+91 8866188126 [email protected]

Power PCB guide

Heavy copper PCBs for high current: copper weight, trace width and heat

Motor drivers, battery packs, chargers, LED drivers and power supplies push amps, not milliamps, through their copper. This guide explains what copper weight really means, how to size traces for current and temperature rise, what changes when you go to heavier copper, and which copper weights you can order online at Microplacer.

Get an instant quote

What copper weight (oz) means in thickness terms

PCB copper is specified by weight: the number of ounces of copper spread evenly over one square foot. Because the area is fixed, weight translates directly into thickness. 1 oz per square foot works out to roughly 35 µm (about 1.4 mil).

Copper weightApprox. thicknessWhere it is typically used
0.5 oz≈ 17–18 µmInner signal layers and fine-pitch routing where narrow traces must be etched accurately
1 oz≈ 35 µmThe everyday standard for outer layers on most electronics
2 oz≈ 70 µmPower rails of a few amps, motor and LED drivers, better heat spreading
2.5 oz≈ 87 µmHigher-current outer layers on simple power boards
3.5 oz≈ 122 µmBattery, charger and high-current distribution boards
4.5 oz≈ 157 µmBusbar-like conductors on the board, very high current paths

These are nominal values. On outer layers the finished thickness also includes the copper plated onto the surface while the holes are plated, so finished outer copper is usually a little thicker than the starting foil, and the exact figure varies between builds. The industry generally calls boards with about 3 oz or more on a layer “heavy copper”.

Why thickness matters

A trace’s resistance — and therefore the heat it makes — depends on its cross-section: width × thickness. Doubling copper weight roughly doubles the cross-section, so a 2 oz trace can be about half the width of a 1 oz trace for the same resistance and similar temperature rise.

How current, temperature rise and trace width relate

A trace does not have a fixed “maximum current”. Current heats it (I²R loss), and the right width is the one that keeps the temperature rise within a limit you choose — commonly 10 °C for a conservative design, 20–30 °C where space is tight and the parts and laminate tolerate it.

Current

Heat grows with the square of current: twice the current makes about four times the heat in the same trace.

Cross-section

Width × copper thickness. More area means lower resistance and less heat, so you can widen the trace or use heavier copper.

Allowed temperature rise

Choose it from the hottest acceptable trace temperature minus the worst-case ambient inside your enclosure. Keep the total comfortably below the laminate’s rated operating temperature and its TG.

IPC-2152 is the current IPC reference for sizing conductors for current. It is based on measured data and takes into account things the older charts ignored, such as board thickness and nearby copper planes that pull heat away. Its predecessor, the chart in IPC-2221, is still widely used as a quick, conservative estimate. The table below uses that classic formula for an outer-layer trace with a 10 °C rise — treat it as a starting point, then check your final widths with an IPC-2152-based calculator.

Current1 oz outer trace2 oz outer trace3.5 oz outer trace
1 A≈ 0.3 mm≈ 0.15 mm≈ 0.1 mm (often limited by the minimum width heavy copper can be etched to)
2 A≈ 0.8 mm≈ 0.4 mm≈ 0.2 mm
3 A≈ 1.4 mm≈ 0.7 mm≈ 0.4 mm
5 A≈ 2.8 mm≈ 1.4 mm≈ 0.8 mm
10 A≈ 7.2 mm≈ 3.6 mm≈ 2.1 mm

General guidance only, rounded, for a single isolated trace in still air. Real boards often run cooler (planes and pours spread heat) or hotter (enclosed boxes, neighbouring hot parts, many loaded traces side by side). Always allow margin for peak and inrush current, not just the average.

  1. 1

    Find the worst-case continuous current

    Use the real RMS current of each net, including the highest load, lowest input voltage (for converters) and any long-duration peaks.
  2. 2

    Pick an allowed temperature rise

    Start from the maximum ambient inside your enclosure and the hottest temperature the board and nearby components may reach. 10 °C is a common, comfortable choice.
  3. 3

    Choose the copper weight

    Decide this before routing. If the required widths at 1 oz will not fit, move the power layer to 2 oz or heavier instead of squeezing traces.
  4. 4

    Calculate the width and check voltage drop

    Wide traces can still drop noticeable voltage over a long run. Check the IR drop against the tolerance of the load, especially on low-voltage rails.

    Tip: Copper resistance rises with temperature — roughly 0.4% per °C — so hot traces drop more voltage than a room-temperature calculation shows.

  5. 5

    Review the hot spots

    Necks where a wide trace squeezes between pads, thin connections into a connector pin and single vias are where heat concentrates. Fix those first.

Outer vs inner layers: why inner traces carry less current for the same width

An outer trace can lose heat straight into the air (and through the solder mask). An inner trace is buried in glass-epoxy, which conducts heat poorly, so it must push its heat through the laminate before it can escape.

