Soldermask

Introduction

The purpose of Soldermask (SM) is to provide a protective coating on the PCB against contamination, oxidisation, humidity, mechanical damage and electrical shorts.

The application of SM requires certain criteria to ensure that it has good adhesion, quality and reliability and the PCB layout has a major influence on this.

Generating Soldermask Data

The data output from a CAD system for SM is usually negative, this means that only the SM openings are output (usually as pads).

This format of output was inherited from the days before laser plotters or Direct Imaging (DI).

Copper Layer

Copper Layer

Green is the Soldermask Opening Layer Overlay

SM Pad Overlay

As the SM opening is usually larger than the copper pads it is advisable to consider the following points during the layout of the PCB.

  • Allow sufficient isolation between copper pads if a SM web/segment is required between them – See Pad-to-Pad (PP) in the tables below.
  • Allow sufficient isolation between tracks/plans and copper pads to ensure they are fully covered by SM – See Track-to-Pad (TP) in the tables below.

Soldermask Rules

The values below are the minimum we require to achieve a good and reliable SM application.

These are based on our production parameters and the SM specification.

The method of exposure used is defined by the SM colour.

DI Soldermask

Colours available – Green, Black, Red and Blue.

Advantages

  • Improved Registration Accuracy.
  • Smaller Mask Annular Ring (MAR).
  • Smaller Mask SegMent (MSM) or Web.
  • Smaller Mask Overlap Clearance (MOC).

Disadvantages

  • No White or Transparent Colours currently available due to the high energy required.


The table below contains the minimum values for DI Soldermask.

LDI
Soldermask
Colour
Minimum
MAR
MSM
MOC
Green
0.030mm 0.075mm 0.060mm SM Clearances
Black
0.030mm 0.075mm 0.060mm
Red
0.030mm 0.075mm 0.060mm
Blue
0.030mm 0.075mm 0.060mm

* Soldermask opening shave = 0.005mm Maximum.

MAR (Mask Annular Ring) – The clearance from the edge of SM to the edge of the copper pad.

MSM (Mask SegMent) – The bridge/web of SM between adjacent pads.

MOC (Mask Overlap Clearance) – Distance between a copper track/plane and an adjacent SM opening.

The table below shows the minimum Design Rule values to achieve the minimum LDI Soldermask values.

LDI
Soldermask
Colour
Minimum
PP
TP
Green
0.135mm 0.090mm Copper Clearances
Black
0.135mm 0.090mm
Red
0.135mm 0.090mm
Blue
0.135mm 0.090mm

PP (Pad to Pad) – The isolation between adjacent copper pads.

TP (Track to Pad) – The isolation between adjacent copper pads and tracks/plans.

TT (Track to Track) – The isolation between adjacent copper tracks/plans.

Photo Imageable Soldermask (PI)

Colours available – White or Transparent.

Advantages

  • Able to expose White or Transparent SM.

Disadvantages

  • Reduced Registration Accuracy.
  • Larger Mask Annular Ring (MAR) required.
  • Larger Mask SegMent (MSM) or Web.
  • Larger Mask Overlap Clearance (MOC) required.


The table below contains the minimum values for PI Soldermask.

Photo Imageable
Soldermask
Colour
Minimum
MAR
MSM
MOC
White
0.100mm 0.130mm 0.090mm SM Clearances
Transparent
0.100mm 0.130mm 0.090mm

** Soldermask opening shave = 0.040mm Maximum.

MAR (Mask Annular Ring) – The clearance from the edge of SM to the edge of the copper pad.

MSM (Mask SegMent) – The bridge/web of SM between adjacent pads.

MOC (Mask Overlap Clearance) – Distance between a copper track/plane and an adjacent SM opening.

The table below shows the minimum Design Rule values to achieve the minimum PI Soldermask values.

Photo Imageable
Soldermask
Colour
Minimum
PP
TP
White
0.330mm 0.190mm Copper Clearances
Transparent
0.330mm 0.190mm

PP (Pad to Pad) – The isolation between adjacent copper pads.

TP (Track to Pad) – The isolation between adjacent copper pads and tracks/plans.

TT (Track to Track) – The isolation between adjacent copper tracks/plans.


Soldermask segments less than he minimum MSM value will be removed as in the example below.

Original CAD Date

SM CAD Data

MSM less than Minimum Value

SM Production Data

Tented Via Holes

Where the copper pad of the Via Hole is to be covered with SM, it does not mean that the hole will be completely covered or closed by the SM.

Completely covered (Tented) Via Holes can only be guaranteed if Via Filling is used (See PCB Design Guidelines – Via Filling page).

IMPORTANT

If you require tented Via Holes, please make sure that you generate your SM data without SM pads for Via Holes.

Non-Plated Through Holes (NPTH)

NPTH with copper pads should follow the same rules as for Plated Holes.

NPTH without a copper pad will requires a Mask Annular Ring (MAR) of 0.125mm.

Board Outline

Always include the board outline in your SM data, this best done using a small line – e.g. 0.50mm wide.

The centre of the line should be exactly on the actual board outline (we will remove the line from the final production data).

IMPORTANT

If you require board edge areas of your PCB to be free of SM, use a wide line to indicate the board outline.

The line-width should be at least 2.00mm resulting in 1.00mm border free of SM.

It is also advisable to indicate that you require a border free of SM in the mechanical data.


Page Update History

25/06/2020 – DI Soldermask MSM (0.070 to 0.075mm) and PP (0.130 to 0.135mm) values Updated

Back to Top