Effective design means building with manufacturing limits in mind.
Everyone makes mistakes. In PCB design, design for manufacturing (DfM) is all about correcting mistakes after reviewing a PCB layout. We then devise corrective actions to fix those mistakes and improve procedures to make products error-free.
The term “PCB manufacturing” includes fabrication and assembly. Reliable and smooth PCB manufacturing requires DfM-compatible design practices. The journey begins with the schematic, followed by layout, which serves as the blueprint for the design. PCB design is a unique field where success depends on the designer’s understanding of fabrication and assembly technologies. We are no longer living in an era of simple designs that are easily manufactured.
Figure 1. Use industry standard or manufacturer-approved land patterns.
Indeed, PCB manufacturing involves state-of-the-art technologies and sophisticated procedures, requiring PCB designers to perform layout within manufacturing boundaries. At the layout stage, for example, tools are watching for electrical parameters, while at the fab and assembly stages the focus is solely on manufacturing criteria, i.e., size and spacing.
For example, at the design stage, a GND net should never come close to a POWER net to avoid a short. But two GND features (traces, vias, pins or shapes) can be placed close to each other, violating spacing constraints. PCB design tools would not mind it, since those are the same net features, whereas in manufacturing, the nature of the nets does not matter. Instead, the size of the smallest feature and the spacing between circuits are what matter. Hence, PCB layout is one of the unique fields of engineering where you design every bit of it, always considering the limits of manufacturing. It is a wonderful blend of art and science, giving birth to the term DfM.
Common DfM mistakes in PCB design are related to pad definitions of SMD and PTH pins and vias, component placement, trace routing, etc. These are major areas where a designer can influence the quality of PCB manufacturing. As in manufacturing, the designer should implement practices that ensure a good process capable of producing high yields. Here we chart out some design practices that can help prevent common fabrication and assembly defects.
Understanding manufacturer capabilities. At the start, finalize the fabricator and assembler and collaborate with design by going through their published processing capabilities. Understand those completely and resolve any ambiguities.
The tooling bridge. Understanding tooling requirements is essential when designing a PCB, as it ensures manufacturability and reliable assembly. Designers must account for assembly drawings, solder paste stencils and test fixtures to align with fabrication processes. Lack of tooling knowledge can lead to production errors and delays. Considering these factors early helps ensure a smooth and successful build. For example, consider the assembly of a press-fit pin component. These parts require specially designed tooling for installation, which in turn demands a dedicated area around the component free from tall components on both sides.
Define the land patterns. While developing the component footprints, adhere to the land pattern specs in its datasheet or by the manufacturer, and define all layers, specifically the solder mask and solder paste, per the requirements for both fabrication and assembly.
Verify all footprints carefully. Check pad sizes, numbering, spacing, orientations and so on. Incorrect footprints can cause placement, alignment and soldering issues on the assembly floor.
Critical rule for pad solder mask exposure. Manufacturing processes inherently involve tolerances, especially for solder mask layers. The solder mask is applied using an LPI (liquid photoimageable) process, which comes with an artwork alignment tolerance of ±2 mils. Designers must carefully design solder mask openings to avoid exposing any copper features from other nets, as this can result in shorts during soldering. To prevent solder bridging during automated soldering, copper features from other nets should be kept at least 4 mils away from solderable pads.
Silkscreen guidelines for component orientation. Define the silkscreen for each part, clearly indicating the PIN 1 location in its assembly layers. It helps to place the parts in the correct orientation on the assembly floor.
Toe and heel requirements for SMT pads. When designing SMT pads, ensure sufficient toe and heel; these are the parts of the pad that extend beyond and under the component lead. The toe helps solder flow and stick properly during reflow, while the heel gives the joint strength and stability. If these areas are too short, the risk is weak solder joints or misaligned parts. It is a small detail that makes a big difference in soldering quality. Hence, always follow standard pad guidelines to avoid trouble during assembly.
Drilling aspect ratio considerations. Based on the PCB thickness, look at the smallest hole (via drill) size in the design to ensure that the aspect ratio is within the manufacturing capabilities of the fab shop. For example, most bare board manufacturers can drill a PCB up to a maximum aspect ratio of 20:1. Failing to meet this can lead to plating voids due to high aspect ratio, low yield, costlier builds or even a “No Bid” from the manufacturer.
