7 PCB Layout Design Tips for Power Electronics

Designing PCBs for power electronics can be challenging due to the interconnected nature of electrical and thermal factors in these circuits. These boards must handle high voltage and current levels while ensuring effective heat dissipation and adhering to strict safety standards.

Highlights:

When designing a power electronics board:

1. Select copper thicknesses ranging from 35 to 105 µm for currents over 10 A.
2. Use high-thermal-conductivity materials like ceramics or PTFE laminates for high-power designs.
3. Integrate protection devices like fuses and current-limiting resistors for added safety.
4. Adhere to IPC and UL/IEC standards for thermal and electrical safety.

In this blog, you’ll learn 7 layout design techniques for creating reliable power electronics PCBs.

1. Do not cluster power components to prevent hot spots

Maximizing energy efficiency and heat dissipation is critical in power electronics circuits. Improper component placement can lead to energy losses and excessive heat buildup, degrading components and reducing reliability.

11 strategies to place components on a power electronics board

1. Place high-current components like voltage converters and power transistors away from the PCB edges. Ensure traces connected to these components are wide enough to safely support the required current.
2. Keep components that generate significant heat, like power transistors and diodes near heat sinks or thermal vias that can effectively dissipate heat away from the components.
3. Position highly integrated digital components, such as microcontrollers and processors, at the center of the board for better heat distribution.
4. Avoid clustering power components in the same area to prevent hotspots; opt for a linear arrangement instead.
5. Make sure the power supply components are as close as possible to keep the associated traces short.
6. Prioritize placing components carrying high currents (requiring the widest traces) first on the PCB.

• • Begin with key power supply components like the converter IC, followed by placing other power parts, such as the input capacitor, inductor, and output capacitor, closely together. Keeping them on the same board side helps reduce EMI and avoids impedance discontinuity caused by vias. Refer to layout suggestions on the component manufacturer’s datasheet.

To learn more, see how to select components and materials for power electronics PCBs.

7. Place IC converters close to the devices they supply power to minimize trace length.
8. Keep the high switching current (high di/dt) loops as narrow and compact as possible to minimize distributed inductance and prevent voltage spikes. Position the current and return paths directly on top of or adjacent to each other to reduce the loop area and minimize electromagnetic interference.

   
9. Place the analog control components last, as they require thin tracks and save space. One approach to managing them is to create functional subgroups and connect them accordingly.

   

10. Position large components such as MOSFETs, rectifiers, and capacitors on the top side of the PCB to prevent movement during soldering. Have the smaller components on the bottom side of the board.
11. Connect bypass or decoupling capacitors to the ground and position them as close as possible to the IC’s power pins to prevent noise and minimize ripple effects. For more tips, see decoupling capacitor placement guidelines.

    

    

Download our DFA handbook to learn how to cut assembly costs and speed up the production of your prototypes.

Design for Assembly Handbook

6 Chapters - 50 Pages - 70 Minute Read

What's Inside:

• Recommended layout for components
• Common PCB assembly defects
• Factors that impact the cost of the PCB assembly, including:
  • Component packages
  • Board assembly volumes

Download Now

2. Use thicker copper for power traces to reduce trace resistance

Poorly routed boards can lead to excessive power losses, increased electromagnetic interference, and hot spots. Power electronics engineers should follow these trace design tips to effectively route the PCB for power electronics.

11 best routing guidelines for power electronics PCBs

1. Use thicker copper in PCBs for high power to reduce heat buildup. This also allows you to have narrower traces on the board. Copper thicknesses ranging from 35 to 105 µm (1 to 3 oz/ft²) are commonly used for currents over 10 A.
2. Select the appropriate width of copper traces based on the expected current. Trace widths and vias should be sized for maximum current handling to prevent thermal stress and voltage drops.

• • For 10A, use at least 0.5mm (20mil) traces.
  • For 50A, use 1mm (40mil) or wider traces.

