With the rapid development of modern electronic technology, PCBA is also developing towards high density and high reliability. Although the current level of PCB and PCBA manufacturing processes has been greatly improved, the conventional PCB solder mask process will not have a fatal impact on product manufacturability. However, for devices with very small device pin spacing, due to the unreasonable design of PCB flux pads and PCB solder mask pads, it will increase the difficulty of SMT soldering process and increase the quality risk of PCBA surface mount processing. In view of the hidden problems of manufacturability and reliability caused by the unreasonable design of PCB flux and solder mask pads, combined with the actual process level of PCB and PCBA, the manufacturability problem can be avoided by optimizing the design of device packaging. The optimization design mainly starts from two aspects, one is the optimized design of PCB LAYOUT; the other is the optimized design of PCB engineering.

Current Situation of PCB Solder Mask Design
PCBA Solder Mask Design for Manufacturability Research
The PCB LAYOUT design is based on the IPC 7351 standard package library and the package design with reference to the pad size recommended in the device specification. In order to design quickly, Layout engineers give priority to increase and correct the design according to the recommended pad size. The length and width of the PCB soldering pads are increased by 0.1mm, and the solder mask pads are also based on the soldering pads. Increase by 0.1mm. As shown in Figure 1:
(Picture 1)

PCB engineering design The conventional PCB solder mask process requires that the edge of the soldering pad be covered by 0.05mm, and the solder mask bridge between the two soldering pads should be larger than 0.1mm, as shown in Figure 2 (2). In the PCB engineering design stage, when the solder mask pad size cannot be optimized and the solder mask bridge between the two pads is less than 0.1mm, the PCB project adopts the group pad window design process. As shown in Figure 2 (3):

(Figure II)

PCB Solder Mask Design Requirements
PCBA Solder Mask Design for Manufacturability Research
PCB LAYOUT design requires that when the edge spacing between the two flux pads is greater than 0.2mm, the package should be designed according to conventional pads; when the edge spacing between the two flux pads is less than 0.2mm, DFM is required. Optimized design, DFM optimized design methods include solder flux and solder mask pad size optimization. Ensure that the solder mask process solder resist can form a minimum solder mask bridge isolation pad when the PCB is fabricated. As shown in Figure 3:

(Figure 3)

PCB engineering design requires that when the distance between the edges of the two soldering pads is greater than 0.2mm or more, the engineering design shall be carried out according to the conventional requirements; when the distance between the edges of the two pads is less than 0.2mm, DFM design is required, and the DFM method of engineering design has resistance. Solder layer design optimization and flux layer copper trimming treatment; the size of copper trimming must refer to the device specification, the solder flux layer pad after copper trimming should be within the size range of the recommended pad design, and the PCB solder mask design should be single soldering Pad window design, that is, solder mask bridges can be covered between pads. Ensure that during the PCBA manufacturing process, there is a solder mask bridge between the two pads for isolation to avoid the appearance of soldering quality problems and electrical performance reliability problems.

PCBA Process Capability Requirements
PCB solder mask design for PCBA manufacturability research Solder mask can effectively prevent solder bridges and shorts during the soldering assembly process. The factory cannot guarantee the local welding quality of the product. For PCBs with high-density fine-pitch pins without solder resist for isolation, the current processing method of PCBA manufacturing plants is to determine that the PCB incoming materials are not good, and they will not be produced online. If the customer insists on going online, in order to avoid quality risks, the PCBA manufacturing factory will not guarantee the welding quality of the products. It is foreseen that the welding quality problems that occur during the manufacturing process of the PCBA factory will be dealt with through consultation.

case analysis
PCB solder mask design for PCBA manufacturability study The size of the device specification is as shown in Figure 4, the center distance of the device pins: 0.65mm, the pin width: 0.2~0.4mm, the pin length: 0.3~0. 5mm.
(Picture 4)