Outer layerInner layer
How heat escapesConvection and radiation from the surface, plus conduction into the boardOnly by conduction through dielectric to the surface or to nearby planes
Classic IPC-2221 viewBaselineAbout half the current for the same cross-section — inner traces needed roughly 2.6× the cross-section for the same current
IPC-2152 viewDepends on board thickness and nearby planesOften closer to outer-layer performance than the old chart suggests, especially next to a solid copper plane
Practical ruleUse the outer-layer numbersSize conservatively (wider) unless you have done an IPC-2152-based calculation for your stack-up

Inner copper on a multilayer board is usually thinner than outer copper, which makes the difference larger. A good layout puts the heaviest currents on outer layers, or on an inner plane with a large area, and uses inner layers for wide pours rather than narrow power traces. How layers are arranged is covered in the stack-up and impedance guide.

Copper weights our online calculator offers

These are the copper choices our online calculator offers for instant pricing. Choose the weight in the “High-spec options” section of the quote form.

Board typeOuter copper (oz)Inner copper (oz)
Rigid FR-4, 1 layer1, 2—
Rigid FR-4, 2 layers1, 2, 2.5, 3.5, 4.5—
Rigid FR-4, 4 to 16 layers1, 20.5, 1, 2
Flexible, 1–2 layers⅓, ½ or 1 — set by the flex thickness you choose—

Instant online price

FR-4 and flex PCBs up to 16 layers with the copper weights above get an instant price that includes GST and shipping. The minimum order is 5 PCBs.

Quoted by our team

Heavier copper on multilayer boards, more than 4.5 oz, metal-core boards for power and LEDs (aluminium or copper core), and anything outside the table — send your files and our team will quote it. Ask through the contact page.

Copper weight interacts with other options, such as board thickness and impedance. See the full list of choices on the PCB capabilities page and in the materials and thickness guide.

How heavy copper changes minimum trace and space and the etching process

Copper is removed by chemical etching. The etchant works downward through the copper, but it also eats sideways under the edge of the etch resist (undercut). The thicker the copper, the longer the etch, and the more sideways loss.

Trapezoid, not rectangle

A heavy-copper trace comes out wider at the base than at the top. Fabricators add “etch compensation” to the artwork so the finished width matches your design.

Wider gaps are needed

Narrow gaps cannot be cleared through thick copper, so minimum spacing grows with copper weight — often a little more than the minimum width.

Finer features suffer first

Fine-pitch pads, thin traces between pads and small annular rings are the first to be affected. Keep signal routing on lighter copper where possible.
Copper weightTypical industry minimum trace / space (general guidance)Design advice
1 ozAround 0.1–0.15 mmComfortable for most mixed signal and power designs
2 ozAround 0.15–0.2 mmGive fine-pitch ICs extra room; keep signal traces short and simple
3–4.5 ozAround 0.25–0.4 mm and upUse generous gaps; avoid fine-pitch parts on the heavy-copper layer if you can

These ranges are common across the industry, not Microplacer limits. Our engineers check every file before production and contact you if a gap or trace is too tight for the copper weight you chose. General width, spacing and clearance rules are in the PCB design rules guide.

Thick copper also needs more resin and mask

Deep gaps between heavy inner traces must be filled by prepreg resin during lamination, and solder mask must cover tall copper edges on the outside. Very dense heavy copper can cause thin mask on trace edges or resin-starved areas, so leave space and avoid isolated thin slivers of copper.

Carrying current between layers: via arrays

A via is a short copper tube. Its current capacity depends on the plated wall thickness and the hole diameter, not on the copper weight of the layers it connects — so a single via is often the weakest link in a heavy-copper path.

Via drillRough continuous current per via (general guidance)Notes
0.3 mmOn the order of 1 APlated wall is typically about 20–25 µm thick, much thinner than heavy outer copper
0.5 mmOn the order of 1.5–2 ALarger circumference gives more wall copper
1.0 mmOn the order of 3 AUseful for power transfer; check pad size and spacing

Rough estimates for a modest temperature rise. Vias are short and connect to large copper areas that draw heat away, so they often run cooler than a trace of the same cross-section — but plating thickness varies, so design with margin.

  1. 1

    Divide the current

    Estimate the current per via, then use enough vias in parallel to stay comfortably below it — for example, at least 5–6 small vias for a 5 A path.
  2. 2

    Spread them across the path

    Place vias across the full width of the trace or pour, not in a single line at one edge, so the current shares evenly.
  3. 3

    Keep them near the load

    Put the via array close to where current enters or leaves the layer to keep the path short.
  4. 4

    Watch thermal reliefs

    Solid via connections into planes carry the most current; thermal spokes reduce it. Use solid connections for power vias that are not soldered.

