+91 8866188126 [email protected]

PCB design guide

PCB thermal management: thermal vias, copper and material choices

Every regulator, MOSFET, LED and processor turns part of its power into heat, and the board is usually the main path that carries it away. This guide explains how heat moves through a PCB, how copper, vias and placement help, when the laminate or a metal-core board matters, and what to specify when you order.

Get an instant quote

Where heat goes on a PCB

Heat leaves a component in three ways: conduction into the board and leads, convection into the surrounding air, and radiation. On most boards conduction through copper does the heavy lifting, because the glass-epoxy laminate itself is a poor conductor of heat.

Conduction through copper

Copper conducts heat roughly a thousand times better than FR-4. A component pad soldered to a wide copper area spreads its heat sideways, and vias carry it to other layers and the opposite side.

Convection from the surface

Once heat is spread over a larger area, the air carries it away. Still air removes heat slowly; a fan or a vented enclosure can remove several times more from the same board.

The enclosure and mounting

In a closed plastic box the air inside warms up, so the whole board runs hotter. Screws, standoffs, thermal pads or a metal case can become a second heat path.
MaterialTypical thermal conductivity (general values)What it means in practice
CopperAbout 380–400 W/m·KThe main heat spreader on any board. Thicker and wider copper spreads heat further.
FR-4 laminateAbout 0.3 W/m·K through the thicknessActs almost like an insulator. Heat crosses it mainly through plated vias.
SolderAbout 50–60 W/m·KGood enough for joints, but voids under exposed pads reduce heat flow.
Thermally conductive dielectric (metal-core boards)Typically 1–3 W/m·K or moreA thin, better-conducting insulating layer that lets heat reach a metal base quickly.
AluminiumAbout 130–230 W/m·K, depending on the alloyUsed as the base of metal-core boards and in heatsinks.

The basic relation

A component runs at roughly ambient temperature + power × thermal resistance. For a part dissipating 1 W with a total thermal resistance to air of 40 °C/W, the rise is about 40 °C. Good board design is about lowering that thermal resistance with copper, vias and airflow.

Copper planes and pours as heat spreaders

The cheapest way to cool a part is usually more copper connected to its thermal pad or hot leads. Copper area, copper thickness and connection to inner planes all add up.

Area matters most

A larger copper pour around a hot pad spreads heat over more surface. The gain is largest for the first few square centimetres and gets smaller further away, because heat has to travel through thin copper to reach the edges.

Copper thickness

Doubling the copper weight (for example 1 oz, about 35 µm, to 2 oz, about 70 µm) roughly halves the sideways thermal resistance of the copper. It also lets traces carry more current with less self-heating.

Inner planes work too

On 4-layer and larger boards, a solid ground plane connected by vias under a hot part is a very effective spreader, even though it is buried in the laminate.

Keep planes continuous

Long slots and narrow necks in a plane block heat as well as current. Avoid cutting a plane right next to a hot component.
Copper optionWhat our online calculator offersThermal effect (general guidance)
Outer copper1 oz or 2 oz on most layer counts; 2-layer boards can also be ordered with 2.5, 3.5 or 4.5 ozThicker outer copper spreads heat from surface-mount pads and carries more current.
Inner copper (4+ layers)0.5, 1 or 2 ozHeavier inner planes improve spreading on power and motor-drive boards.

Trace current and temperature rise

Trace width for a given current and allowed temperature rise is usually taken from the charts in IPC-2152, which is now generally preferred over the older IPC-2221 curves for this purpose. The older charts treated inner-layer traces as running much hotter than outer ones; the newer data shows the result depends strongly on board thickness, nearby copper planes and how the board is mounted, so treat any chart value as a starting point and leave margin. See PCB design rules for general layout limits.

Thermal vias under exposed pads

QFN, DFN, power SOIC, D-PAK and many LED packages have a large exposed pad that is the main heat path. An array of plated vias in that pad carries heat to inner planes and to copper on the other side of the board.

ParameterCommon starting point (general guidance)Why
Drill sizeAbout 0.2–0.35 mm finished holeSmall enough to limit solder loss into the hole, large enough to plate reliably.
PitchAbout 1.0–1.2 mm gridMore vias lower thermal resistance, but packing them too tightly weakens the pad and the plane.
CountAs many as fit the grid inside the padEach via conducts in parallel. One via in a 1.6 mm board is very roughly 100–200 °C/W; nine of them together are closer to 15–25 °C/W.
Copper plating in the holePlated wall typically around 20–25 µmThe plated barrel, not the hole, carries the heat. Filled vias add a little more conduction.
Bottom-side copperA pour the same size as the pad or largerGives the heat somewhere to go. Vias into a tiny island help very little.
Via treatmentSolder wicking during reflowNotes
Untented (open)High — solder can drain through the holesCan leave the pad starved and create voids or solder balls on the other side.
Tented (covered by solder mask)Reduced on the tented sideCommon for vias next to pads. Tenting the bottom side of in-pad vias limits solder escaping.
PluggedLowThe hole is closed so solder stays on the pad.
Epoxy filled and cappedVery low — the pad surface is flat and plated overThe usual choice for via-in-pad under fine-pitch parts and exposed pads.
Copper paste filled and cappedVery lowLike epoxy fill but with a more conductive fill, which helps heat flow slightly.

