User Guides
Our User Guides provide step-by-step instructions on how to use our free online smart tools and other available software.
Tolerances on Printed Circuit Boards
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
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 | 0.10mm |
See our PCB Design Guidelines – Drilled Holes |
| Production Hole Oversize – Non-Plated | 0.00mm | |
|
STANDARD Hole Size Tolerance – Plated |
≤4.00mm +/- 0.10mm >4.00mm +/- 0.20mm |
Standard Tolerance Range – 0.20mm Standard Tolerance Range – 0.40mm |
|
MINIMUM 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 Ratio | 1:8 | Ratio of board thickness to production drill tool |
| Hole Positional Tolerance | 0.10mm | Hole to Hole |
| Minimum Hole to Hole Distance | 0.25mm |
Measured 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 Copper | 0.25mm | |
| Hole Wall Copper | ||
| Minimum Copper Thickness | 20μm | |
| Surface Finish Thickness | ||
| Lead-free Hot-Air Leveling | 1 – 30μm | |
| Electroless Gold over Nickel |
Ni:3 -6μm; Au: 0.05 – 0.10μm |
|
| Immersion Silver Thickness | 0.2 – 0.4μm | |
| Plated Hard Gold over Nickel | Ni: 3 – 6μm; Au: 1- 1.5μm | |
| Soldermask | ||
| Minimum Soldermask to Pad Clearance = Mask Annular Ring (MAR) – Plated Holes |
LDI – 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 Holes | 0.125mm | |
| Soldermask Thickness on Top of Conductors | >7μm | For more information see our Technical page on Soldermask |
| Soldermask Thickness on Conductor Edges | >7μm | For more information see our Technical page on Soldermask |
| Legend | ||
| Minimum Line Width | 0.10mm | |
| Minimum Height for Legibility | 1.00mm | |
| Legend to Soldermask Cut-Back (clipping) | 0.10mm | After clipping we also remove any bits of line smaller than 0.10mm |
| Break-Routing | ||
| Minimum Clearance Board Edge to Copper Tracks/Pads – Outer Layers | 0.25mm | 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 | 0.40mm | |
| Minimum Slot Finished Width | 0.50mm | |
| Profile Dimensional Tolerance | +/- 0.20mm | |
| Positional Tolerance Profile/Cut-Out to Hole | +/- 0.20mm | |
| Slot Dimensional Tolerance | Width: +/- 0.20mm Length: +/- 0.20mm |
|
| 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 | 0.80mm | |
| Minimum Clearance Board Edge to Copper Pattern – Outer and Inner Layers | 0.45mm | This to allow for the V-cut. If copper pattern is nearer to the board edge, use break routing |
| Profile Dimensional Tolerance after Separation | +/-0.30mm | |
| Rest Material | 0.45mm +/- 0.10mm | |
| Positional Tolerance Upper to Lower Score | +/- 0.15mm | |
| Minimum Score Depth | 0.15mm | |
| Edge Beveling | ||
| Nominal Bevel Angle | 30° +/- 5° | See our Technical page on Edge Connector Gold Surface |
| Rest Material | 0.25mm | |
| Via Fill | ||
| Maximum Via Fill Finished Hole Size | 0.5mm | See PCB Design Guidelines on Via Filling and our Technical page on Via Filling |
| 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 Pitch | 0.10mm | |
| Smallest Testable Pad | 0.05mm | |
| 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 |
|
Other ways to find help
Glossary
To simplify communication Eurocircuits uses abbreviations for many of these technical terms. Most of the technical terms and abbreviations are international standards in the Printed Circuit Board manufacturing industry. However to make it clear to everyone involved, we here present a list of technical terms and abbreviations along with their explanation.
Still need help?
Talk to our customer support via our online chat, telephone or email.