Design for eXcellence

Unit 2: Design for fabrication

Section 4: DfF - solder mask and finishing processes

Section Contents

Solder mask

As you will know from your studies of Materials and Processes for EDR, there are several different types of solder mask and a number of ways of applying it. However, most solder masks are photoimageable types: both liquid materials (LPISM = Liquid Photo-Imageable Solder Mask) and dry film materials are used, the former being by far the more common. For both types, a layer of material is applied to the entire board surface, dried (if liquid), exposed to ultraviolet light through an artwork, developed and finally cured, leaving just the apertures required in an otherwise impermeable and even coating of solder resist.

In practice, as we saw when considering plating thieves, the evenness of coat will depend on the profile of the copper tracks. So the typical capability statement1 extract in Table 1 gives different coverage thicknesses for the knee and the crest of the track.

1 All the specific figures on this page are based on the Circatex Capability Statement as at December 2002. They are representative of general practice within the industry, but you should always check with your supplier before deciding on a board specification.

Photo 1: Section through resist and track

Section through resist and track


Table 1: Solder mask design categories2
  volume capability  
dimension no review DfF review pilot/special
dam by wet weight
(on FR-4 laminate)
6 gsm
75 µm
50 µm
7 gsm
75 µm
50 µm
9 gsm
75 µm
50 µm
min aperture to copper
50 µm
40 µm
< 40 µm
breakdown voltage
500 V
1000 V
> 1000 V
track coverage
3 µm
5 µm
> 5 µm
8 µm
12 µm
> 12 µm

2 In the full Circatex version, this table includes mention of tented, covered and plugged vias (what these terms mean is explained in Materials and Processes for EDR). We haven’t included that topic in this module because tenting needs thick dry film solder mask, which is “bad news for fine-pitch assembly”. Most people have junked their dry film solder mask laminators, and almost all vias now produced are plugged. The current fashion is for LPISM, with vias plugged by a separate printing operation.

Solder mask apertures

The minimum aperture suggested is 50 µm larger than the copper pad which the solder mask surrounds. Whilst not at the limit of attainable accuracy, this is in line with designs using 100 µm gaps. The normal recommendation is that the aperture size should be determined by minimum pad-to-pad/track gaps on a design (Figure 1), and that standard apertures be used across the whole of the design.

Figure 1: Solder mask design features

Solder mask design features

However, as with line and space characteristics, the designer may opt to generate the solder mask layers as ‘pad to pad’ and allow the fabricator to adjust for his process. This gives the manufacturer the option of using different oversize openings for different features, and can improve manufacturability by minimising the areas where the tightest registration must be held.

Over-large apertures can present particular problems if they expose adjacent copper tracks (Figure 2), because this may lead to unwanted solder pick-up and short-circuits after soldering.

Figure 2: Effect of over-large solder mask apertures

Effect of over-large solder mask apertures


Photo 2: Effect of over-large solder mask aperture

Effect of over-large solder mask apertures


If the assembly operation does not require ‘pocket windows’, with a mask dam or ‘webbing’ between pads, fabricators will often recommend that designers use a ‘gang solder mask’ window (also known as a ‘postage stamp’ aperture) around fine pitch devices. The two different types of window are shown in Figure 3, from which it is clear that pocket windows need solder mask that is much better defined and in register than gang windows.

Figure 3: Solder mask window types

Solder mask window types

This means that, at the bare board level, gang older mask windows will give a higher yield than pocket windows. The gang window can even sometimes be manufactured by screen printing, using a 0.38 mm spacing, whereas solder mask pockets require clearances of 75–125 µm, and must therefore be made with photoimageable resist.

However, the standard apertures (also referred to as ‘pocket windows’) are needed if there are tracks between pads, and some assembly houses prefer the isolation this affords between solder areas. As shown in Figure 4, Circatex have the capability to process webbing down to 50 µm, but recommend a minimum width of 75 µm.

Figure 4: Minimum dimensions for solder mask webbing

Minimum dimensions for solder mask webbing

Two more thoughts about solder resist between pads, which are taken from Materials and Processes for EDR:

There are specific problems when solder resist is used to surround the pads for fine-pitch BGAs. With a pad size of 0.2 mm diameter on 0.5 mm pitch, allowing 75 µm all round window clearance demanded by the ±75 µm alignment tolerance is not a problem, because the web between pads will still be 150 µm wide. However, the designer may well wish to have some surface tracking: even with 100 µm tracks, it is not possible to guarantee that the solder mask alignment will be sufficiently good to cover the track. You will need to negotiate with your fabricator to find an acceptable compromise on size and positional tolerance.

Solder mask problems

A number of processing problems associated with solder mask have their origins in fine features in the design. For example, slivers of material can become detached and move during development, but are not totally removed from the board. The curing process which follows development will then bake the slivers into an inappropriate position, perhaps on a pad surface or down a plated through-hole. Either way, the result may be a reject assembly.