    Tip: Vias in pads and under parts may need plugging or filling — see the vias guide.

Via types, plugging and filling options are explained in the vias and special holes guide.

Power-board layout tips

Copper weight is only half the job. Layout decides whether the current actually flows where you planned.

Use pours, not traces

For currents of several amps, a polygon pour from source to load usually beats a trace: it is wider, spreads heat and lowers inductance.

Short and direct

Every extra centimetre adds resistance and voltage drop. Place the power stage, input and output connectors close together.

Mind the bottlenecks

A wide pour that narrows to a thin neck between two pads is only as good as the neck. Check every point along the path.

Connector pins and pads

Check the connector’s current rating per pin, split high currents across several pins, and connect each pin with a wide copper area and several vias.

Use both sides

On a 2-layer board, run the same power net on top and bottom and stitch them with via arrays to almost double the cross-section.

Separate power and signal

Keep high-current switching loops small and away from sensitive analog and feedback traces. Give the return current its own wide path.

Spread the heat

Large copper areas under hot parts, thermal vias to an inner or bottom plane and space for airflow keep temperatures down.

Respect voltage spacing

High-current boards are often high-voltage boards too. Creepage and clearance depend on voltage, pollution degree and the product standard — IPC-2221 gives general tables.

Think about assembly

Heavy copper soaks up heat during soldering. Use thermal reliefs on soldered pads connected to big pours. See design for assembly.

Cost and lead-time impact of heavier copper

Heavier copper costs more for clear reasons: more copper material, longer plating and etching, more careful lamination and more inspection.

FactorWhat changes with heavier copper
MaterialThicker foil and laminate with heavy copper cost more than standard 1 oz material.
Process timeEtching, plating and lamination cycles take longer, and some steps may be repeated.
YieldTighter features on thick copper are harder to build, so design margin directly helps price.
Lead timeHeavier copper can add production steps and time; if your schedule is tight, ask our team before ordering.

The cheapest way to carry current is often a smart layout on standard copper — wider pours, both layers in parallel, shorter paths. Move to heavier copper when the space is truly limited. Our calculator updates the price instantly when you change copper weight, so you can compare options before you order. More on what drives price in PCB cost factors.

What to specify when ordering heavy copper

A clear order avoids questions and delays. Include the following in your files or in the note field of the order form.

ItemWhat to tell us
Copper weight per layerOuter and inner copper weight, matching the values used in your design rules and calculations.
Finished thickness requirementSay whether your oz value is the starting foil or the finished copper you need, if it matters for your design.
High-current netsWhich nets carry high current and the expected current, so our engineers can pay attention to them.
Board thickness and layer countThe same values as in your Gerber files and stack-up.
Voltage and spacing needsAny working voltage, creepage or clearance requirement from your product standard.
Assembly needsIf we also assemble the board, mention heavy-copper pads on large pours and any press-fit or high-current connectors.

How to package Gerbers, drill files, readmes and notes is explained in Preparing your design files.

How ordering works at Microplacer

Pick your copper weight in the calculator and pay at order time by online payment or bank transfer. Our engineers check your files before production and read the production notes inside your files, comparing them with the options you selected. Every board gets a 100% flying-probe electrical test free of charge, and bare PCBs typically arrive in 10–15 working days, including express shipping within India.

Heavy copper FAQ

No. 2 oz carries more current and spreads heat better, but it needs wider gaps, makes fine-pitch routing harder and costs more. Use it when your current needs it, not by default.

Yes, on rigid 2-layer FR-4 boards our online calculator offers outer copper up to 4.5 oz. For multilayer boards the calculator offers 1 or 2 oz outer and 0.5, 1 or 2 oz inner copper; send your files for anything heavier.

As a rough starting point with the classic IPC-2221 formula and a 10 °C rise, an outer 1 oz trace needs roughly 2.8 mm, or about 1.4 mm at 2 oz. Confirm with an IPC-2152-based calculator for your board, and use pours where possible.

Yes. Thicker copper lowers impedance slightly for the same trace width. If you have controlled-impedance lines, decide copper weight first — see the stack-up and impedance guide.

Not always. Many designs work with 1 oz or 2 oz copper and good layout. For very high heat, a metal-core board (aluminium or copper core) may suit better — those are quoted by our team.

Usually yes. Large copper areas need more heat during soldering, so thermal reliefs and good pad design help, and our engineers review the files before assembly. See our PCB assembly page.

Yes. Every board gets a 100% flying-probe electrical test for opens and shorts at no extra cost.

Related guides

Still have a question?

Send us your files or call us — our engineers will help you choose the right options for your boards and assembly.

Streamline your innovation with seamless PCB ordering.

For More Details Contact Us