The Importance of PCB Line Spacing for Creepage and Clearance

by | Dec 11, 2020 | 0 comments

The PCB line spacing for creepage and clearance becomes an important factor from a product safety viewpoint when the standard operating voltage is above 30VAC or 60VDC. Voltages above these levels are considered hazardous, and that is why these designs are regarded as high voltage.

In high-density interconnect PCBs, maintaining a minimum line spacing between traces is quite a challenging task. Creepage and clearance distances of the traces become important at high voltages.

Designing a high-voltage circuit board requires good knowledge of international safety standards and regulations such as IPC 2221A and UL 60950-1. Following these IPC standards ensures that the final product is safe and functional. These standards are designed considering the safety of human beings operating the product and other equipment in the vicinity.

A designer will need to have a thorough understanding of parameters such as insulation resistance of dielectric, dielectric breakdown voltage, board material, leakage current, clearance and creepage, and tracking and operating conditions such as humidity and moisture altitude. To confirm that the board is designed as per the safety standard, one needs to test it in a lab environment using test equipment. This process helps to find any issues which may come up in the future during the operation due to environmental conditions or high voltages.

In this blog post, we will take you through the following essential aspects of line spacing for creepage and clearance:

Importance of PCB line spacing

The shifting trend towards miniaturization of electronic circuitry poses substantial challenges to the designer, specifically in hybrid technology that includes high-voltage circuits. Most of the electronic circuits require a compact PCB design, whether it is your smartphone or handheld medical imaging systems. Earlier, the use of high-voltage boards as a separate board was a common practice in a multi-board system.

With miniaturization, it is possible to merge multiple boards, which also allows the designer to utilize mixed technologies, including analog, digital, and RF circuits. The PCB line spacing considerations have become a primary concern for manufacturers as high-voltage circuits require additional rules to form increased electrical clearances and isolation for operator safety. These rules help to find ways for implementing precise circuit formation and reducing overall product size.

Sierra Circuits has developed certain standards based on the copper weight that mention required PCB line spacing for proper operation. Trace width and spacing which can be manufactured are given in the table.

PCB Trace width and line spacing

Trace width and spacing based on Copper for inner and outer PCB layers.

Trace Width Calculator

What is the minimum PCB line/trace spacing?

The minimum line spacing between PCB components and other traces is the distance required to withstand a given voltage. It is defined in terms of creepage and clearance distances. Factors such as voltage, application, and the type of PCB assembly play a key role in determining the minimum PCB line spacing requirements. It is difficult to derive a single solution to specify minimum spacing for multiple applications. The distance between the two PCB traces is measured by various methods and calculations, keeping the standards for clearance and creepage in mind.

What are creepage and clearance distances?

Creepage is the shortest distance between conductor traces on a PCB along the surface of the insulation material while clearance is defined as the minimum distance through the air (line of sight) between two conductor traces.

PCB clearance and creepage distance

Clearance and creepage distances between two PCB conductors.

Unlike clearance, which is measured in air, creepage is measured along the surface of the insulation material. While dealing with high-voltage designs, it is essential for designers to know the difference between both creepage and clearance rules. 

How contamination affects the PCB surface?

The trace gets stemmed due to contamination of dust particles and moisture, resulting in current leakage from one or two conductors. This can cause a slow breakdown of the surface of the insulating material between the conductors. The breakdown of the surface may be caused due to a voltage spike. The constant high voltage whose comparative tracking index (CTI) is too low will lead to a breakdown of the surface.

Comparative Tracking Index (CTI) for PCB material selection

Comparative tracking index (CTI) defines the electrical voltage breakdown of the insulation material of PCB caused due to environmental conditions such as dirt and moisture. It indicates the ability of the PCB substrate to withstand any breakdown between two tracks on the PCB surface. It is used to assess the proportionate resistance of the PCB base material and helps calculate the high-voltage isolation values between the tracks. The CTI value indicates how resistant the PCB material is against environmental influences such as dirt and moisture. The higher the CTI value of the material, the more resistant it becomes for a breakdown. The default CTI value for FR4 is 175 and goes up to 600 on special materials.

