What Tolerances should I Design into my PCB?

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

Eurocircuits use 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.

Specification Table

Description
Tolerance
Notes
Materials
Material thickness +/- 10% Based on Manufacturers’ Specifications
Maximum Bow and Twist on Boards with SMDs 0.75% See our Blog – Bow and Twist in Printed Circuits
Maximum Bow and Twist on Boards without SMDs 1.5%
Drilling
Production Hole Oversize – Plated 0.10 mm

See our PCB Design Guidelines on Holes Section

Production Hole Oversize – Non-Plated 0.00 mm
Hole Size Tolerance – Plated

+/- 0.10 mm

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

+/- 0.05 mm

Aspect Ratio 1:8 Ratio of board thickness to production drill tool
Hole Positional Tolerance 0.10 mm Hole to Hole
Minimum Hole to Hole Distance 0.25 mm Measured from production hole to production hole.

See our PCB Design Guidelines on Overlapping Drill Holes (point 9) and our Technical blog – The Smallest Possible Distance Between Two Holes

Minimum Non-Plated Production Hole to Copper 0.25 mm
Hole Wall Copper
Minimum Copper Thickness 20 μm
Surface Finish Thickness
Lead-free Hot-Air Leveling 1 – 30 μm
Electroless Gold over Nickel Ni:3 -6 μm;

Au: 0.05 – 0.10 μm

Immersion Silver Thickness 0.2 – 0.4 μm
Plated Hard Gold over Nickel Ni: 3 – 6 μm; Au: 1- 1.5 μm
Soldermask
Minimum Soldermask to Pad Clearance = Mask Annular Ring (MAR) – Plated Holes 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) 0.10 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) 0.10 mm
Minimum Soldermask to Pad Clearance = Mask Annular Ring (MAR) – Non-Plated Holes 0.125 mm
Maximum Via Filling Finished Hole Size (ENDSIZE) Resin or Soldermask 0.50 mm See PCB Design Guidelines on Via Filling and our Technical page on Via Filling
Soldermask Thickness on Top of Conductors >7 μm For more information see our Technical page on Soldermask
Soldermask Thickness on Conductor Edges >7 μm For more information see our Technical page on Soldermask
Legend
Minimum Line Width 0.17 mm
Minimum Height for Legibility 1.00 mm
Legend to Soldermask Cut-Back (clipping) 0.10 mm After clipping we also remove any bits of line smaller than 0.17 mm
Break-Routing
Minimum Clearance Board Edge to Copper Tracks/Pads – Outer Layers 0.25 mm Copper 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 Layers 0.40 mm
Minimum Slot Finished Width 0.50 mm
Profile Dimensional Tolerance +/- 0.20 mm
Positional Tolerance Profile/Cut-Out to Hole +/- 0.20 mm
Slot Dimensional Tolerance Width: +/- 0.10 mm

Length: +/- 0.20 mm

Minimum Copper Around Plated and Non-Plated Slots As annular ring for plated and non-plated holes
Scoring/V-Cut
Maximum Board Thickness for Scoring 2.00 mm
Minimum Board Thickness for Scoring 0.80 mm
Minimum Clearance Board Edge to Copper Pattern – Outer and Inner Layers 0.45 mm This to allow for the V-cut. If copper pattern is nearer to the board edge, use break routing
Profile Dimensional Tolerance after Separation 0.30 mm
Rest Material 0.45 mm +/- 0.10 mm
Positional Tolerance Upper to Lower Score +/- 0.25 mm
Minimum Score Depth 0.15 mm
Edge Beveling
Nominal Bevel Angle 30° +/- 5° See our Technical page on Edge Connector Gold Surface
Rest Material 0.25 mm
Via Fill
Maximum Via Fill Finished Hole Size 0.5 mm
Peelable Mask
See our PCB Design Guidelines on Peel-off Mask
Carbon
See our PCB Design Guidelines on Carbon
Heatsink Paste
See our PCB Design Guidelines on Heatsink Paste
Electrical Test
Minimum Test Pitch 0.10 mm
Smallest Testable Pad 0.05 mm
Test Voltage up to 1000V
Test Current 100 mA Adjustable
Continuity Test Capacitance/

resistance 1 Ohm – 10 KOhm

Isolation Test Capacitance/

resistance up to 10 GOhm