Always account for surge currents and transient responses. The table below provides additional guidance on trace widths and their current capacities, assuming the following conditions:

• • 1 oz/sq foot copper (0.035 mm thick).
  • 10°C rise on outer layers and 20°C rise on inner layers.
  • Traces are not close to or over heat sink areas.
  • High current trace groups are de-rated.

Table 1: Trace widths and their corresponding current capacity 

You can quickly calculate the trace width and current capacity using our tool.

PCB DESIGN TOOL

Trace Width, Current Capacity and Temperature Rise Calculator

TRY TOOL

3. Minimize the length of power traces to reduce inductance, which can cause voltage drops and EMI. Place power components, such as the input capacitor, inductor, and output capacitor of a DC-DC converter, as close together as possible to reduce trace length.
4. Isolate sensitive or high data rate signals from power traces and regulators, particularly if they operate as switching types.
5. Place traces carrying sensitive signals on layers that are isolated from power layers by a solid ground pour in a multilayer PCB.
6. Route high current traces on the outer layers of the PCB. If this isn’t feasible, utilize vias to interconnect multiple layers. For increased currents, employing multiple vias may be necessary. Keep in mind that vias with a diameter of 14 mil support currents up to 2A, while those with a diameter of 20 mil or more can handle currents up to 5A.
7. Avoid routing signal traces parallel to power traces on different layers to reduce the risk of signal coupling. Instead, aim to route them at a 90° angle whenever possible for optimal performance.
8. Remove the solder mask to expose the underlying copper and add additional solder to increase the copper thickness, reducing resistance and enabling the trace to carry higher currents. While not a standard design rule, this technique helps avoid increasing trace width while improving the trace’s power-handling capacity.
9. Use 10-mil inner ring feed-throughs for layouts, which provide a current capacity of approximately 1 A per feedthrough. So multiple vias may be needed to support higher currents.
10. When routing high-voltage circuits, consider using cutouts to increase creepage. Avoid placing large holes, as they can cause issues with the board’s structural integrity, causing it to crack.

    

11. Keep the size of the current loops as small as possible to reduce parasitic capacitance which occurs in circuits with high di/dt (rapid changes in current over time). It leads to voltage ringing, reducing the circuit’s overall efficiency.

Parasitic capacitance is most commonly observed in two critical areas of power conversion circuits:

• • Switching loop (hot loop): This loop runs from the input capacitor through the two switches and back to the capacitor. Known as the “hot loop” in power electronics, it is especially susceptible to parasitic inductance due to its high-frequency switching.
  • Gate loop: This loop connects the controller to the switches and back to the gate driver.

Sierra Circuits offers high-quality rigid PCBs for a wide range of applications with advanced technology, fast turnaround times, and precision manufacturing. Visit our rigid PCB capabilities to learn more.

3. Include bulk capacitors to stabilize the voltage supply

Ensuring a stable power delivery network (PDN) is crucial in power electronics. These circuits often operate under high voltage and current conditions, making it essential to maintain consistent voltage levels and minimize noise or ripple to prevent performance degradation.

12 power integrity considerations for power electronics prototypes

1. Use a solid ground plane to reduce noise and ensure power integrity.
   • Use solid, uninterrupted areas or large polygons for ground planes to provide low-impedance paths for high-return currents and facilitate heat dissipation from critical components.
   • Use a separate ground plane for power circuitry, connected to the system ground at one point to minimize interference.
   • Ensure good grounding practices on backplanes where high current switching occurs, to reduce ground noise and improve performance.
   • Place ground planes on both sides of the PCB to help absorb radiated EMI and reduce ground loop noise.
2. Provide clear separation between low-voltage and high-voltage sections of the board to mitigate noise and interference issues.
3. Place bypass capacitors as close as possible to the target components, on the same side of the board. Multiple capacitors may be needed for bulk or low or high-frequency filtering. For high-frequency noise, avoid vias when bypassing at MHz frequencies.