CTI values help to deduce the overall PCB tracking resistance. These values give an estimation for leakage or short-circuit as trace spacing becomes small due to component density. As per the IEC-60112 standard, a higher CTI grade substrate offers good resistance to electrical breakdown. CTI is a critical number while selecting a PCB material. IEC has prescribed three of the following classes for PCB CTI calculation:

Comparative tracking index values for PCB material selection

CTI values help to deduce the overall PCB tracking resistance.

CTI is the measurement of the susceptibility of the PCB’s insulating material to the electrical breakdown. CTI is that voltage, which results in failure by breakdown after 50 drops of 0.1 percent ammonium chloride solution has fallen on the material. 

DOWNLOAD OUR HDI DESIGN GUIDE:

HDI Design Guide

Creepage distance and CTI value

Depending upon the CTI value of the PCB base material, the creepage value will differ. If the CTI value is higher, then the minimum creepage value is required. In short, a high CTI value indicates a smaller distance between the PCB conductors.

Calculating PCB creepage and clearance

The measurement of clearance depends on factors such as the applied voltage, air pollution, and temperature variations. Additionally, humidity decides the breakdown voltage of air and affects the likelihood of arcing. On the other hand, along with board material and environment conditions, moisture, and contamination due to particulate accumulation shorten the creepage distance.

PCB creepage and line spacing affected by breakdown voltage

Humidity results in breakdown voltage, leading to arcing.

Designers are unable to solve issues related to clearance at PCB layout design stage since the measured distance is along the air pathway (line of sight). Component placement will likely reduce errors occurring during spacing. However, key factors, such as the usage of insulating materials and the adoption of double-sided assembly, play a critical role while determining PCB component spacing requirements.

Insulating materials acts as a sheet barrier between the high-voltage nodes. They also sleeve or cover overexposed high-voltage leads. There is a high proportion of PCB components belonging to the surface-mounted category, allowing designers to place circuits as per the requirement of clearance on opposite sides of the board. It is also important to maintain clearance from the bounding surface and through-hole connection points present on the board. Nodes within the same high-voltage circuits at the same potential do not require increased clearance or creepage. However, low-voltage circuits have to meet clearance requirements in relation to high-voltage circuits.

Few international standards have suggested the use of conformal coating for limiting issues related to the clearance. The conformal coating is applied as per the design requirement. Minimum creepage distance can solve tracking failures. Avoiding the conductive path along the insulator surface limits tracking failures. Several factors affecting creepage and clearance include:

  • Working voltage
  • Pollution degree
  • Insulation
  • Type of circuit

Working voltages for PCB creepage and clearance

A working voltage is the highest voltage across any particular insulation when the equipment is subjected to a rated voltage. This definition is stated in various international standards, including IEC 950 and EN 60950. The creepage and clearance values are calculated by determining the working voltage under a certain operating voltage. While determining working voltages, we need to evaluate both peak and root-mean-square (RMS) voltages. The peak value of the DC voltage will determine the clearance, and the RMS value of the AC voltage will determine the creepage distance.

Based on the working voltage, we calculate the minimum PCB line spacing. For instance, the working voltage of the 609V secondary circuit will withstand the peak voltage of 2700V as per IEC-60950-1, so the root-mean-square (RMS) voltage will be 2700V*√2= 3818V. As per UL 796, the 40V/mil criterion is applied to calculate the required minimum distance. So, the spacing between the two traces would be 3818/40=95.45 mils.

Working voltages for PCB creepage and clearance

Peak-to-peak voltage variations based on working voltages.

The above table shows how peak-to-peak voltage values vary with working voltages as per IEC-60950-1.

Pollution degree for PCB creepage and clearance

Pollution degree considers how pollutants will affect products exposed to different environments from a high-voltage/safety standpoint. It is a classification as per the amount of dry pollution and condensation present in the surroundings. The higher the pollution degree, the more the dust contamination and condensation, thus affecting the safety of the product. The creepage and clearance distances are adjusted to ensure the safety of a PCB. The pollution degree varies as per the contamination level and humidity level in the atmosphere.

For instance, laboratory areas come under pollution degree 2 as per several safety standards and certification bodies. Pollution degree 1 can be applied to the products that are sealed inside air and watertight enclosures. On the other hand, pollution degree 3 is applicable to harsh environmental conditions such as industrial manufacturing.

