Estimated reading time: 6 minutes

Fresh PCB Concepts: Assembly Challenges with Micro Components and Standard Solder Mask Practices

(Editor’s note: John Piccirilli of Alpha Circuit contributed to this column.)

Micro components have redefined what is possible in PCB design. With package sizes like 01005 and 0201 becoming more common in high-density layouts, designers are now expected to pack more performance into smaller spaces than ever before. While these advancements support miniaturization and functionality, they introduce new assembly challenges, particularly with traditional solder mask and legend application processes. Surface mount technology has given way to micro-sized components, and with them, additional problems. At these microscopic sizes, standard manufacturing practices often become problematic. 

The Simplicity and Complexity of Solder Mask
Solder masks insulate all copper features except the solderable areas of the PCB. During assembly, they prevent shorts caused by solder bridging. However, the thickness of the solder mask, which varies by application method and factory process, can now interfere with the reliable assembly of low-profile components.

There was an era in the PCB industry when solder mask and silkscreen were simple additions to a PCB. A PCB design engineer would only need to specify solder mask on both sides and legend ink on one side of the board. The PCB supplier would always deliver a board with green solder mask and white legend ink. 

Compared to other PCB manufacturing processes, the solder mask application is relatively straightforward and much simpler today than it was in the past. The PCB was coated, tack-cured, printed, developed, and final cured. Now, solder mask can be mixed to achieve virtually any color and finish desired, and different application methods yield different finished mask thicknesses.

Table 1 shows a general comparison of modern solder mask application methods and their typical thickness ranges:

Today, silkscreen machines, curtain coaters, spray systems, and inkjet tools have not only changed how solder mask is applied to the PCB, but also the imaging methods used. Table 2 shows four common methods for developing solder mask: 

The application and imaging variability between PCB suppliers also makes it difficult to define and control solder mask thickness in a tight specification. The best way to determine the solder mask thickness is to contact your PCB supplier and speak with one of their engineers. The First Article Report (FAR) also lists solder mask thickness. 

Micro Components Meet Macro Problems
Considering how mask is applied and the final thickness, how do we get consistent solder mask? IPC provides guidance through IPC-6012 and IPC-SM-840. However, the minimum thickness of 25 µm is for electrical performance, but a measurement location is not given. In addition, there is no maximum solder mask thickness specified for suppliers, but IPC-6012 provides for solder mask variations in manufacturing. The best way to get consistent solder mask thickness is to work with your PCB supplier. Most, if not all, PCB suppliers have a way to measure solder mask thickness. They can also make adjustments in the solder mask application process to get more consistent coverage when the application warrants tighter tolerances.

Micro components like 0201s and 01005s are incredibly sensitive to even minor variations in solder mask application. These packages sit very low on the PCB, and if the solder mask is too thick or uneven, especially under or near the pads, the component might not seat properly during reflow. 

In typical LPI mask processes, even 25–30 µm of cured thickness can cause assembly defects if it creeps into areas where the component leads need to rest flat. At these sizes, there is almost no tolerance for inconsistency. Uneven solder mask under a quad flat no-lead or land grid array, for example, can cause the package to rock, shift, or lift during reflow, resulting in opens or tombstoning.

To mitigate this, consider removing solder mask between pads on some tight-pitch components. I urge caution here. Be sure of the consequences of removing solder mask dams. Solder mask dams are there to prevent solder bridging during assembly. However, a “gang relief” approach often provides better results than trying to squeeze in dams where there’s no room. While mask dams are helpful for larger packages, they can become the root cause of soldering issues in dense areas. In addition, solder mask dams below 76 µm may likely not survive solder mask processing. 

I remember developing a panel when I was a solder mask tech. As I was conducting a visual check of the mask, I noticed an area that had broken solder mask dams. The engineering department reviewed the solder mask artwork and discovered the dams were below 76 µm. As the boards passed through the dryer during development, the dams broke because of the air pressure. We had to place the board on hold while we waited for customer input.

Minor misalignment will not be harmful to larger SMD components, as the pads are relatively large. A standard solder mask relief will work fine in those situations. The solder mask relief is smaller with micro components, and even the slightest misalignment can cause problems. This is where Dynamic Solder Mask Compensation (DSMC) is helpful. DSMC uses a camera system to locate fiducial marks and measure inherent material distortion caused by manufacturing. The machine then exposes the solder mask with a correction based on the PCB currently being exposed. This provides better accuracy and resolution than a typical phototool used to print the solder mask. 

Legend Ink: Helpful or Hazardous?
Solder mask is not the only concern. Silkscreen (legend) ink can also interfere with assembly when placed too close to micro components. Since legend is typically printed over solder mask, its height is often unregulated and inconsistent. If legend ink ends up under a component, even slightly, it can prevent flush seating and cause pickup or placement issues during SMT assembly.

Imagine an entire production line put on hold because of unnecessary silk screen markings, like component outlines. The component outline could have caused the component to rock slightly, making it impossible to place reliably on the PCB. In high-density layouts, that tiny misstep can mean costly delays.

To avoid this, keep all reference designators and markings at least 0.15 mm away from fine-pitch or low-profile component pads. If space is tight, consider omitting legend altogether in these zones, especially component outline markings. Use a dot to mark the reference pin. 

Best Practices for Designers

The good news is that many of these challenges are avoidable with proactive design and clear communication. Here are some key recommendations:

• Communicate with your supplier about their specific mask application method and finished solder mask thickness.
• Specify solder mask thickness ranges only if your application is highly sensitive. Be reasonable. Tolerances that are too tight may cause your list of PCB suppliers to decrease quickly.
• Consider using solder mask gang relief instead of dams in micro component areas. Once again, I urge caution here. 
• Keep legend clearances generous, especially for low-profile components.
• Consider removing legend component outlines; instead, use a dot to mark the reference pin of the component.
• Do not specify solder mask by brand; instead, specify the performance needs, such as resolution and accuracy. 

Keep in mind that volatiles in the solder mask can affect the final thickness. How you cure and bake the mask can cause it to shrink or swell, adding another layer of variability that most drawings fail to capture. When solder mask swells, it typically indicates a problem with the solder mask process, not the PCB design. 

Conclusion
As component sizes shrink and board complexity grows, engineers must reexamine processes once considered “standard.” The solder mask and legend ink that once served as simple finishing touches are now critical elements that can make—or—break a high-density PCB assembly. Miniaturization requires the solder mask to be as flat as possible. 

The micro components of today demand precision not just in layout, but in every step of manufacturing. Engineers who understand how solder mask is applied—and how much of it ends up on the board—can achieve first-pass success and avoid a frustrating rework cycle.

When in doubt, ask your supplier how they handle solder mask and legend near fine-pitch components. It’s a small conversation that could save you a big headache later.

Ryan Miller is a field applications engineer with NCAB Group.