrong on your press brake, because bend allowance depends on material, thickness, tool radius and the machine itself. The fix is a bend table built from your fabricator's test pieces, applied in CAD. Once it exists, first-off parts stop needing a trim.
What we do on issue
Every sheet metal pack we issue carries a general tolerance note, specific tolerances only on mating features, flat patterns generated against the fabricator's own bend table, and a DXF nested to the sheet size the shop actually buys. It is not more work — it is the same work, decided deliberately.