The actual design of PCB LAYOUT is as shown in Figure 5. The size of the soldering pad is 0.8*0.5mm, the size of the solder mask pad is 0.9*0.6mm, the center distance between the device pads is 0.65mm, and the distance between the soldering edges is 0.15mm. , The solder mask edge spacing is 0.05mm, and the unilateral solder mask width is increased by 0.05mm.
(Figure 5)

The PCB engineering design requires the conventional solder mask engineering design, and the size of the unilateral solder mask pad is required to be larger than the size of the flux pad by 0.05mm, otherwise there will be a risk of the solder mask covering the flux layer. As shown in Figure 5 above, the width of the unilateral solder mask is 0.05mm, which meets the requirements of solder mask production and processing. However, the distance between the edges of the two resist pads is only 0.05mm, which does not meet the minimum solder resist bridge process requirements. The engineering design directly designs the entire row of pins of the chip as a group pad type window design. As shown in Figure 6:

(Picture 6)

The actual welding effect is made according to the engineering design requirements, and the SMT patch is completed. Through functional test verification, the chip welding defect rate is above 50%; after passing the temperature cycle experiment again, the defect rate of more than 5% can be screened out. The first choice is to analyze the appearance of the device (20 times magnifying glass), and find that there are tin slag and solder residues between the adjacent pins of the chip; secondly, analyze the failed product and find that the failed chip pins are short-circuited and burned. As shown in Figure 7:

(Figure 7)

Optimization
PCBA Solder Mask Design for Manufacturability Research
The PCB LAYOUT design optimization refers to the IPC 7351 standard package library. The design of the flux pad is 1.2mm*0.3mm, the design of the solder mask pad is 1.3*0.4mm, and the center distance between adjacent pads remains unchanged at 0.65mm. . Through the above design, the size of unilateral solder mask of 0.05mm meets the requirements of PCB processing technology, and the distance between adjacent solder mask edges is 0.25mm to meet the solder mask bridge process. Increasing the redundant design of solder mask bridges can greatly reduce the risk of welding quality. , thereby improving the reliability of the product.

(Figure 8)

PCB engineering design optimization According to Figure 8, the width of the soldering flux pad is cut to copper, and the size of the solder mask width pad is adjusted. Ensure that the distance between the edges of the two soldering pads of the device is greater than 0.2mm, and the distance between the edges of the two soldering pads is greater than 0.1mm, and the lengths of the soldering and soldering pads remain unchanged. Meets manufacturability requirements for PCB solder mask single-pad window designs.
(Figure 9)

Demonstration program
PCB solder mask design for PCBA manufacturability research and design verification For the problem pads mentioned above, the pad and solder mask design are optimized through the above scheme, the edge spacing of adjacent pads is greater than 0.2mm, and the edge spacing of solder mask pads is greater than 0.1mm, this size can meet the requirements of solder mask bridge process. As shown in Figure 10:

(Figure 10)

Test yield comparison After optimizing the solder mask design from the PCB LAYOUT design and PCB engineering design, the organization re-supplied the same number of PCBs, and completed the placement and production according to the same process. The parameters of the products are compared in Table 1:

(Table I)

The above data can be obtained, the optimization scheme is verified to be effective, and the product manufacturability design is satisfied.

Optimal Design Summary
PCB solder mask design for PCBA manufacturability research In summary, chips with a device pin edge spacing less than 0.2mm cannot be designed in accordance with conventional packaging, and the width of the soldering pads in the PCB LAYOUT design will not be compensated. By lengthening the soldering pads Length circumvents solder contact area reliability issues. If the solder mask pad is too large and the distance between the two solder mask edges is too small, the copper cutting treatment is given priority; for the solder mask pad design is too large, optimize the solder mask design to effectively increase the edge width of the two solder mask pads, so as to ensure the PCBA Welding quality assurance. It can be seen that the coordination between solder flux and solder mask pad design plays a decisive role in improving PCBA manufacturability and solder pass-through rate.