Solder Mask Design – PCB DFM Part 6
6.1 Solder Mask Design for Copper Traces Generally, solder mask will cover copper traces, but in special cases, traces can be exposed according to the specific requirements.
6.2 Solder Mask Design for Holes6.2.1 Via Holes  Via holes should have solder mask openings on both sides of the board centered about the hole, as shown in Figure 33. The required diameter of the opening should be D + 5mil where D is the diameter of the plated hole. Figure 33: Solder Mask opening for via holes. 6.2.2 Alignment Holes  For metallic rivet holes, the solder mask opening should be centered about the rivet hole with a diameter + 6mil of the plated pad, on both sides. Figure 34: Metallic rivet hole solder mask opening.  For non-plated rivet holes, the solder mask opening should be greater than the clearance area for the screw head. Figure 35: Non-metallic rivet hole solder mask opening.  The solder mask openings for Type A wave soldered holes should satisfy: Figure 36: Type A mechanical hole solder mask opening. 6.2.3 Positioning Holes  The solder mask opening on the front and back sides of non-plated holes should be D +10mil, concentric about the hole, where D is the diameter of the non-plated hole. Figure 37: Solder mask opening for non-plated mechanical holes. 6.2.4 Buried and Plugged Vias  Internal vias (buried vias) do not require solder mask openings on either side of the board.  For PCBs requiring wave soldering or if the board has BGA (or CSP) with a pitch smaller than 1.00mm, the BGA via hole should be plugged.  If an in circuit testing (ICT) point is added under the BGA, it is recommended to lead out the testing pad from the via hole as shown in figure 38. The diameter of the test pads should be 32mil; solder mask opening is 40mil. Figure 38: BGA Testing pad.  If the PCB does not require wave soldering, and the pitch of BGA components is greater that 1.00mm, then there is no need for plugged vias. The BGA via itself can be used as a test point. The top side solder mask opening should be 5mil bigger than the diameter of the hole. The bottom side testing pad should be 32mil with a solder mask opening of 40mil.
6.3 Solder Pad Solder Mask Design Solder mask design for copper pads should follow figure 39. Figure 39: Solder mask openings for copper pads  Since PCB manufacturers have limited precision and limits on the minimum width of solder mask openings, solder mask openings should be at least 6mil bigger than pad size (3mil each side), with a minimum solder mask bridge width of 3mil. There must be solder mask separating pads and holes to prevent solder bridges from forming and causing short circuits. Figure 40: Solder mask openings and material widths for various copper pads. Table 7: Recommended minimum solder mask material width between pads.  Groups of SMD pads less than 0.5mm (20mil) apart or less than 10mil between the pad edges do not need solder mask to separate them and can be opened as a group. See figure 41. Figure 41: Solder mask openings for fine pitch SMD components  Solder mask openings are recommended for heatsink contacts.
6.4 Gold-Finger Solder Mask Design The copper pads of gold-finger connectors should open up the solder mask together. The top of the pads (where the trace is connected) should be opened flush with the solder mask material, and the bottom end solder mask opening should close beyond the edge of the board, as shown in figure 42. Figure 42: Solder mask opening for a gold-finger Seeed Studio Fusion prototype PCB manufacturing service offers 6 kinds of colors incluing green, blue, red, white, black, yellow for free, and Fusion Advanced PCB service even support purple and matt green color! More Chapters: 1. Brief Introduction 2. Seeed Fusion PCB Specification 3. Panelization and Bridge Design 4. Component Layout Considerations 5. PCB Hole design 6. Solder Mask Design 7. Copper Trace Design 8. Silkscreen Design 9. PCB Lamination Structure 10. PCB Dimensions Specification 11. Fiducial Mark Design 12. Surface Treatment 13. Files for Manufacture Requirements 14. Appendix