Design for assembly (DFA) is an ongoing struggle to balance assembly, fabrication and layout. The layout designer strives to create a product with ease of assembly in mind. The easier the product is to assemble, the cheaper the final product. In order to design the best assembly, the layout designer needs to understand the fabrication limitations of the components and the fabrication shop. The layout designer is a mediator between the requirements of the engineer, the fabrication shop abilities and the needs of assembly.
DFA is more than placing components at a safe distance from one another. The small pitch components of today are pushing the limits of fabrication tolerances. Understanding the fabrication shop’s minimum soldermask webbing is crucial for footprint development. Copper land patterns should take soldermask webbing into account. Oversizing the width of the pin footprint should not eliminate the soldermask webbing. Combining the pins into one soldermask opening is called soldermask ganging. Soldermask ganging increases the likelihood of shorts between the pins during assembly. Avoid ganging soldermask when possible.
Vias are a major factor in testability and DFA. Vias that are too close to a pin do not allow a soldermask webbing. The absence of the webbing will starve the solder from the pin. The paste will travel through the via and short components on the opposite board. Vias should be exposed for testability. Adequate clearance from pins allows test probes to reach the via and allows a soldermask web. Vias are concern for cold solder joints as well. On a multi-lamination board with four or more ground fills, a direct connect via can absorb the heat into the planes and cause cold solder joints.
Figure 1 shows a solder bridge caused by inadequate soldermask between a pad and via on the opposite side of the board. The pin also suffered from solder starvation since the solder was wicked away from the pin. The solder that was wicked away caused a short fount under connector in the image. Shorts of this nature are difficult to find since components must be removed to debug.
Consider connector placement. Allow ample room for mating connection and room to allow removal. Not all connectors are a single plug in. A common mistake is to place a component too close to a connector. The component blocks the end user from removing the connection. Even placing components on the edge of the board requires space. SMAs and several other connectors require wrenches or other tools to connect them correctly (Figure 2).
Silkscreen is used for orientation and debug. A good silkscreen will indicate the shape of the component, the orientation and any necessary labeling. Labels should be legible and not covered by other components. The end user needs to be able to identify any connectors, switches, or indicators for debug or configuration. The silkscreen is used during the layout portion to determine the physical placement of the components. Accurate silkscreen will prevent component conflicts during assembly (Figure 3).
Footprint accuracy is the single most destructive mistake a layout designer or engineer can make. The component specs are not standardized. Footprint drawings are not always to scale. Some specs are drawn from a bottom view as opposed to a top view. Many components do not fit on the manufacturer recommended footprint. The controlling dimensions are not always clear.
Using a CAD tool built to verify footprints can save schedules and rework. These tools have the ability to build a model to the dimensions of the component. The tool is able to overlay the model of the physical component over the footprint generated in the design tool. Using the latest spec ensures that the component is the latest revision.
The DFA check covers pin pitch (Figure 4), row pitch (Figure 5), pin type, component spacing, pin toe and heel (Figure 6), pin width (Figure 7) and overall assembly review.
Any one of these items can delay a schedule or cause unattractive rework on a board. Many of the issues will scrap a complete lot of fabrication (Figure 8).
Pin pitch mistakes typically are made during the conversion from mils to mm or vice versa. The other error made is not identifying the correct controlling dimensions. The majority of mechanical drawings will include the controlling dimensions. Pin pitch is a cumulative error. On low pin count items it rarely is a problem. The more pins a device contains, the larger the cumulative error becomes. For example, 0.5 mm converted to mils equals 0.019685. A common mistake is to round up to .020 or 20 mil, with the difference being 0.000315. The difference is not enough in a 6-pin device to cause assembly issues. On a 48-pin device, however, the difference grows to .007. Now the pin no longer fits on the intended pad.
Row pitch does not suffer the same ability for cumulative errors except on multi-row/column components. Ball grid arrays (BGA) and connectors should be built in the original dimensions. Row pitch on quads can force a designer to use smaller pads on the corners or increase the toe while decreasing the heel of the solder joint.
Typically, pin type is a mistake that is made during the component look up or a late BOM change. The manufacturer part specs are accurate between SMT and through-hole pins. The conflict arises on mounting holes. Many manufacturer specs do not indicate if the mounting pins are plated or non-plated. Press fit pins require a tighter tolerance and should be noted in the fabrication and assembly drawings. Component spacing affects the initial placement and the effort level of rework. BGAs require room for rework or the surrounding components will need to be removed before the BGAs can be removed.
Pin toe and heel are critical for a solid solder joint. According to Texas Instruments’ solder pad recommendations for surface mount devices, “The criteria for a well-designed solder joint is based on both empirical data and reliability testing. Solder joint strength is directly related to the total solder volume. An observable solder fillet is evidence of proper wetting.
Therefore, a positive solder fillet is usually specified. A joint can be described by the solder fillets formed between the device pins and the PCB pads.”1
Pin width also is a factor to consider. The expected assembly process will help determine the width variations for the pin width increase. Wave solder boards will need a wider pad than reflow boards. A major concern when making the pads wider is the soldermask webbing. The soldermask webbing between the pins prevents shorts.
BGA soldermask and routing on the assembled side can destroy assembly yields. The smaller the BGA pin pitch, the more crucial the soldermask becomes. The Texas Instruments MicroStar BGA spec illustrates how to create an even solder ball for the strongest BGA joint (Figure 9).
The majorities of the manufacturer’s drawings do not show the actual pin diameter but rather the ball diameter. The MicroStar spec can be used as a guide to design the pin size for BGAs (Figure 10). Some manufacturers have started using the pin size instead of the ball size. These few specs match with the MicroStar spec guidelines. Once the pad is the correct size, the routing must be considered as well for reliable assembly. Gang routing the powers and/or grounds will cause the ball to deform. The shape change will cause shorts and opens on the BGAs. Each pin should have a via to allow a low inductive path and to prevent the ball from deforming.2
DFA is continuous process in which assembly, fabrication and layout must all work together. Understanding the requirements of each is key to creating a successful, smoothly running assembly. The layout designer plays an important role in this, acting as a mediator between the engineer, fabrication shop and assembly needs.
As published in the PCB West 2012 conference proceedings. For more information, contact Noah Fenley, CID, Design Manager, at ACD, 1250 American Pkwy, Richardson, TX 75081; 469-624-5153; E-mail: email@example.com; Web site: www.acdusa.com.