Section 13 – PCB Design: Solder Mask

This is the thirteenth section in the back-to-school series for PCB Designers and those who may want to know more about it. 

Contents

Solder Mask

Solder mask is a vital piece of the PCB puzzle. When looking at a bare printed circuit board, you see mostly the mask and the ink. Oddly enough, they are often left for last as we focus first on the actual connectivity. Let’s start with the solder mask and we will get to the marking in the next section. There are two basic types of solder masks, liquid photo-imageable (LPI) and dry film with LPI being the most common.

Dry film photo imageable solder mask is more like a sticker or two stickers held together with the solder mask. One side is peeled off and the remaining material goes over the entire board mask-side down. The areas where the metal is to remain exposed are masked off before curing it with ultraviolet light. Peel off the remaining side and clean the board. That’s the short version. Liquid mask follows a similar process except there’s no sticker.

It used to be green 100% of the time but then we got blue followed by one color after another. Black is the new blue as far as popularity. It provides the highest contrast with the white or yellow ink of the silkscreen and it looks cool too. You can buy a solder mask in a little bottle with a brush applicator or a pen to do touch-up work. For production, it comes in gallon-size jugs on up to big barrels.

The low-cost method of applying the LPI mask is by silkscreening it onto the board. The more accurate and costly method involves lasers to define the features. It is essentially an ink that cures to a high melting point and doesn’t readily burn. It will affect the impedance of outer-layer traces so there is a good reason to use a specific kind and control it to a thin coating.

Padstack editor for defining masks of circuit footprints

Figure 1: Image Credit: Author - The padstack editor is where the mask is defined for the footprints.

Solder Mask Slivers - A Leading Cause of PCB Defects

Solder mask adheres well to the surface but a narrow segment may still flake off. The so-called solder mask slivers are a reject. The designer needs to account for the minimum width of 100 microns (four mils) for a solder dam between any two mask openings. The IPC has developed a test method where adhesive tape of a specific stickiness is stuck on and ripped off of the board. (1) Then, we can check the tape to see if anything, conductive or non-conductive came off.

Once upon a time, I was the receiving inspector for the wireless group in a telecom outfit. When PCBs came in, the tape test was one of my jobs. We had the mylar 1:1 artwork to compare the circuit pattern on a light table. We had a machine that measured the thickness of the gold on the fingers and another that determined the average thickness of the copper barrel in the via. I could check for cracks in the barrel under a microscope.

We didn’t mask over the vias back then. I think most fab shops would still prefer that you didn’t. The holes don’t always fill completely with the mask. That potentially leaves a little pocket of air that might cause a blow-out when the board goes through the soldering process. It’s the shrinking electronics that drive the situation.

Anyway, there were pin gauges to check hole sizes, feeler gauges and a big block of granite to evaluate bow and twist. My lab even had an optical comparator to show the silhouette at 10X actual size to measure details of the board outline. It was an interesting job but I left before a toxic manager took over. I gave a two-week notice right there in the meeting with the out-going manager when the announcement was made. Then I lined up a cush job running a stock-room that lasted until I went off to ECAD school.

So, I digress. Out of all of the possible defects, more boards failed the tape test than the others. That knowledge stays with me as I design my footprints and boards. Most of the other issues were cosmetic having to do with contamination and a few were not flat enough to pass the spec. Working in assembly and inspection was a good background for the work I’m doing now. Moving on.

Containing the Solder During Reflow

Solder mask protects the bare copper while keeping the solder from spreading beyond its intended location. Plated through-hole and surface mount components both require a mask to ensure proper solderability. Through-hole pins can be drag soldered where the board is lowered into a bath of molten solder. Another method is wave soldering where the solder is made to well up under the stationary board.

Finally, there is pin-in-paste for mixed technology boards. The idea here is to add a relatively large area of paste on the side where the pins protrude through the board. The size of the paste stencil opening will be much bigger than the solder joint. The idea is to deposit enough paste in the area to fill the space between the pin and the hole with extra for a solder fillet.

Besides the hole diameter and pin size, the other factors are the thickness of the board and the thickness of the stencil. The paste is only added on the secondary side; it will be acceptable to have no solder fillet on the through-hole component side. It also means that the area around the bottom of the through-hole component has to be clear of other components or exposed metal.

We’re counting on a wicking action to draw in the solder paste while the SMD components are also reflowed. While this process can be tricky to dial in, the benefit is that the through-hole and secondary side components are all soldered at the same time. I’ve also seen over-pasting like that for BGAs where the aperture is a square that surrounds the circular BGA pad.

Vias and Solder Mask

Most PCBs have the vias covered with solde rmask. When the vias are designed with the solder mask opening, the fan-out vias have to account for the minimum dam plus expansion of the mask over both the soldered land and the opened via. Without the dam, the solder is prone to migrating into the via and leaving the connection with insufficient solder.

