I’ve been using a 1:1 ratio between my pads and solder mask openings in my Gerber files, as I understand that most fabricators prefer this approach. From what I’ve heard, many manufacturers apply their own global solder mask expansion based on factors like minimum solder mask webbing, especially for fine-pitch designs.
However, I’ve also been told that if the solder mask expansion isn’t consistent across the design, some fabricators may ignore my mask settings entirely and regenerate it based on the non-solder mask defined (NSMD) pads in the design.
Would it be better to use a 2 mil global solder mask expansion from the start, or is sticking to a 1:1 ratio still the best approach? What’s been your experience with fabricators and their handling of solder mask data?
Solder mask registration can vary significantly, so if you use a 1:1 ratio, you should be prepared for the possibility that some pads might be partially covered by the mask due to misalignment. Since some pads are Non-Solder Mask Defined (NSMD) while others are not, I’ve found that NSMD works best for BGAs in my experience.
For most components (resistors, capacitors, QFNs, QFPs), I typically use a 0.035mm solder mask expansion, while for BGAs, I apply a slightly larger expansion to account for potential registration shifts.
In the past I used to follow a 1:1 ratio for nearly every component (with the exceptions being fiducials and some custom-shaped mask/paste features). I always included fab notes instructing the manufacturer to adjust the solder mask expansion as needed for their processes, which typically set a minimum mask sliver of about 0.2 mm. More recently, I’ve shifted most layouts to use a global mask expansion of around +3 mils. For fine-pitch devices or when using solder mask defined (NSMD) pads, I dial the expansion back as required—but I aim for the maximum expansion that my design rules will allow. I also enforce minimum mask sliver rules (usually about 4 mils) to ensure consistent clearance.
I’ve been using a 2 mil global solder mask expansion on most of my designs for years. For vias, I generally keep the expansion at 0 or even slightly negative to control the opening size. For through-hole boards, I tend to use a 4 mil expansion—though I can’t pinpoint exactly why, it seems to work best in practice. I also enforce a minimum mask sliver of 4 mil to ensure consistent clearance.
I generally use a similar approach to Nikh, though expansion varies slightly depending on the footprint. I agree that providing 1:1 data and letting the fab adjust as needed is a practical approach, as they will optimize based on their process capabilities. One key advantage of this is when a design includes a mix of SMD and NSMD pads—especially for RF components’ GND pins. A skilled CAM department will expand those differently to maintain consistent finished pad sizes.
I use a 3 mil solder mask expansion but ensure a minimum 4 mil mask sliver where possible. For tight-pitch components with less than 10 mil spacing, I leave the mask 1:1 with the pad and add a fab note requesting adjustment as needed. This helps ensure proper mask clearance without assuming the fab’s default approach.
I use a 2–2.5 mil expansion for pads and 3 mil from hole edge for vias. I’m generally fine with fabricators adjusting mask expansion. However, for RF designs, I prefer full control to avoid unintended changes.
In my experience, capable fabricators often make thoughtful mask modifications that balance fabrication and assembly requirements. I’ve seen cases where CAM editors customized mask shapes for SMD BGA pads rather than simply applying global adjustments. This is why I prefer providing precise mask data with targeted expansions for different component types, along with clear fab notes for critical areas.
For solder mask expansion, I tailor values based on component types to balance manufacturability and reliability:
0402 to 0805 passives: 3 mil (0.075mm) per side.
0.5mm/0.4mm QFN: 2.7 mil (0.07mm) to accommodate tighter pitch while avoiding mask slivers.
1206 and larger components: 4 mil (0.1mm) for added clearance.
BGA: Adjusted case-by-case, as fabricators often apply their own rules for via-in-pad or NSMD pads.
Regarding vias near SMT pads, I avoid non-tented vias too close to components since they can pull solder away from the pad, affecting joint reliability. If a via must be close, I ensure there is a solder mask sliver between the via and the pad.