Save. Share. Connect.
Thursday, May 26, 2016
VOLUME - NUMBER
PCB and Test
Test and Assembly
SMT and Assembly
Assembly and Production
PCB and Production
Assembly and Production
PCB and Assembly
Assembly and Packaging
PCB and Manufacturing
SMT and Production
Test and Measurement
Components and Distribution
Production and Packaging
HOME / CURRENT ISSUE
Assembly and Production
Add Message Board
The Reality of Design for Assembly
Solder bridge caused by inadequate soldermask between a pad and via on the opposite side of the board.
By Noah Fenley, ACD, Richardson, TX
Understanding the concept behind design for assembly (DFA) is the key to a successful assembly. Unfortunately, this often includes an ongoing struggle to balance assembly, fabrication and layout ? these elements must work together in order for the process to run smoothly. It also is necessary to understand the requirements and limitations of each of the three elements. Enter the layout designer, who strives to create a product that is easy to assemble. The easier the product is to assemble, the lower the final product cost.
In order to design the best assembly, the layout designer must 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's abilities and the needs of the assembly itself.
DFA is more than placing components at a safe distance from one another. Today's fine pitch components push fabrication tolerances to their very limits. For proper footprint development, it is crucial to understand the fabrication shop's minimum solder mask webbing. In addition, copper land patterns should take soldermask webbing into account. Oversizing the width of the pin footprint should not eliminate the soldermask webbing. Soldermask ganging — combining the pins into one soldermask opening — increases the likelihood of shorts between the pins during assembly. Therefore, it is best to avoid ganging soldermask when possible.
Vias currently are a major factor in testability and DFA. Vias that are too close to a pin do not allow soldermask webbing, and this absence will starve the solder from the pin. The paste will travel through the via and short components on the opposite side of the board. Vias should be exposed for testability. Adequate clearance from pins allows test probes to reach the via and allows a soldermask web.
Vias also cause concern for cold solder joints. 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. Inadequate soldermask between a pad and via on the opposite side of the board can cause a solder bridge. In the case illustrated here, 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 the connector. These types of shorts are difficult to find because components must be removed to debug. Now consider connector placement. Allow ample room for mating connection and removal. Not all connectors are a single plug-in. Placing a component too close to a connector is a common mistake. The component blocks the end user from removing the connection. Even placing components on the edge of the board requires space. Several other connectors require wrenches or other tools to connect them correctly.
The Texas Instruments MicroStar BGA spec illustrates how to create an even solder ball for the strongest BGA joint.
Silkscreen is used for orientation and debug. A good silkscreen indicates the shape of the component, the orientation and any necessary labeling. Labels should be legible and not covered by other components. The end user must be able to identify any connectors, switches, or indicators for debug or configuration. The silkscreen is used during the layout portion to determine the components' physical placements as well as to prevent any component conflicts during assembly.
Footprint accuracy is the single most destructive mistake that a layout designer or engineer can make. Unfortunately, component specs are not standardized, footprint drawings are not always to scale and some specs are drawn from a bottom view as opposed to a top view. In addition, many components do not fit on the manufacturer's recommended footprint and the controlling dimensions are not always clear. But using a CAD tool built to verify footprints can save schedules and rework because it builds a model to a component's actual dimensions, as well as overlaying 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, row pitch, pin type, component spacing, pin toe and heel, pin width, and overall assembly review. Any one of these items can delay a schedule or cause a board to need rework. Many of these issues can result in scrapping an entire fabricated lot.
Pin pitch mistakes typically are made during the conversion from English to metric or vice versa. The other error made is not identifying the correct controlling dimensions. The majority of mechanical drawings include the controlling dimensions.
The MicroStar spec can be used as a guide to design the pin size for BGAs.
Pin pitch is a cumulative error and rarely is a problem with low pin-count items. The more pins a device contains, the larger the cumulative error becomes. For example, 0.5mm 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; however, on a 48-pin device, the difference grows to 0.007, causing the pin to no longer fit on the intended pad.
Row pitch does not suffer the same tendency 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 heal of the solder joint. Typically, pin type errors are made during the component lookup or a late bill of material (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 (SMD), "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."
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 Pin Size
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 majority 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. 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.
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.
Contact: ACD, 1250 American Pkwy., Richardson, TX 75081
469-624-5153 E-mail: email@example.com Web:
© 2015 USTECH. All Rights Reserved. |
Contact Us: 610-783-6100 | firstname.lastname@example.org
powered by GIM