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).

ACTION TIP

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.

NOTE

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.

SEE ALSO

Understanding Manufacturing Tolerances on a PCB

Specification Table

Description
Tolerance
Notes
Materials
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%
Drilling
Production Hole Oversize – Plated0.10 mm

See our PCB Design Guidelines – Drilled Holes

Production Hole Oversize – Non-Plated0.00 mm
STANDARD

Hole Size Tolerance – Plated

≤4.00mm +/- 0.10 mm

>4.00mm +/- 0.20 mm

Tolerance Range – 0.20mm

Tolerance Range – 0.40mm

MINIMUM

Hole Size Tolerance – Plated

≤4.00mm +/- 0.05 mm

>4.00mm +/- 0.20 mm

Minimum Tolerances must fall within the Standard 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/-0.30 mm

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 +/- 0.05 mm

>4.00mm +/- 0.10 mm

Aspect Ratio1:8Ratio of board thickness to production drill tool
Hole Positional Tolerance0.10 mmHole to Hole
Minimum Hole to Hole Distance0.25 mmMeasured 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 Copper0.25 mm
Hole Wall Copper
Minimum Copper Thickness20 μm
Surface Finish Thickness
Lead-free Hot-Air Leveling1 – 30 μm
Electroless Gold over NickelNi:3 -6 μm;

Au: 0.05 – 0.10 μm

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

Conventional – 0.10 mm

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 – 0.09 mm

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 -0.13 mm

Minimum Soldermask to Pad Clearance = Mask Annular Ring (MAR) – Non-Plated Holes0.125 mm
Maximum Via Filling Finished Hole Size (ENDSIZE) Resin or Soldermask0.50 mmSee PCB Design Guidelines on Via Filling and our Technical page on Via Filling
Soldermask Thickness on Top of Conductors>7 μmFor more information see our Technical page on Soldermask
Soldermask Thickness on Conductor Edges>7 μmFor more information see our Technical page on Soldermask
Legend
Minimum Line Width0.10 mm
Minimum Height for Legibility1.00 mm
Legend to Soldermask Cut-Back (clipping)0.10 mmAfter clipping we also remove any bits of line smaller than 0.10 mm
Break-Routing
Minimum Clearance Board Edge to Copper Tracks/Pads – Outer Layers0.25 mmCopper 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 Layers0.40 mm
Minimum Slot Finished Width0.50 mm
Profile Dimensional Tolerance+/- 0.20 mm
Positional Tolerance Profile/Cut-Out to Hole+/- 0.20 mm
Slot Dimensional ToleranceWidth: +/- 0.20 mm
Length: +/- 0.20 mm
Minimum Copper Around Plated and Non-Plated SlotsAs annular ring for plated and non-plated holes
Scoring/V-Cut
Maximum Board Thickness for Scoring2.00 mm
Minimum Board Thickness for Scoring0.80 mm
Minimum Clearance Board Edge to Copper Pattern – Outer and Inner Layers0.45 mmThis to allow for the V-cut. If copper pattern is nearer to the board edge, use break routing
Profile Dimensional Tolerance after Separation0.30 mm
Rest Material0.45 mm +/- 0.10 mm
Positional Tolerance Upper to Lower Score+/- 0.25 mm
Minimum Score Depth0.15 mm
Edge Beveling
Nominal Bevel Angle30° +/- 5°See our Technical page on Edge Connector Gold Surface
Rest Material0.25 mm
Via Fill
Maximum Via Fill Finished Hole Size0.5 mm
Peelable Mask
See our PCB Design Guidelines on Peel-off Mask
Carbon
See our PCB Design Guidelines on Carbon Contacts
Heatsink Paste
See our PCB Design Guidelines on Heatsink Paste
Electrical Test
Minimum Test Pitch0.10 mm
Smallest Testable Pad0.05 mm
Test Voltageup to 1000V
Test Current100 mAAdjustable
Continuity TestCapacitance/

resistance 1 Ohm – 10 KOhm

Isolation TestCapacitance/

resistance up to 10 GOhm