Skip to main content

Applying IPC-2221 Standards in Circuit Board Design

IPC-2221 is a generic standard for circuit board design. It lays down the requirements for PCB design and different forms of component mounting/interconnection structures. Thus IPC-2221 becomes the basis on which the design principles and recommendations for boards are established.

Author headshot: The Sierra Circuits Team

By The Sierra Circuits Team

July 20, 2021  |  0 Comments

IPC-2221 is a generic standard for circuit board design. It lays down the requirements for PCB design and different forms of component mounting/interconnection structures. Thus IPC-2221 becomes the basis on which the design principles and recommendations for boards are established. Let us see in detail about this particular standard and the design requirements it imposes.

What are IPC standards?

IPC standards are established for the electronic manufacturing industry and are issued by a trade association named IPC. At the time of its foundation, IPC stood for the institute of printed circuits, but later it was changed to the institute for interconnecting and packaging electronic circuits. Although after 1999, it has been declared just as IPC without any specific expansion.

IPC standards lay the foundation for the design, assembly, packaging, interconnection, material, performance, and inspection specifications for the electronic industry. These standards are followed throughout the world.

What is the IPC-2221 standard?

IPC-2221 establishes the generic standards for the printed circuit board design, component mounting, and interconnections. This standard belongs to the family of documents under IPC-2220. As per IPC, a document set is identified with a four-digit number ending with zero. The hierarchy of the 2220 series is given below.

Hierarchy of IPC-2220 series
Hierarchy of IPC-2220 series

From the above hierarchy, we can understand that for each type of board, there are specific standards. For example, to design rigid PCBs, standards mentioned in IPC-2221 should be referred alongside the ones laid out in IPC-2222. Similarly, this applies to flex, multichip module (MCM-L), and high-density interconnect (HDI). Therefore, it is important that all the generic standards established by IPC-2221 be used in conjunction with the detailed requirements of the standards specific to the type of circuit board.

A PCB designer should primarily focus on balancing the required electrical, mechanical, and thermal performances. In addition to that, the board’s reliability, manufacturing difficulties, and cost should be monitored. IPC-2221 focuses on all these aspects.

The IPC-2221 standard covers a vast number of topics related to board design. In this article, we will focus on some of the important ones such as clearance, creepage, insulation requirements, and high-voltage design requirements.

What is clearance in board design?

Trace clearance as per IPC-2221
Clearance in PCB design

The distance between two conductors or nodes, measured in air, is referred to as clearance distance. IPC-2221 refers to so many different clearances related to different aspects of the circuit board. Let us have a look at a few of the important ones mentioned in this standard.

Component leads0.13mm (up to a voltage of 50V)
Uncoated conducting areas (washers or similar mechanical hardware)0.75mm
Test probe sites80% of the component height (0.6mm minimum and 5mm maximum)
Mounting hardwareShould not protrude more than 6.4mm below PCB surface
PTH relief in the heat sink2.5mm larger than the hole (includes electrical clearance and misregistration tolerance)

For solder masks, the IPC-2221 mask clearance and dams are given below.

Mask typeClearanceDam
Liquid screenable0.25mm0.25mm
Photoimageable dry film ≤0.0635mm0.051mm0.127mm
Photoimageable dry film 0.066 to 0.1mm0.051mm0.25mm

What is creepage in PCB?

Creepage as per IPC-2221
Creepage in PCB design

Creepage and clearance are two parameters that are related to the distance required between conductors on a circuit board. As discussed above, clearance refers to the distance between two conductors or nodes in the air. Creepage, on the other hand, refers to the distance between conductors or nodes along the surface of an insulator.

As per IPC-2221, space between the conductors should always be maximized and optimized to the possible extent. Conductor spacing will be allotted in such a manner that there is enough space for the etch compensation of the other physical features. This etch compensation should be twice the etched copper thickness. Apart from the etch compensation, it should also consider conductor imperfections and also copper wicking between PTHs and adjacent plane layers.

How thick should traces be?

IPC-2221 standards for trace thickness
PCB trace thickness

For carrying a specific amount of current, a PCB trace should have an appropriate thickness. If it is less than what is required, the trace will burn while the current propagates through it. Thus, the thickness and width of the traces will depend on the signal characteristics, current carrying capacity, and the maximum allowable temperature. This is determined by referring to IPC-2141 and IPC-4562 as well.

The thickness of the traces will also change according to the construction requirements of the board. If the circuit board construction involves sequential lamination, blind or buried vias, then the thickness of copper on the layers will depend on these parameters as well.

Trace Width Calculator

To calculate the trace width for allowable current, the following formula can be used:

Width [mils]=Area [mils2] / (Thickness [oz] x 1.378 [mils/oz])

The cross-sectional area, A is calculated by:

A = ( I / [k x (ΔT0.44)](1/0.725)

Where, I is the maximum current in Amps, k is a constant, ΔT is the temperature rise above ambient in °C, and A is the cross-sectional area of trace in mils².

For internal layers,

  • k = 0.024
  • Conductor thickness = copper foil thickness of the base laminate.
  • If blind and buried vias are implemented, then, conductor thickness = copper foil thickness that includes the copper plating.

For external layers,

  • k = 0.048
  • Conductor thickness = thickness of the base foil and the plated copper of PTH without including the thickness of the solder coating, tin-lead plating, or secondary platings.


