The Right Approach: Get Ready for ISO 9001 Version 6
Dan’s Biz Bookshelf: ‘Still Broke: Walmart’s Remarkable Transformation'
Driving Innovation: Depth Routing Processes—Achieving Unparalleled Precision in Complex PCBs
DFM 101: Edge Plating
March 18, 2022 | Anaya Vardya, American Standard CircuitsEstimated reading time: 4 minutes
One of the biggest challenges facing PCB designers is not understanding the cost drivers in the PCB manufacturing process. This article is the latest in a series that will discuss these cost drivers (from the PCB manufacturer’s perspective) and the design decisions that will impact product reliability.
What is Edge Plating?
Edge plating is the encapsulation of the edges of printed circuit boards to improve EMI shielding of higher frequency designs, as well as for improving chassis ground in systems. The requirement for edge plating is being implemented for single axis, as well as multiple axis edges of the circuit board, including all four edges.
Edge plating is created when a rout path is implemented prior to the metallization of the circuitry features of the printed circuit board and is sometimes referred to as “plated rout.” The design requirements for implementing this technology are dependent on the requirement for the number of edges of each board, the size of the board, and whether the boards will be delivered in a multi-up array.
Stability of the material used for manufacturing of the board will also play a part in the development of the routing requirements. Materials where the reinforcement is not the standard glass-reinforced FR-4 type may require an alternative routing design to improve the structure of the parts inside the panel that is used to carry the parts during manufacturing. The parts are processed still intact inside the carrier panel, also called an array, used for manufacturing and assembly, requiring the development of tabs in some cases for edge plating. For a single edge requiring plating, tabs may not be required for stability.
Development of Tabs for Transporting the Panels
The drawing on the left in Figure 2 shows how perforated tabs are implemented for a circuit that is manufactured in a multiple-up array. The requirement is that the tabs being used to hold the board in the array will be broken off after the assembly operation (also called singulation). Figure 2 (right) shows a solid tab that is placed at the plated rout process. In both cases the internal and external layer artwork around the tabs must be void of metal. This will prevent the metal from being exposed in the singulation process. When a solid tab is used, the tab is removed at the final fabrication stage using a router (the same router that removes standard parts from the carrier panels). Removal of the tab will leave a small protrusion along the edge of the part.
Also detailed are the minimum requirements for the dimensions of the tabs. Placement of the tabs is based on assembly requirements and materials being used to construct the circuits. Less dimensionally stable materials, typically non-reinforced materials, as well as thin (0.200”), will require additional tabs for stability in processing. Conservatively, the tabs are placed every two inches along the plated edges. For non-FR-4 materials this is more the rule.
Design Rules for Plated Edges
It is required that the plating not only encapsulate the edge of the panel, but that the plating also wrap around to the surface of the panel. This is shown in Figure 3, and the minimum distance the plating is required to wrap around to the surface is 0.015”. The wrap-around is required for internal processing and adhesion of the plating to the edge. Also detailed is the minimum distance a feature can be placed to the wrap around plating (0.010”) as well as the distance required for an adjacent routed feature (0.100”).
It is typical that the plating be continuous along the entire edge of the circuit, but interruptions in the plating can be designed with two methods. By placing a tab at the interruption, and subsequently removing it, the tab prevents the plating (Figure 4a). Alternatively, the plating interruptions can be removed at the final routing stages. The subsequent removal of the plating will leave a small tab or an indentation into the circuit (Figure 4b). The indentation is created when the router bit contacts the edge where the plating is removed and advances into the circuit to completely remove the plating. When the interruption of the plating is a minimum of 0.200” the use of a tab to prevent the continuous plating can be used. When less than 0.200” the edge will be plated entirely across and subsequently removed by the routing process described.
Edge plating typically involves the connection of one or more of the internal planes in a board. These planes extend to the edge of the board and are electrically connected by the plating process. Those layers are typically fabricated with a polarity border (ref. 0.050”) to prevent exposed copper when they are routed and removed from a panel.
Figure 4: a) By placing a tab at the interruption, and subsequently removing it, the tab prevents the plating; b) the subsequent removal of the plating will leave a small tab or an indentation into the circuit.
Understanding the cost drivers in PCB fabrication and early engagement between the designer and the fabricator are crucial elements that lead to cost-effective design success. Following your fabricator’s DFM guidelines is the first place to start.
Anaya?Vardya?is president and CEO of American Standard Circuits;?co-author of The Printed Circuit Designer’s Guide to…?Fundamentals of RF/Microwave PCBs?and?Flex and Rigid-Flex Fundamentals; and author of?Thermal Management: A Fabricator's Perspective.?Visit?I-007eBooks.com?to download these and other?free, educational?titles. He?also?co-authored?“Fundamentals of Printed Circuit Board?Technologies” and provides a discussion of flex and rigid flex PCBs at RealTime with… American Standard Circuits.
Share on:
Testimonial
"In a year when every marketing dollar mattered, I chose to keep I-Connect007 in our 2025 plan. Their commitment to high-quality, insightful content aligns with Koh Young’s values and helps readers navigate a changing industry. "
Brent Fischthal - Koh YoungSuggested Items
Closing the Loop on PCB Etching Waste
09/09/2025 | Shawn Stone, IECAs the PCB industry continues its push toward greener, more cost-efficient operations, Sigma Engineering’s Mecer System offers a comprehensive solution to two of the industry’s most persistent pain points: etchant consumption and rinse water waste. Designed as a modular, fully automated platform, the Mecer System regenerates spent copper etchants—both alkaline and acidic—and simultaneously recycles rinse water, transforming a traditionally linear chemical process into a closed-loop system.
Driving Innovation: Depth Routing Processes—Achieving Unparalleled Precision in Complex PCBs
09/08/2025 | Kurt Palmer -- Column: Driving InnovationIn PCB manufacturing, the demand for increasingly complex and miniaturized designs continually pushes the boundaries of traditional fabrication methods, including depth routing. Success in these applications demands not only on robust machinery but also sophisticated control functions. PCB manufacturers rely on advanced machine features and process methodologies to meet their precise depth routing goals. Here, I’ll explore some crucial functions that empower manufacturers to master complex depth routing challenges.
Trouble in Your Tank: Minimizing Small-via Defects for High-reliability PCBs
08/27/2025 | Michael Carano -- Column: Trouble in Your TankTo quote the comedian Stephen Wright, “If at first you don’t succeed, then skydiving is not for you.” That can be the battle cry when you find that only small-diameter vias are exhibiting voids. Why are small holes more prone to voids than larger vias when processed through electroless copper? There are several reasons.
The Government Circuit: Navigating New Trade Headwinds and New Partnerships
08/25/2025 | Chris Mitchell -- Column: The Government CircuitAs global trade winds continue to howl, the electronics manufacturing industry finds itself at a critical juncture. After months of warnings, the U.S. Government has implemented a broad array of tariff increases, with fresh duties hitting copper-based products, semiconductors, and imports from many nations. On the positive side, tentative trade agreements with Europe, China, Japan, and other nations are providing at least some clarity and counterbalance.
How Good Design Enables Sustainable PCBs
08/21/2025 | Gerry Partida, Summit InterconnectSustainability has become a key focus for PCB companies seeking to reduce waste, conserve energy, and optimize resources. While many discussions on sustainability center around materials or energy-efficient processes, PCB design is an often overlooked factor that lies at the heart of manufacturing. Good design practices, especially those based on established IPC standards, play a central role in enabling sustainable PCB production. By ensuring designs are manufacturable and reliable, engineers can significantly reduce the environmental impact of their products.