According to the IEC 60947-1 standard, the pollution degree is divided into four major categories:

  1. Pollution degree 1: Zero pollution or dry environment. In this type, there is non-conductive pollution, which is not harmful to electronic circuit operations. Examples can be sealed enclosures or potted products.
  2. Pollution degree 2: Mostly, there is non-conductive pollution. However, there is a possibility of temporary conductive pollution, which is caused due to the condensation. Laboratory area is one of the examples of pollution degree 2.
  3. Pollution degree 3: In this type, conductive pollution or contamination occurs due to humidity or dust in the surroundings. For example, heavy industrial environments are more exposed to dust.
  4. Pollution degree 4: There is a persistent conductivity, which is caused by the excess of humidity and dust contamination. External conditions, such as rain or snowfall, can lead to pollution degree 4 and result in persistent conductivity.

Controlling pollution degrees with design features

Several steps are taken to avoid the effect of pollution degree on creepage and clearance. These steps are taken according to the design features related to the PCB line spacing and the operating characteristics of the system. For instance:

  • Pollution degree 1 can be avoided by hermetic sealing of the product.
  • Pollution degree 2 is avoided by limiting the accumulation of humidity or dust particles via ventilation. 

Also, heaters and fans will avoid contamination. The continuous energizing or application of heat is highly preferred for cases in which equipment is operated without interruption. Continuous energizing also avoids the excess of cooling, so the condensation won’t occur. Furthermore, pollution degree 3 is avoided with the use of the appropriate enclosures. These enclosures limit external environmental factors such as moisture.

Insulation for PCB creepage and clearance

Typically, a single level of insulation is preferred for the electronic circuits that are not accessible. However, we prefer the use of double level insulation for protection against hazardous voltage. Several rules must be followed to implement a double-level insulation system.

The insulation barriers are necessary for circuits that fall under Safety Extra-Low Voltage (SELV) standards. The user-touchable voltage or SELV systems are termed as an electrical system in which the voltage cannot exceed a permissible value under normal conditions as per IEC and EN 60335 standards. These SELV voltages must be non-hazardous. These SELV circuits operate at low power and logic levels, such as ±3.3 to ±24VDC. Some of the examples of SELV circuits include input/output connectors and cables attached to peripheral devices such as printers and keyboards.

Classification of insulation types

Insulation types are majorly categorized into five different types, which are functional (F), basic (B), double (D), supplementary (S), and reinforced (R). Definitions for these insulation types are mentioned in multiple standards and are quite complex. It is important for designers to know all these rules and apply them in the design as per the requirement.

It is highly critical to insulate hazardous voltages from safety extra-low voltage (SELV) circuits. Following insulation types are defined as per international standards:

  1. Functional insulation: This type of insulation ensures the proper functionality of the product, but it does not guarantee safety protection.
  2. Basic insulation: This provides a single layer of insulation to avoid any harm to the electronic component.
  3. Supplementary insulation: This type of insulation adds an extra layer of protection (minimum thickness of 0.4mm) to the basic insulation to protect it from condensation.
  4. Double insulation: This is a combination of functional, basic, and supplementary insulation.
  5. Reinforced insulation: This comes under a single system that provides the same protection as double insulation. It also requires a minimum thickness of 0.4mm for use in a single layer (according to UL60950/EN60950).

These safety standards help designers to protect the electronic circuit from an abnormal (single-fault) condition. Single-fault conditions are avoided by implementing double or reinforced insulation, where a second layer remains for protection.

DOWNLOAD OUR IPC CLASS 3 DESIGN GUIDE:

IPC Class 3 Design Guide

Conductive Anodic Filament (CAF) failure

Conductive Anodic Filament is the metal filament, caused due to the electromigration of copper in a printed circuit board. This further leads to device failure. The growth of CAF bridges two oppositely polarised copper conductors. CAF occurs in four different ways: through-hole to through-hole, line-to-line, through-hole to the line, and layer-to-layer. CAF majorly takes place due to two key factors, a test or bias voltage (voltage applied during the testing of the device) and high relative humidity. CAF failure particularly occurs in the hole to hole as showcased in the diagram below.

CAF due to electromigration of copper in a PCB

High-density PCBs are prone to CAF failure, leading to reduced PCB line spacing.