Annular ring requirements. For plated through-hole (PTH) components, pad sizes must be defined to ensure a proper annular ring. This ring is critical for reliable electrical and mechanical connections, even with drill wander/deflection. According to IPC Class II, an 90° annular ring breakout is acceptable. PCB fabricators demand an annular ring of 4 to 5 mils to meet IPC class II annular ring conditions. Always align pad and drill sizes with the fabrictor’s capabilities and IPC guidelines.
Component-to-edge clearance guidelines. When placing the components, ensure proper clearance of SMT and PTH parts from the edge of the PCB per the published guidelines of the assembler.
Rework considerations. Plan component placement as per the logic and keep the functionality intact. While placing components, always consider and plan for ease of rework. Leave space around components for tool access and avoid placing tall or heat-sensitive parts near areas likely to need repair. The layout should support safe use of soldering and rework tools.
Avoid solder mask slivers. In dense and HDI boards, always place components with a minimum width of solder mask web between the pads of the components. It should be in strict accordance with the manufacturer's recommendations. Failing to do so can cause it to lift off during manufacturing, creating a risk of shorting the different net SMD pads during the assembly process. If rework is not a concern, then SMDs can be placed with toe print to toe print spacing of 7 mils. This will permit a solder mask web of 3 mils, with individual solder mask clearance of 2 mils per side.
Figure 2. Careful routing will eliminate trapped chemicals.
Milling/routing/profiling requirement. During layout, make sure all routing copper features (traces, vias and shapes) are within a specified distance from the edge of the PCB per the defined parameters from the manufacturer. Failing to do so can cause the copper to be exposed near the PCB, possibly leading to an electrical short. The capability of the board edge to copper spacing varies from shop to shop; however, most fabricators support 8-10 mil edge clearance to avoid exposed copper at the board edge.
Base copper weight vs. copper feature spacing. Copper feature spacing requirements differ between inner and outer PCB layers. During PTH plating, copper builds up on the outer layers, increasing their thickness. This added copper height requires larger spacing between copper features on the outer layers compared to the inner ones, to ensure proper insulation and avoid shorts during the etching process. Additionally, the spacing of copper features depends on the base copper weight. The thicker the copper, the more spacing is needed to avoid shorts during the etching process.
So, always know your bare board manufacturer’s recommendations. Any parameter less than the minimum allowed value may lead to a higher build cost.
Know the cost of blind/buried vias. Based on the situation, blind or buried vias can be used, but add cost. They impact both the signal integrity and manufacturability of the PCB. So, use them only when a fine-pitch component cannot break using a mechanical via, or to avoid back-drilling against high-speed routing.
Smart PCB routing to increase production yield. Thin traces, sharp corners and tight spacing can trap chemicals during manufacturing, potentially causing corrosion or short circuits. To avoid these issues, follow standard routing rules. For example, avoid 90° routing or very sharp angles for traces, and add teardrops where traces connect to pads or vias to ensure reliable trace-to-pad junctions.
Heat balance in discrete component pads. Discrete components often have one pin connected to a thin trace and the other to a large copper area. This causes uneven heat transfer during soldering, which can lead to tombstoning of SMD parts. To prevent this, use thermal reliefs. They help balance heat flow between both pads, ensuring stable placement during assembly.
Designing for testability. To simplify debugging and validation, include dedicated test points (TP) on the PCB. These should be clearly marked and positioned for easy access, ideally on a single side of the board to reduce testing time and cost. Proper placement of test points helps ensure efficient and reliable inspection, which involves consideration of TP size, TP to TP pitch, TP to component spacing, TP to silk screen clearance and TP to board edge clearance.
Set constraints per design rule manual. PCB manufacturers each have their own minimum spacing requirements for shapes, pads (pins and vias) and traces, which are listed in their design rule manuals (DRM). These spacing values ensure that the board can be manufactured reliably without issues such as shorts or open circuits. Carefully review the DRM of the selected manufacturer and set the design constraints according to their specified limits. This helps avoid manufacturing defects and ensures that the design passes the required checks.
Akber Roy is CEO and founder of RUSH PCB Inc., a printed circuit design, fabrication and assembly company in Milpitas, CA; This email address is being protected from spambots. You need JavaScript enabled to view it..
