What Tolerances should I Design into my Printed Circuit Board?

Where possible, design to Printed Circuit Board manufacturing industry standard mid-range tolerances. If you use these tolerances you should be able to source your boards from any manufacturer in the world without cost-penalty.

Eurocircuits uses these specifications and tolerances as the basis of our lowest-cost pooling services. Of course there may be times when component geometry or mechanical constraints mean that you

need tighter tolerances. We can usually build boards to meet these requirements but they will cost a bit more as they need special handling or additional process steps (for example for Blind or Buried Via’s).


It’s always a good idea to check your data-set and especially any drawings to make sure that they don’t specify tighter tolerances than you need. If they are outside our standard range, we may need to raise an exception, possibly delaying delivery and/or increasing costs.


Minimum tracks, gaps and annular rings are defined in the specifications of each service and are not included in this table. There is a complete list in our PCB Design Guidelines – Classification Section.


Understanding Manufacturing Tolerances on a PCB

Specification Table

Material thickness+/- 10%Based on Manufacturers’ Specifications
Maximum Bow and Twist on Boards with SMDs0.75%See our Blog – Bow and Twist in Printed Circuits
Maximum Bow and Twist on Boards without SMDs1.5%
Production Hole Oversize – Plated0.10mm

See our PCB Design Guidelines – Drilled Holes

Production Hole Oversize – Non-Plated0.00mm

Hole Size Tolerance – Plated

≤4.00mm +/- 0.10mm

>4.00mm +/- 0.20mm

Standard Tolerance Range – 0.20mm

Standard Tolerance Range – 0.40mm


Hole Size Tolerance – Plated

≤4.00mm +/- 0.05mm

>4.00mm +/- 0.10mm

≤4.00mm Min. Tolerance Range – 0.10mm

>4.00mm Min. Tolerance Range – 0.20mm

Minimum Tolerances must fall within the Minimum Tolerance Range.

example: +0.00mm/-0.10mm

Using the minimum Tolerances may increase the cost of the PCB.

Hole Size Tolerance – Via Holes

+ 0.10/-0.30mm

By default we take all holes 0.45 mm or less to be via holes. If you have component holes with finished diameter 0.45 mm or less, use the box in the Price Calculator marked “Holes <= may be reduced” to indicate the largest hole which can be treated as a via hole. The negative tolerance allows us to reduce via hole sizes to solve annular ring issues and/or to reduce board costs by reducing the number of drilling cycles needed. More.

Hole Size Tolerance – Non-Plated

≤4.00mm +/- 0.05mm

>4.00mm +/- 0.10mm

≤4.00mm Standard & Min. Tolerance Range – 0.10mm

>4.00mm Standard & Min. Tolerance Range – 0.20mm

Aspect Ratio1:8Ratio of board thickness to production drill tool
Hole Positional Tolerance0.10mmHole to Hole
Minimum Hole to Hole Distance0.25mmMeasured from production hole to production hole.

See our PCB Design Guidelines on Drill Holes and our Technical blog – The Smallest Possible Distance Between Two Holes

Minimum Non-Plated Production Hole to Copper0.25mm
Hole Wall Copper
Minimum Copper Thickness20μm
Surface Finish Thickness
Lead-free Hot-Air Leveling1 – 30μm
Electroless Gold over NickelNi:3 -6μm;

Au: 0.05 – 0.10μm

Immersion Silver Thickness0.2 – 0.4μm
Plated Hard Gold over NickelNi: 3 – 6μm; Au: 1- 1.5μm
Minimum Soldermask to Pad Clearance = Mask Annular Ring (MAR) – Plated HolesLDI – 0.03mm

Conventional – 0.10mm

This depends on the copper pattern classification – see our PCB Design Guidelines on Soldermask
Minimum Soldermask Track Cover = Mask Overlap Clearance (MOC)LDI -0.06mm

Conventional – 0.09mm

On tight layouts there may need to be a “trade-off” between MAR and MOC – see our PCB Design Guidelines on Soldermask
Minimum Soldermask Web = Mask Segment (MSM)LDI – 0.07mm

Conventional -0.13mm

Minimum Soldermask to Pad Clearance = Mask Annular Ring (MAR) – Non-Plated Holes0.125mm
Soldermask Thickness on Top of Conductors>7μmFor more information see our Technical page on Soldermask
Soldermask Thickness on Conductor Edges>7μmFor more information see our Technical page on Soldermask
Minimum Line Width0.10mm
Minimum Height for Legibility1.00mm
Legend to Soldermask Cut-Back (clipping)0.10mmAfter clipping we also remove any bits of line smaller than 0.10mm
Minimum Clearance Board Edge to Copper Tracks/Pads – Outer Layers0.25mmCopper planes can extend to the board edge. Select “copper to board edge” in the Price Calculator
Minimum Clearance Board Edge to Copper Tracks/Pads – Inner Layers0.40mm
Minimum Slot Finished Width0.50mm
Profile Dimensional Tolerance+/- 0.20mm
Positional Tolerance Profile/Cut-Out to Hole+/- 0.20mm
Slot Dimensional ToleranceWidth: +/- 0.20mm
Length: +/- 0.20mm
Minimum Copper Around Plated and Non-Plated SlotsAs annular ring for plated and non-plated holes
Maximum Board Thickness for Scoring2.00 mm
Minimum Board Thickness for Scoring0.80mm
Minimum Clearance Board Edge to Copper Pattern – Outer and Inner Layers0.45mmThis to allow for the V-cut. If copper pattern is nearer to the board edge, use break routing
Profile Dimensional Tolerance after Separation+/-0.30mm
Rest Material0.45mm +/- 0.10mm
Positional Tolerance Upper to Lower Score+/- 0.15mm
Minimum Score Depth0.15mm
Edge Beveling
Nominal Bevel Angle30° +/- 5°See our Technical page on Edge Connector Gold Surface
Rest Material0.25mm
Via Fill
Maximum Via Fill Finished Hole Size0.5mmSee PCB Design Guidelines on Via Filling and our Technical page on Via Filling
Peelable Mask
See our PCB Design Guidelines on Peel-off Mask
See our PCB Design Guidelines on Carbon Contacts
Heatsink Paste
See our PCB Design Guidelines on Heatsink Paste
Electrical Test
Minimum Test Pitch0.10mm
Smallest Testable Pad0.05mm
Test Voltageup to 1000V
Test Current100 mAAdjustable
Continuity TestCapacitance/

resistance 1 Ohm – 10 KOhm

Isolation TestCapacitance/

resistance up to 10 GOhm