The key factors influencing CAF growth include electric field strength, temperature rise, humidity, and the laminate type. CAF failure primarily arises in high-density circuit boards, leading to reduced PCB line spacing. Nevertheless, manufacturing defects can also lead to CAF failure. 

The growth of the metal filament is typically from a copper anode to a copper cathode, which ultimately leads to the electrical failure of the electronic circuit. CAF occurs in two stages: the degradation of the resin glass interface, and an electrochemical migration of copper, causing the filament growth.

The degradation of the resin glass interface is a reversible process where the material’s insulation resistance is returned after baking and drying processes. The second step of actual CAF growth is believed to be irreversible. The time required for CAF failure to occur is dependent on test voltage, relative humidity, spacing, temperature rise, and the resin system.

The degradation of the resin glass interface takes place as the PCB behaves like a cell, with the occurrence of the following reaction:

At the anode:

Cu -> Cu(n+) + ne(-)

H2O-> ½ O2 + 2 H+2e(+)

At the cathode:

H2O+ e- -> ½ H2 +2 OH(+)

Type of circuit for PCB creepage and clearance

In order to define circuit type, it is essential to identify each circuit block according to SELV (non-hazardous circuits are classified as SELV), ELV, hazardous, etc. This information can be used to define the appropriate insulation type and number of levels for use between circuit blocks and between internal components, and the user.

The following categories are used to define different circuit types along with the type of insulation required:

  1. Class 0 circuit: Appliances with class 0 circuit have no protective-earth connection. They feature a single level of insulation. Such appliances are intended for use in dry areas and a single fault could cause an electric shock. These appliances have been banned in most EU countries.
  2. Class 01 equipment: They are similar to Class 0, but have an earth terminal which is unused since two core cables are used.
  3. Class I equipment: They use protective earthing (e.g., grounded metal enclosure) as one level of insulation thus, require only basic insulation between the enclosure and any part of hazardous voltage.
  4. Class II equipment: They use double or reinforced insulation to eliminate the need for a grounded metal enclosure as well as a grounded power plug.
  5. Class III equipment: Powered from SELV source and with no potential for generation of hazardous voltages internally, and therefore only require functional insulation.

PCB component spacing

In some cases, electrical safety and voltage isolation are given high priority, creepage, and clearance, and isolation distances matter significantly. The terminal, connector, and PCB component spacing are well-defined in several international standards. However, we will be dividing spacing into two parts, such as:

  • Spacing between the uninsulated live parts and other uninsulated metal parts. It includes spacing between terminals and heatsink, chassis, metal boxes, cabinets, etc.
  • Spacing between the uninsulated live parts with opposite polarity. It includes the terminal, connector, bare wire, adjacent component spacing, etc.

High-temperature silicone potting on the device terminals allows an increase in creepage distance and enhances the pollution degree. It avoids any formation of cavities and voids during the deposition process to prevent isolation problems. This measure also improves electrical safety by increasing the “spacings” of the terminations.

Webinar SnapEDA by Sierra Circuits banner

Design guidelines for PCB creepage and clearance issues

Lower clearance leads to over-voltage, resulting in instantaneous fault between neighboring conductive traces. Adopt the following measures to resolve clearance and creepage issues:

  1. Creepage errors can be avoided by moving tracks and increasing the surface distance in your design.
  2. Have sufficient spacing between high voltage and low voltage circuits as per standard.
  3. Bend the traces using curves rather than any angle.
  4. The oblong pad can improve the spacing distance between pins.
  5. Select board material with high dielectric high CTI that are best equipped to handle high voltages to resist board insulation breakdown.  Have a discussion on material with the contract manufacturer.
  6. Interact with UL engineer while the board is in placement and routing phases, in case your board will undergo UL certification.
  7. Apply conformal coating to protect your board from external contamination; however, its composition is dielectric which adds insulation to your PCBA surface.
  8. Designers can also add a slot between traces or place vertical barriers of insulation. Incorporating a V-groove, parallel-sided notch, or placing a slot in your design can effectively solve your creepage issues.

We know that creepage is the space between PCB conductors along its surface. We need to maintain both a minimum creepage distance and packing density at the same time. Let us discuss some of the techniques that will help in higher packing density while maintaining the desired creepage distance.