   

4. Include bulk capacitors to stabilize the voltage supply, especially for surge currents. Proper calculation of bulk capacitance (based on surge current and voltage drop) is essential for reliable power delivery.

   
5. Shield the load and sense circuits from high-frequency noise that can negatively affect its performance.
6. Ensure precise current sensing by carefully selecting and placing sense resistors. The resistor should be directly connected to the MOSFET output and the slot power to minimize errors.
7. Place the power controller, MOSFET, and sense resistor close together. This ensures proper operation and minimizes resistance in the current path.
8. Use a differential pair layout for the sense resistor, ensuring the sense voltage is measured directly across it. This minimizes errors from other circuit elements.
9. Connect the sense resistor in a differential pair to the hot plug controller. This ensures accurate voltage measurement across the sense resistor without interference from other PCB traces. A Kelvin connection for the sense resistor helps improve measurement accuracy by separating the voltage sensing path from the current path.

   

10. Place a 1 nF capacitor at the sense resistor input to the controller to filter out noise above 1 MHz. For optimal noise suppression, capacitors may also be placed on each side of the sense resistor to the ground, particularly for dealing with common-mode noise.
11. Noise on the ground plane can couple into the sense lines, especially in systems with high current switching (e.g., PCIX or PCIX-2 transceivers). Ensure that the ground and power planes are well-designed to handle the switching noise and prevent interference.
12. Bulk capacitors stabilize the power supply by providing surge current to the load.

    

    • • Calculate the bulk capacitance needed based on the surge current (I), voltage tolerance (∆V), and surge duration (∆t) using the formula:
        C=I×Δt/ΔV
    • Place bulk capacitors near the MOSFET input for the power supply and near the sense resistor output for the load.

To learn how to tackle power integrity challenges, see 4 common PDN design challenges and how to resolve them.

4. Implement shielding cans to mitigate EMI

Electromagnetic interference is a critical concern in designing power electronics PCBs, particularly caused by high-frequency switching in AC/DC converters. To avoid this, you need to incorporate the right filters and EMI shielding methods as discussed below.

10 tips to mitigate EMI in power electronics boards

1. Implement EMI shielding materials, such as conductive coatings (copper, silver, chromium, or nickel alloys) or metal shielding cans to block emissions.

   
2. Implement a Faraday cage in critical areas to contain electromagnetic fields and prevent radiated EMI from affecting nearby components or external systems. Make sure the shield is properly grounded to prevent resonance and maximize suppression.

   

3. Place filtering components, like feed-through capacitors, at critical points in the circuit to filter leakage and eliminate unwanted high-frequency noise in your power electronics PCB design.
4. Apply band stop filtering at the circuit’s natural frequency to mitigate current spikes. This may not be practical for complex designs with a high number of components.
5. Place sensitive components away from switching regulators. If unavoidable, shield sensitive components near switching regulators to block radiated EMI and preserve signal integrity.
6. Use guard traces around sensitive circuitry to block noise. Keep a consistent distance of 3W to 5W between the guard traces and the critical signal traces.

   

7. Isolate power planes for each supply when using multiple power supplies to prevent noise and ground loops from affecting sensitive circuits.
8. Use via stitching to create multiple low-impedance paths to the ground. Adjacent vias should generally be spaced between λ/20 and λ/10, where λ represents the signal’s operating wavelength. This technique helps mitigate the potential for radiation and noise coupling.

   
9. Incorporate a solid ground plane, if space permits, to enhance electromagnetic shielding and boost immunity to noise and crosstalk. Use a smaller ground plane for power components when space is limited.
10. Ensure compliance with relevant EMI standards and regulations such as FCC Section 15 and CISPR. Perform functional, environmental, EMI/EMC, and reliability (HALT and HASS) tests to ensure performance specifications are met.