Good design practices require short power and ground loops so the vias are best held closely to the SMD pad. When the vias are open metal, you have to strike a balance between the two requirements. The easy way out is to cover the vias with a tent of solder mask on both sides.

Via-in-pad locations on a circuit board through solder mask openings

Figure 2. Image Credit: Author - Open mask on all of the vias can lead to some compromised fan-outs, especially on a densely populated board. The via-in-pad locations are filled while the vias in the random solder mask openings are left open.

While it is common with BGA packages to tent the component side and relieve the solder side, the vendors typically squawk at that idea because it’s hard to know where the solder mask is going to flow in that situation. The last thing they want to do is eat (or try to rework) those boards after getting all the way to the solder mask step.

Doing bring-up and trouble-shooting on analog systems can be a high-touch affair. A via that is tented with a mask doesn’t allow access with a circuit probe. While the technician can scrape off a little solder mask for rework, it shouldn’t be necessary just to take a voltage or current reading. It’s not an automated test solution because the vias are too small.

Underside of the board in a BGA with selected vias open

Figure 3. Image Credit: Author - Underside of the board in a BGA area with selected vias open to access the pin on the device.

Opening up the mask on all of the vias makes arranging the silkscreen more of a hassle. A workaround that satisfies most cases is to mask over the ground-vias while keeping the power and signal vias exposed. Finally, as above, a specific list of nets that require probing for bring-up are cleared of solder mask.

Graduate School Zone - Solder Mask Defined Pads

Fine pitch components may be required to have solder mask overlapping the pad. The threshold is the 100 micron minimum width mentioned above. Take, for instance, a 0.4 mm pitch BGA. It will have a ball diameter around 250 microns. A rule-of-thumb is that the pad size can be a minimum of 80% of the ball size. The only way to fan-out the BGA of that pitch is with micro-via-in-pad.

Not many fab shops, especially in the United States, will sign up for a 200 micron pad for the micro-via. Going overseas, I will comfortably design with 250 micron pads for the via with 50 micron overall expansion for the mask. On a 400 micron pitch, that leaves the IPC compliant 100 microns left over for the solder dam. I may get down to 224 microns for the capture pad if the mask expansion has to be 76 microns. It’s about silkscreening the mask vs. laser defined.

Bringing the fabrication for a 0.4 mm pitch BGA to the homeland, I would expect the vendor to require a 320 micron via pad which would then become the SMD pad size. That leaves an 80 micron air-gap. There’s no option to expand the mask and keep the 100 micron minimum dam. Contracting the mask by the 76 micron value creates a mask-defined pad-size of 244 microns. That leaves us a very acceptable 156 micron solder mask width.

You probably have noticed that I don’t usually go that deep into the numbers. When I do, it’s usually the metric system because that is the unit of measure for most of our components these days. Even when the pin-pitch is 100 mils, I’m likely to call it 2.54 mm. Board designers should be fluent in everything from angstrom units to inches. Avoiding the numbers makes you go and find out from your vendor. They all have a technology roadmap and no two are exactly the same.

Related Documents

  • IPC-SM-840 Qualification and Performance Specification of Permanent Solder Mask
  • IPC-7525 - Guidelines for Stencil Design
  • IPC-7527 - Requirements for Solder Paste Printing
  • IPC-7350 - Guidelines for Temperature profiling for Mass Soldering Process (Wave and Reflow)
  • IPC-HDBK-840 supplements the solder mask requirements established in IPC specifications

 (1)IPC-TM-650 Test Method 2.4.28.1, Adhesion, Solder Resist (Mask), Tape Test Method, defines the procedure for determining the adhesion of solder resists (masks) used over melting metals. The test method requires a roll of pressure sensitive self-adhesive film tape exhibiting an adhesive strength of at least 44 N/100 mm [40 oz-force/in] but no more than 66 N/100 mm [60 oz-force/in] as tested per ASTM D3330. Regular Scotch tape fits the bill along with others.

Next - Section 14: Silkscreen Marking

About the Author

John Burkhert

John Burkhert Jr is a career PCB Designer experienced in Military, Telecom, Consumer Hardware and lately, the Automotive industry. Originally, an RF specialist -- compelled to flip the bit now and then to fill the need for high-speed digital design. John enjoys playing bass and racing bikes when he's not writing about or performing PCB layout. You can find John on LinkedIn.

Follow on Linkedin More Content by John Burkhert
Previous Section
Section 12 – PCB Design: How to Design For Test
Section 12 – PCB Design: How to Design For Test

Learn about design for test, placing test points prior to routing, and more

Next Section
Section 14 – PCB Design: Silkscreen Marking
Section 14 – PCB Design: Silkscreen Marking

Learn about silkscreen marking, marking without a silkscreen, and more