A PCB tolerance table lists each item on its own: one value for hole location, one for the outline, one for thickness. Assembly uses them in combination. A connector has to hit two holes at once, an enclosure snap has to clear a hole and the board edge, a card guide has to grip the board thickness. If the drawing only says "standard tolerances", every item can pass inspection while the combined dimension still exceeds the mechanical clearance.
This article covers two things: what to use as datums on the fabrication drawing, and how hole, outline and thickness tolerances stack. The values themselves are on the SKPCB manufacturing tolerance table. Nominal versus acceptance values, and which items default to the table when the drawing is silent, are covered in PCB manufacturing tolerances on the drawing: nominal vs accepted.
1. Each tolerance has a different reference
| Item | Set by which process | Measured relative to |
|---|---|---|
| Hole location | Drill program and drill registration | Drill program origin or tooling holes |
| Outline | Routing or punching, a separate setup | The profile itself |
| Thickness | Lamination, plating, surface finish | Between the two surfaces, at an agreed location |
Holes and outline come from different operations. Holes drilled in the same program only carry drilling error relative to each other. The distance from a hole to the board edge carries drilling error plus the registration error of the routing setup. Dimensioning holes from the board edge puts both processes into one dimension.
2. Choosing datums
Pick datums from how the board is mounted, not from whichever corner is convenient to draw from:
- Datum A: the mounting face, usually the bottom side. Thickness and component height are referenced here.
- Datum B: one mounting or tooling hole, fixing position.
- Datum C: a second mounting hole, fixing rotation.
Dimension critical holes (connector, press-fit, alignment) from B and C. If the board edge plays no part in locating the board, leave it at general tolerance. If it does (card guide, snap fit), call that edge segment out as a critical dimension and state which datum it refers to.
3. How the tolerances stack: a worked example
The arithmetic below uses the standard values published on the SKPCB tolerance table, imperial authoritative: hole location ±0.003" (≈0.076mm), board outline ±0.005" (≈0.13mm).
| Chain | Worst case (linear sum) | Statistical (root sum square) |
|---|---|---|
| Hole to hole (same program, each hole to datum) | ±0.006" (≈0.15mm) | ≈ ±0.0042" (≈0.11mm) |
| Hole to board edge | ±0.008" (≈0.20mm) | ≈ ±0.0058" (≈0.15mm) |
When to use which:
- Worst case fits small lots, fits that cannot be reworked, or assemblies that are scrapped if they do not go together.
- Root sum square assumes independent, centred errors and fits high volume where some sorting is acceptable.
Compare the result with the mechanical clearance: pin-to-hole clearance on the connector, snap-fit relief in the enclosure, screw-to-clearance-hole gap. If the clearance is smaller than the stack, either open up the mechanical design or tighten one item and write it on the drawing.
4. Where thickness enters the chain, and where to measure it
Thickness tolerance on the table is ±10% or ±0.005", whichever is greater. It enters the assembly chain at edge connectors, card guides and press-fit connectors. The drawing should state:
- What is measured: laminate to laminate, or overall including copper, solder mask and finish.
- Where it is measured: the gold-finger area, the guide edge, or the board centre.
Without this, the fabricator and incoming inspection may measure in different places and reach different conclusions. Process factors behind thickness are in finished PCB thickness tolerance control.
5. What the drawing should say
- Definition and location of datums A, B and C.
- Critical dimensions with their own tolerance and the datum they refer to.
- A note that all other dimensions follow the manufacturing tolerance table.
- Thickness measurement type and location.
- Tightened items listed one by one, for example "hole B to hole C ±0.002"", not a general "high precision". Tightening can change the process route and inspection method and is confirmed in project review.
How the routing method affects outline accuracy is in PCB profiling tolerance. Checks before releasing the drawing with the stack-up are in the stack-up drawing release checklist.
6. Matching inspection to the drawing
Hole location and outline dimensions can be measured from datums on a 2D vision measuring machine. Once the drawing defines datums, the inspection report gives data in the same coordinate system and incoming inspection can re-measure the same dimensions. If you need measurement data for critical dimensions shipped with the boards, ask for it at RFQ via the quote page.
FAQ
Q: What tolerance applies to a dimension with no tolerance on the drawing?
A: The standard value from the manufacturing tolerance table. No callout does not mean no limit.
Q: Why not dimension holes from a board corner?
A: The corner comes from routing, the holes from drilling. Dimensioning from the corner combines both errors in one dimension, which is larger than hole-to-hole.
Q: Worst case or root sum square?
A: Worst case for small lots, non-reworkable fits, or assemblies scrapped on failure. RSS for high volume where errors can be treated as independent.
Q: Can hole-to-hole tolerance be tighter than the table?
A: Yes, requested item by item on the drawing. Feasibility and impact on process and inspection are confirmed in project review.
Q: Does thickness need a measurement location?
A: Yes. Overall thickness differs from laminate thickness by copper, solder mask and finish. Mating areas such as gold fingers should be called out separately.