Download our eBook to learn how to design high-speed PCBs with signal integrity.

High-Speed PCB Design Guide

8 Chapters - 115 Pages - 150 Minute Read

What's Inside:

• Explanations of signal integrity issues
• Understanding transmission lines and controlled impedance
• Selection process of high-speed PCB materials
• High-speed layout guidelines

Download Now

5. Insulate sensitive components to prevent thermal variations

Power electronics circuits generate a significant amount of heat, which can cause damage to components, reduce their lifespan, and even lead to circuit failure. Therefore, it is essential to consider PCB thermal management strategies from the early stages of PCB design.

13 ways to manage heat in your power electronics circuits

1. Always maintain the junction temperature below the maximum temperature specified in the manufacturer’s datasheet. It typically ranges from 125°C to 175°C for silicon-based devices.
2. For high-powered supplies, use PCB materials that offer higher thermal conductivity like ceramics or PTFE laminates (Teflon). Note that non-standard fabrication processes for these materials may increase manufacturing costs. Avoid materials with low thermal conductivity, such as FR-4.
3. Utilize thermal pads and conductive traces to channel heat toward the ground planes through vias, ensuring effective heat dissipation.
4. Thermally insulate sensitive components, such as regulators and amplifiers, to prevent thermal variations that can cause signal errors and reduce device reliability.
5. Place high-voltage signals on the external layers for enhanced thermal management. External layers have better heat dissipation due to increased exposure to ambient air than internal layers.
6. Utilize thermal vias and solid copper areas beneath high-heat components, along with traces of increased copper weight, to efficiently transfer heat away and prevent hot spots.

   
7. Optimize component placement on the PCB to ensure effective heat management. Space out heat-generating components, such as power transistors or diodes, to avoid heat accumulation. Position components in regions with adequate airflow to facilitate efficient heat dissipation.
8. Place components of individual power supplies close together to reduce trace lengths and parasitic inductance. However, spread out different power supply circuits across the board to prevent hot spots and ensure uniform temperature distribution.
9. Use passive cooling methods such as heat sink which is commonly used in power electronics.

   

   • Tailor the heat sink design to the specific component it cools, considering factors such as surface area.
   • Construct it from materials with high thermal conductivity, such as aluminum or copper.
   • Balance the size of the heat sink with available PCB space, ensuring that larger heat sinks, which dissipate more heat, are used appropriately without overcrowding the design.
10. Use bus bars to transfer heat away from heat-generating components, such as power transistors, capacitors, or high-current traces, to the surrounding areas or a heat sink. These are made of metal conductors like copper or aluminum, offering excellent high thermal conductivity.
11. Consider active cooling devices like fans or liquid cooling for applications with very high temperatures.

    
12. Use pyrolytic films that provide a tenfold increase in thermal conductivity. Panasonic’s diamond films, and heat control products offered by Bergquist, can be used between the heat sink and the components to ensure efficient thermal contact.
13. Mount the fan installed on the enclosure and power it directly from the input AC signal when converting power from a wall outlet to DC. For DC-to-DC power supplies, however, use a PWM signal to operate the fan and ensure effective cooling of your components.

6. Comply with IPC and UL/IEC design standards 

Power supply PCBs must comply with various industry standards, including IPC and other sector-specific guidelines to help prevent issues such as ESD and excessive conductor temperature rise.

4 design standards to follow for power electronics board

1. IPC-2221: Provides guidelines to ensure proper creepage and clearance distances between exposed conductors, reducing the risk of ESD in your power supply design.
2. IPC-2152: Recommends sizing of copper pours, power planes, and rails to manage current-carrying capacity and control temperature rise.
3. IPC-6012 and IPC-A-600: Defines standards for reliability, ensuring your design meets the appropriate class (Class 2 or Class 3) based on performance requirements.
4. UL/IEC safety standards: Ensures compliance with essential safety requirements across various industries and applications.