Methods for solving PCB creepage issue

Use V-groove, notch, and slot techniques for creepage issues in a PCB.

  • Default situation of a flat insulating surface: In this method, the creepage is measured along the PCB surface between two conductors. You can increase the creepage distance by increasing the distances between the traces.
  • V-groove method: In this scenario, V-groove increases the surface distance between the conductors. The increased surface length is measured down to the groove till the point it reaches at least 1mm or more.
  • Parallel-sided notch approach: It further increases the surface distance but should be at least 1mm or more in width.
  • Slot implementation: The creepage distance can be further increased by implementing a slot of over 1mm in width. It is one of the easiest and cost-effective methods. This method has one limitation, it requires free space that is why it cannot be applied all the time.

PCB materials for high-voltage design

When designing a PCB for high voltage, designers need to carefully decide on PCB material as the board is exposed to regular environments and overvoltage events as it ages. Secondly, follow the safety standard while selecting PCB material and components too. In general, strictly follow the compliance required for the board.

Designers need to keep the following points in mind.

  1. Components: Select components that are exposed to high voltage as per the compliance. Make sure sufficient spacing is maintained between the terminals. Follow the layout guidelines mentioned in the component datasheet.
  2. Board material: Select PCB laminates with very high dielectric breakdown. High-voltage laminates have very high performance and high prices too. 
  3. Copper: The copper used to create PCB traces and vias should have a thickness (measured in ounces (Oz)) to withstand high currents and mechanical stress. 
  4. Resin and glass: The resin and glass levels on board influences its durability in high-voltage situations. A board with high resin content and a small glass style offers the best dielectric properties.

Check the below table for the creepage spacing requirement (in mm) for working voltage with pollution degree and material group. All measurements should be accurate and must consider the end application.

Insulation and material for creepage and clearance

Creepage requirement for working voltage with pollution degree and material group. Table credit: Calculating creepage and clearance early avoids design problems later by Homi Ahmadi.

HDI PCB material selector by Sierra Circuits

PCB creepage and clearance standards

When a designer is working on a high-voltage board design, it is mandatory to have knowledge of safety standards when dealing with power semiconductors and boards with working voltage >30Vrms/60Vdc. A proper spacing parameter such as clearance and creepage is very critical to avoid any flashover and protect the product and user. Safety standards and testing agencies prescribe the right spacing between the conductor traces based on the product requirements, usage, type of voltages, pollution degree, coating, insulation, and altitude. Since the consequences of incorrect spacing vary from legal non-compliance to serious injury and destruction of important equipment, it’s well worth the time to become acquainted with standards that are relevant to your design

The following standards can be applied:

  • IPC-2221 Generic Standard on Printed Board Design

IPC-2221 is the generic standard for guidance on PCB creepage and clearance. This standard explains in detail the requirements on material quality, traceability, layout guidelines to ensure quality. If you are following the IPC-2221A rule set, then it can be assumed that adequate isolation has been provided. A high-voltage clearance calculator based on IPC-2221 is very helpful in determining the minimum spacing for your PCB. 

For IPC 2221 standard, calculators are also available for creepage and clearance measurements.

  • IEC-60950-1 (2nd edition)

IEC-60950 is another important standard that describes spacing in IT & Telecommunication products with AC main or battery power supply, especially if you want to sell those products internationally. This standard provides safeguard values in terms of pollution degrees, insulation types, and isolation dis­tances.

  • UL61010-1: Electrical Equipment for Laboratory Use
Creepage and clearance standards

Standards for electrical safety and isolation in high-voltage applications. Table credit: Infineon application note AN 2012-10 V1.0 October 2012

Calculation and measurement of creepage and clearance distances are among the most important parts of all safety standards, and therefore it is important for design engineers to consult the product safety engineers throughout the design stages to avoid any failure at the test house before a product is launched into the market. Creepage and clearance distance not only apply to the PCB but also to the components (especially magnetic components) that are mounted on the PCB. It is also important to note that as working voltage, pollution degree, overvoltage category, and altitude increase, both the creepage and clearance distances also increase.

DOWNLOAD OUR DFM HANDBOOK:

DFM Handbook

0 Comments

Submit a Comment

Your email address will not be published.