Vutrax PCB CAD     
OpenBroadband Download
OpenIndividual Downloads
OpenOpenTrack Width/Gaps
OpenOpenRS232 Cables
OpenMail & Contacts

Vutrax Technical Bookcase

Aspects of Track Width and Clearance

Track width and clearances for most designs is primarily a limitation of the PCB manufacturing process.

A very conservative figure for low density designs using pin-through components is 0.016" (16 THOU) tracks with minimum clearance of 0.008" (8 THOU), which allow a single track between pads (at typical 0.1" pitch) of 0.064" (64 THOU) diameter. DIY board processing may also involve larger figures, no tracks between pads, etc. to allow for the difficulties in photo transfer, etching, and accurate drilling.

Professional designs will vastly exceed these limits, frequently using track of a few THOU and similar clearance. The issue of current capacity of these tracks, and SAFE clearances for higher voltage then become major considerations.

This note is the authors interpretation of a series of sci.electronics.cad Internet newsgroup discussions, and web sites, in an attempt to generate some 'rules of thumb'. There is nothing 'official' about these notes - they are provided as-is. You are bound by whatever legislative requirements your country or countries apply.

These aspects are considered independently:-

Current Capacity of tracks

A frequently asked question is how wide should a track be to carry moderate to high currents.

Clearly there are an enormous number of variables, and if you need a truly optimal answer you need a full thermal analysis package (dig deep into your pocket!) and details of the conductivity of your board materials and coatings.

More normally a rough guide is all that is required, and that is what we provide here.

What creates the limits? Except for very high frequencies at high currents, the primary limitation is ohmic heating of the track balanced against the ability of the track to cool itself. Outer layers will cool to air (usually through a coating) while inner layers have first to pass through a substantial thickness of board substrate.

So how much heating can a track tolerate? Apart from safety aspects, the consensus seems to be that heating of a track should be limited to 10 or 20 degrees, depending on reliability requirements. Where the current is switched at a rate lower than a few times per second, go for the lower figure - repeated thermal expansion and contraction obviously fatigue the adhesives and copper more than a continuous current.

In the table the following are assumed

  • 1oz/sq foot copper (0.035mm thickness).
  • 10 degree C rise on outer layers, 20 degree C inner layers
  • Groups of high current tracks will be de-rated
  • Tracks are not near or over 'Heat Sink' areas

Imperial Width

Metric Width

Current Capacity



0.8 Amps



1.2 Amps



1.5 Amps



3.2 Amps



6.0 Amps

You can modify these figures:-

  • Each doubling of copper thickness allows an increase of sqrt(2) (about 1.4) in the current capacity, because although you halve the resistance, power increases as the square of current (W = I^2 * R) and track thickness hardly changes dissipation.
  • Each doubling of a single track width increases dissipation, but does not double it. A suggested factor is to increase current capacity by a factor of 1.65.
  • Remember to derate closely grouped high current tracks.
  • Derate or uprate according to required reliability.
  • Derate boards designed to be used at high ambient temperature.

For most purposes it will be easy to determine a practical width from the above. If you want to make more precise calculations (based, it must be noted, on empirical data) try the formula
    I = 0.048 T0.44 A0.725
Where the units are




Temperature Rise in °C


Cross sectional area in square mils (square THOU)

This formula is for outer layers, and needs to be de-rated to 50% for inner layers.
References to this formula can be found Here in the section PCB Data.


Other Reasons for Wide Tracks

Current capacity is far from the only reason to use wide tracks. The primary use is on boards not using powerplanes (i.e. typical single and double sided boards) where it is important to maintain a low impedance throughout the ground, and often also power rail interconnections.

VUTRAX provides the means to measure track resistance using [Set Resistivity] and [Length and Resistance] from the (Route) menu in appropriate modes.


Using Tracks as 'fuses'

Short form: Don't! Use proper PCB mounted fuses.

Long form: It looks very tempting to include 'unlikely to blow' fuses as very thin tracks on a PCB. All the good advice is against it:-

  • If the fuse blows it will spray copper over a large area of the board, probably writing it off. Even if not, rectification is difficult, and certainly a return to factory job.
  • Any on-site repair is likely to be a wire link- negating all protection.
  • The melting point of copper is much higher than fuse wires - the flying drops may ignite nearby materials.
  • Copper is a good conductor - the tracks required for small currents are very thin (much thinner than the widths recommended for normal use). The slightest variation in original board stock, degree of etching, and thickness of plating will all have major impact on the current limit.
  • For high currents the risk of arcing and potential fire are considerable.


Track Clearances for High voltages

For most purposes track clearances are determined by the ability of the manufacturing process to avoid inter-track shorts.

When high voltages are involved, the following UL derived rule provides the minimum clearance between tracks with designated potentials between them at normal temperature and pressures, or when coated:-

       0.023"      +  (0.0002"    *  peak volts)
       0.584mm  +  (0.005mm  *  peak volts)

For raw single phase 240V UK mains it is necessary to make generous allowance for up to (say) 2KV spikes, where these formulae give 0.423" or 10.584mm.

Mains safety is covered by a plethora of international standards and regulations. Any general list is automatically inadequate.
In EN60065:1994, 3 mm is allowed for Class I (protection by earthing) but 6 mm is required for Class II (double-isolated). Other standards require larger values, especially where insulator surfaces can become contaminated (including dirt, oils and condensation).

Good design practice in any case partitions PCB's into 'safe' and 'unsafe' areas with wide separation (possibly including a safety earth barrier), and restricting 'unsafe' tracks to one side which can then be coated to protect from contamination and prying fingers.

VUTRAX allows you to classify different signals into classes and then specify the required clearance between them. So you can classify the mains side in one class, and the low voltage in another, and Design Rule Checking will check that the clearances are whatever safe value you specify.

If you are wondering whether to compromise on mains isolation, imagine yourself permanently connected to the 'safe' side.

© 1998 Computamation Systems Ltd.