Photo 3: Solder resist sliver

Solder resist sliver


Photo 4: Solder resist in through hole

Solder resist in through hole

Other things that go wrong are more the fault of the layout designer. For example, all printing and placement machines need a clear view of fiducials in order to have an accurate alignment target, so the solder mask should be cut back from the fiducial as far as possible.

Photo 5: Fiducial (on board fret) with good solder mask clearance

Fiducial (on board fret) with good solder mask clearance

Provided that the CAM system has the net list information, and is programmed to review interconnections, then the fabricator will be able to detect problems such as that in Figure 5, where there is no solder mask aperture for some SMD pads.

Figure 5: Missing SMD clearance on solder mask

Missing SMD clearance on solder mask

A final caveat concerns keeping solder mask clear of parts that are attached mechanically. For example, if a board is retained by screws, these should act directly onto bare laminate or copper, and not onto a resist-coated surface, so that the resist is not damaged when the screw is tightened.

Photo 6: Keep solder mask away from screws!

Keep solder mask away from screws!

Self Assessment Questions

  1. Define solder mask ganging and pocket windows and explain under what circumstances you would use each.

  2. What sort of problems do assemblers see with solder mask?

compare your answer with this one

[back to top]

Additional prints

There are many Design for Fabrication considerations, of which Design for Fewest Processes is one key issue that affects not just the layout designer, but other members of the team. Ask questions such as “Do we really need legend?” “Do we need both score and rout?” Bear in mind that scoring will add 50p to the price of a panel, and printing 70p per side. If the process isn’t needed, don’t pay for it.

Alongside design for fewest processes is the absolute need to eliminate all but the most essential special processes, such as via plug, use of peelable resist, gold fingers, and so on. All additional processes cost money, and non-mainstream processes are more expensive. For example, ask whether you really need plugged vias – they are not needed to stop solder migration to the top surface.


Legend inks are available in a variety of colours and may be cured by UV or thermal methods. White is by far the most common colour selected and generally has the best contrast to the common masks in use. Other available colours are yellow, red, orange and blue. As with non-standard mask colours, a premium may be charged for non-standard legends, depending on the volume of the application.

Legend ink should be kept as far as practicable away from the copper features on a PCB, as indicated in Table 2:

Table 2: Legend (nomenclature) design categories
  volume capability  
dimension no review DfF review pilot/special
Minimum line width
200 µm
150 µm
Minimum aperture (to copper)
300 µm
150 µm
<150 µm

If there is contention between legend and other mask features, as in the top image of Figure 6, where the legends impinge on copper and solder mask, the fabricator will crop the legend as shown in the middle image. The final image shows the preferred starting point, which needs no correction.

Figure 6: Options for legend prints

Options for legend prints

One also has to bear in mind that screen printing is associated with fairly loose tolerances, both in positioning the print and because the ink tends to flow. Features such as lines surrounding pads to indicate component position should therefore be kept well clear of any solderable pads. Also, bearing in mind that legend prints have a third dimension, and are not totally flat, designers should not position legend under chip components, in order to avoid the possibility of drawbridging.

Photo 7: Incorrect component identification

Incorrect component identification

Peelable solder resist

Peelable resist is one of the thickest materials ever printed onto a board! Intended to withstand immersion during wave soldering, it is then removed by hand in order to reveal unsoldered pads intended for non-wet assembly.

Photo 8: Removing peelable solder mask

Removing peelable solder mask

As shown in Table 3, the definition of peelable solder mask print is not very good, but, because the material is thixotropic, it can be used successfully to tent even quite large vias.

Table 3: Peelable solder resist design categories
  volume capability  
dimension no review DfF review pilot/special
min. gap resist to copper
300 µm
250 µm
min. resist width
3 mm
2 mm
max. tented hole size
1.6 mm
1.8 mm
min. resist coverage
300 µm
250 µm

Edge connector plating

Another process carried out towards the end of manufacture is the plating of edge connectors. Electroless nickel and immersion gold are both inadequate materials for surfaces that will be subjected to continued rubbing, so electrolytic nickel and hard gold are used. This process requires that the areas to be plated are electrically connected to the cathode of the plating circuit, so a shorting bar is used, as indicated in Figure 7 (left).

Figure 7: Making electrical contact to gold-plated edge connectors

Making electrical contact to gold-plated edge connectorsMaking electrical contact to gold-plated edge connectors

Although the process may be continuous, in order to reduce the amount of gold used, most baths for this process immerse only part of the board. The panel layout therefore has to locate the edge connectors at opposite edges, as shown in Figure 7 (right), so that the board can be cut in half before plating. To reduce still further the usage of gold, areas not designed to be plated will be covered with a temporary plating resist.