7. Adhere to safety considerations in power electronics board

Safety standards and precautions are critical in preventing hazards such as electrical shock, fire, or component failure. This is particularly true in applications like electric vehicles (EVs), where power electronics systems control large battery packs, drive motors, and charging circuits.

7 safety essentials when working with high energy level circuit board

1. Maintain adequate spacing and isolation between high-voltage nodes to prevent accidental contact that may cause arcing or short circuits. Follow standards such as IPC-2221 or IEC 60950-1 to define minimum creepage and clearance distances based on voltage levels, material properties, and environmental conditions.

   

   

   PCB DESIGN TOOL

   Conductor Spacing and Voltage Calculator

   TRY TOOL
2. Use appropriate insulation materials such as polyimide, teflon, or ceramic and ensure sufficient distance of high-voltage components from the user interfaces. Additionally, opt for materials with higher comparative tracking index (CTI) values, as this improves resistance to surface tracking and electrical breakdown.

Higher CTI also allows for smaller creepage distances between PCB conductors, enabling more compact designs.

Table 2: Comparative tracking index for PCB material selection

3. Integrate overcurrent protection devices such as fuses and current-limiting resistors for added safety.
4. Include overvoltage protection circuits such as transient voltage suppressors (TVS diodes) and varistors to safeguard sensitive components from voltage spikes.
   • TVS diodes: Clamp voltage spikes above a certain threshold to protect sensitive components.
   • Varistors: Offer nonlinear resistance that increases significantly with increasing voltage, limiting surge currents.
5. Design low-resistance safe discharge paths to handle stored energy effectively from components such as capacitors, inductors, and batteries that store significant amounts of energy during operation to prevent potential hazards like electrical shock, fires, or damage to components.
6. Apply conformal coating on sensitive areas of the PCB to prevent moisture, dust, or accidental contact from creating short circuits
7. Adhere to relevant safety standards for enclosure design.
   • Choose materials that meet UL (Underwriters Laboratories) or IEC (International Electrotechnical Commission) safety standards, such as flame-retardant plastics or metal casings.
   • Select an enclosure with an appropriate IP rating, such as IP65 or higher, to prevent dust, moisture, and other environmental factors from damaging the power electronics or creating short circuits.
   • Design the enclosure with proper ventilation, heat sinks, fan mounts, or vents to manage thermal buildup and ensure efficient heat transfer from internal components to the environment.
   • Ensure easy access to components for maintenance while ensuring safety features to prevent accidental contact with high-voltage areas when the enclosure is opened.

Safety should be prioritized from the beginning, rather than an afterthought.

Key takeaways:

1. Avoid clustering power components to prevent hot spots and ensure proper heat dissipation, improving component reliability.
2. Place heat-generating components like power transistors near heat sinks or thermal vias.
3. Design high-current paths to be short and wide to minimize resistance and inductance.
4. Expose copper and add solder for increased trace thickness and improved power-handling capacity.
5. Place bulk capacitors to stabilize voltage and handle surge currents, ensuring a steady power supply for the system.
6. Use solid ground planes to reduce noise and interference, connecting power circuitry ground to the system ground at a single point.
7. Implement shielding cans and grounded areas to reduce EMI and protect sensitive components.
8. Insulate sensitive components to mitigate thermal variations and prevent signal errors in power electronics designs.
9. Use bus bars for effective thermal management by transferring heat away from high-power components to surrounding areas or heat sinks.
10. Adhere to safety protocols such as adequate spacing, proper insulation, and protective components to prevent electrical hazards, especially in high-energy applications like electric vehicles (EVs).

Designing power electronics PCBs requires careful consideration of several important factors, including thermal management, high current traces, component placement, and compliance with EMI/EMC. By following these design considerations, designers can create robust and reliable power electronics circuits that meet the requirements of their applications.

Have questions on your prototype design? Post your queries on SierraConnect. Our PCB experts will answer them.