IPC-2221 insulation resistance test recommendations

Insulation is a basic requirement in a PCB for protection against short circuits between conductors by accidental contact, overheating caused by electric conduction, and corrosion or other environmental damages. A lot of materials can be used to insulate a circuit board. The choice of the material, however, depends on the board application.

HDI PCB material selector by Sierra Circuits

IPC-2221 suggests some insulation resistance tests and individual test coupons as follows.

Also read, how to work around black pad in ENIG finish.

Insulation tests

  1. Insulation resistance test: In this test, a voltage is applied across the PCB which induces current flow. This current is measured to calculate the quantifiable resistance value for the whole of the product’s insulation.
  2. HiPot testing: This test is used to check whether the insulation provided is enough to protect the circuit board or not. For this test, a high voltage is applied to the PCB and the resulting current flow through the insulation is measured. This current is called the leakage current and it is measured using the HiPot tester. If the high voltage does not break down the insulation, then the insulation will be good enough to protect the board. This test is also known as the dielectric withstanding voltage (DWV) test and is usually carried out after conducting the dielectric breakdown test.

Insulation resistance test coupons

  1. Moisture and insulation resistance coupons: These test coupons help to evaluate the insulation resistance and the bulk resistance of the circuit board. This evaluation is carried out once the board has been exposed to different humidity and temperature environments with specific voltages applied to it.
  2. E-coupon: The moisture and insulation resistance of the laminated base materials are evaluated using this coupon. A design with a maximum of 10 layers can be tested using this coupon.
  3. Legacy E coupon: This coupon has a Y pattern and is helpful in evaluating the cleanliness and insulation resistance properties.

Surface insulation resistance coupons

The surface insulation resistance test coupons include the following:

  • H coupon: This coupon is used to measure the effects of the process or residues on the surface insulation resistance.
  • Legacy H coupon: Higher level insulation testing requires the use of legacy H coupon. Examples are PCBs for telecommunication.

High voltage circuits

The clearances mentioned by IPC-2221 stands correct for normal PCBs, but when it comes to high voltage circuit boards, these values should be rechecked. When a high voltage is applied across the conductors, there are more chances of a flashover than under normal working voltages. Therefore, different standards should be considered in the case of high voltage design. There are high voltage design tools that can be used to evaluate the values of the clearances for specific voltages.

Selection of insulation materials

The materials used for insulation play a prominent role in withstanding the high potential between two conducting features. The best way to guarantee good insulation in high voltage circuits is by choosing materials with comparative tracking index (CTI) ratings that can withstand high voltages. CTI is the measure of the electrical insulation of a material by subjecting it to higher voltages and monitoring the voltage at which it breaks down.


PCB Material Design Guide - Cover Image

PCB Material Design Guide

9 Chapters - 30 Pages - 40 Minute Read
What's Inside:
  • Basic properties of the dielectric material to be considered
  • Signal loss in PCB substrates
  • Copper foil selection
  • Key considerations for choosing PCB materials



Increasing the clearance and creepage

With the increase of voltages, it is obvious that the clearance and creepage distance between traces and conducting features on the PCB should be increased. But we are working on circuit boards here, and hence there is a limit to which these distances can be increased. The minimum creepage and clearances defined by the IPC-2221 will not be enough to prevent a flashover in this case. Therefore, different methods should be adapted to increase the clearance and creepage distances.

Tips and tricks to increase the creepage distance in high voltage circuits

  • Creating slots, v-grooves, or parallel-sided notches between the conducting features increases the creepage distance.
  • SMT components are used in abundance on the board, hence the ones that require maximum clearance from each other can be placed on the opposite sides of the board.
  • Installing vertical insulator barriers in space will increase both clearance and creepage.
  • Keeping the high and low voltage nodes close to each other will increase the chances of flash-over or arcing. Placing high voltage circuits on the top side of the board and low-voltage ones on the bottom solves this issue to an extent.

IPC-2221 is a reference document that lays down a number of standards while designing a PCB. This document has had many revisions in the past years. These revised documents along with the specific standards for the type of board being designed will help to accurately determine all the design aspects.

Do let us know if there is something specific to this standard that you would like to learn about in the comments section. You can download our DFM handbook to learn how to optimize your PCB design.


Design for Manufacturing Handbook - Cover Image

Design for Manufacturing Handbook

10 Chapters - 40 Pages - 45 Minute Read
What's Inside:
  • Annular rings: avoid drill breakouts
  • Vias: optimize your design
  • Trace width and space: follow the best practices
  • Solder mask and silkscreen: get the must-knows


What is 1900 + 86?

Notify of
Inline Feedbacks
View all comments
Share this article
Zero Defects guaranteed on all PCB fabrication

Reduce Re-Spins with our Zero Defect Guarantee.

Our platform sources the whole package, creating a thread from design to delivery. Fabricating PCBs. Procuring parts. Assembling your boards.

Once you upload your BOM, Our best-in-class software automatically checks for errors and cleans your file for you. After you place an order, your dedicated CAM engineer will run a full DFM and DFA check to ensure your prototype achieves Zero Defect every time—all at no additional cost to you.

Get to market faster and spend less time troubleshooting.

Start Quote

Talk to a Sierra Circuits PCB Expert today

24 hours a day, 7 days a week.

Call us: +1 (800) 763-7503
Email us: through our Customer Care form