An alternative approach preferred by some fabricators is to carry out the deep nickel/gold plating of areas for edge connectors, key pads, slip rings, and similar between the first drill and electroless copper/direct metallisation process steps. The plated areas are then protected by resist during much of the subsequent processing. This adds process and equipment complexity, but allows a much greater proportion of the panel to be used, and may be the cheaper option when quantities are high. As always, any requirement for electroplated nickel/gold should be discussed with your fabricator at an early stage in design.

[back to top]

Finishing steps


Final steps in manufacture include testing to ensure correctness of interconnection, and scoring and/or routing to define the board outline. The probing aspects are considered under Design for Test, but the practicalities of test should be borne in mind especially during panelisation. Although each of the three circuits making up the panel in Figure 8 is testable on its own, as panellised there is a small area (surrounded by the yellow rectangle) where the density of 0.050 inch connections exceeds the probing capabilities of the equipment. This means that the board cannot be tested completely in a single pass, which adds cost.

Figure 8: A problem for electrical test!

A problem for electrical test!

Note that, had the left-hand side circuit been rotated through 180°, the panel could have been tested in one operation. Unfortunately, this proposal for reducing cost could not be implemented, since all the other manufacturing fixtures had already been made. This is a small example of how much of the cost of a product is determined by decisions made early in the development life-cycle, a point we made in our very first unit.

Where impedance is important, it is also necessary to include coupons for TDR (time domain reflectrometry) test. These coupons are placed at 90° to each other, as shown in Figure 9, to ensure that all process variables are taken into account. Note that the fabricator will keep the coupons with the board to which they relate, even after the routing operation, until final measurements have verified that the impedances are correct.

Figure 9: TDR test coupons

TDR test coupons


Most smaller circuits are shipped to the customer in panels from which individual circuits will be broken. Separation can be effected by pre-scoring during fabrication, and then snapping after assembly, or by routing at the end of fabrication, leaving some break-off tabs to allow the assembler to press or snap the sub-units apart. This is not without risk, especially to chip ceramic capacitors, as has been pointed out in Materials and Process for EDR!

The common problem experienced by fabricators when sub-panels are requested is simply lack of sufficient information:

V-score requirements

Figure 10 is a PCB end view cross-section showing the V-score cut into the material before separation. The clearance indicated, which is typically 1.0 mm minimum, is to prevent the copper tracks from being damaged during the scoring process. Figure 11 shows a plan view of a representation of the board: the red stripe down the centre shows the keep-out area for any copper features or components.

Figure 10: Schematic cross-section of the V-score cut

Schematic cross-section of the V-score cut


Figure 11: Copper tracks too close to V-score

Copper tracks too close to V-score

Beware that scoring is prone to ‘run-out’, where the score is not parallel to the circuit, although a typical specification is that scores should be parallel to board edge to within ±0.15mm.

The score depth depends on the board thickness, and the figures for the thickness of the residual material shown in Table 4 have been selected to get good breakout:

Table 4: Recommended score depth as a function of board thickness
0.80 mm
1.00 mm
1.20 mm
1.60 mm
Residual (D)
0.25 mm
±0.05 mm
0.35 mm
±0.1 mm
0.35 mm
±0.1 mm
0.40 mm
7±0.1 mm

Note that, when the scored panel is broken up into individual boards, the size of the boards is greater than might be expected. This ‘increase’, illustrated in Figure 12, depends on where the actual break occurs, and on the geometry of the cutting blade used to separate the boards. For 1.6 mm boards, the typical web thickness W is 0.3 mm, and the extension k is 0.1–0.15 mm. Where scoring affects both sides of the board, the total increase in board dimension will be 2 × k, or 0.2–0.3 mm.

Figure 12: Dimensional increase due to scoring

Dimensional increase due to scoring


Routing is more expensive than V-scoring, but generally more accurate, and results in a vertical profile. With profiling, remember that a small radius on an internal corner means using a smaller diameter drill for the whole routing process, with increased costs due to breakage and quality issues. Particularly if your design has sections removed by internal routing, try and use wide radius corners.

Photo 9: View of a routed profile, showing rounded end and vertical sidewalls

View of a routed profile, showing rounded end and vertical sidewalls

Also remember to provide some weak points, so that each element will break away cleanly from the panel! By drilling small holes slightly inside the outline, as shown in Figure 13, the board can be encouraged to break at modest flexural stress, and the rough edges of the break can be kept within the boundary of the profiled board.

Figure 13: Break-out tab design

Break-out tab design


Photo 10: Break-out tab on a board

Break-out tab on a board

Clearances are important for post-assembly routing and for the in-board chamfers used to accommodate standard edge connectors. Figure 14 suggests a 3.0mm minimum clearance at both sides to accommodate the ‘over-run’ of the cutter: smaller clearances will require hand finishing.

Figure 14: Clearance required for in-board chamfers

Clearance required for in-board chamfers

Self Assessment Questions

  1. Explain why it is important to place silkscreen legend without contention with the copper features.

  2. What are the requirements of a fabricator when you are specifying sub-panels?

compare your answer with this one

[back to top]