Via covering in our online calculator

All five options above (tented, untented, plugged, epoxy filled and capped, copper paste filled and capped) can be selected in our online calculator for FR-4 boards, and the price updates as you change them. Check the minimum via sizes and pad rules on PCB capabilities and vias and special holes.
  1. 1

    Start from the package footprint

    Use the land pattern and thermal via recommendation in the component datasheet. Footprint naming and pad sizing usually follow IPC-7351.
  2. 2

    Place a via grid in the exposed pad

    Fill the pad with a regular grid, keeping vias clear of the pad edge so the solder fillet can form.
  3. 3

    Decide how to stop solder loss

    Either fill and cap the vias, or keep them small and tent them on the opposite side.
  4. 4

    Split the paste opening

    Large exposed pads usually get a stencil opening divided into several smaller windows (often around 50–80% total coverage), so the part does not float and voids stay small.

    Tip: If vias are open, keep the paste windows between the vias rather than on top of them.

  5. 5

    Connect to real copper

    Tie the vias to a ground plane or a large pour on the other side. That is where the heat actually spreads.

Component placement and spacing

Where parts sit decides how heat flows between them. A few placement habits prevent most hot spots.

Spread the heat sources

Do not cluster regulators, power transistors and drivers in one corner. Spreading them lets each one use its own copper area.

Protect sensitive parts

Keep electrolytic capacitors, crystals, sensors and precision references away from hot parts. A common rule of thumb is that electrolytic capacitor life roughly halves for every 10 °C rise.

Respect the airflow

With a fan or vents, place hot parts where the air arrives and orient tall parts parallel to the flow so they do not shade smaller ones.

Use the board edges carefully

Parts near a metal case or a mounting screw can dump heat into it, but parts near a closed plastic wall get very little cooling.

Leave room for a heatsink

If a heatsink or thermal pad may be needed later, reserve the area and mounting holes now, and keep tall parts clear of it.

Think about vertical boards

On a board mounted upright, warm air rises along it. Put the hottest parts near the top so they do not preheat everything above them.

Assembly side of placement

Very large copper areas take longer to heat during reflow, so parts sitting on them need a good profile. Our engineers check files before production; see design for assembly for spacing and orientation habits that keep boards easy to solder.

Laminate temperature limits: Tg and multiple reflows

Tg (glass-transition temperature) is where the laminate resin softens and starts expanding much faster through its thickness. That expansion stresses plated holes and vias, which is why heat-related failures often appear in vias first.

Laminate propertyWhat it describesWhy it matters thermally
TgTemperature where the resin turns from glassy to rubberyKeep the maximum operating temperature well below it; a margin of roughly 20–25 °C or more is a common rule of thumb.
Td (decomposition)Temperature where the resin starts to lose weight and break downRelevant for lead-free reflow, which typically peaks around 240–260 °C.
Z-axis expansion (CTE)How much the board grows in thickness when heatedLower expansion means less stress on via barrels during reflow and thermal cycling.
Time to delaminationHow long the board survives at a high fixed temperature before layers separateIndicates margin for multiple reflow passes and rework.

When a higher Tg helps

Boards that run hot in service, boards that see two reflow passes plus wave or hand soldering, thick multilayer boards that take longer to heat through, and products that face many power or temperature cycles.

What our online calculator offers

TG135 as standard on 1–6 layer boards, higher-TG grades selectable from 2 layers up, TG155 or above required from 8 layers, and TG170 only on boards with 10 or more layers. The full table per layer count is in the materials and thickness guide.

Moisture and reflow

Moisture absorbed by the board or by plastic component packages turns to steam during reflow and can crack packages or delaminate the board. Moisture-sensitive components are typically classified under J-STD-020 and handled, stored and baked under J-STD-033; keep boards and parts sealed until assembly and follow the part’s moisture-sensitivity label.

Metal-core and other thermal substrates

When copper pours and vias on FR-4 are not enough, the substrate itself can do the work. Metal-core boards are quoted by our team rather than priced instantly; for other special substrates, contact us.

SubstrateHow it moves heatTypical usesTrade-offs
FR-4 with heavy copper and thermal viasCopper spreads heat, vias carry it throughMost power supplies, motor drivers, chargersLowest cost; limited by via count and copper area.
Aluminium core (insulated metal substrate)Thin dielectric bonds the circuit to an aluminium baseLED modules, lighting, simple power stagesUsually single-sided; through-hole parts and routing are restricted.
Copper coreSame idea with a copper base, which conducts heat betterHigh-power LEDs and power electronicsHeavier and more expensive than aluminium.
Ceramic substratesCeramic conducts heat well and insulates electricallyHigh-temperature or high-power modulesSpecialist process; brittle and costly.

How to get a metal-core board priced

Choose Aluminium or Copper core as the material in our online calculator and send it for a quote. Our team reviews the files and emails the quotation. Instant online prices cover FR-4 and flex boards up to 16 layers; see PCB materials for the difference between the options.

Thermal relief vs solid connections

A pad joined to a plane on all sides is great for heat flow but hard to solder, because the plane pulls heat away from the iron or the reflow oven. A thermal relief (spokes) is a compromise.

ConnectionSolderingHeat flow and currentUse it for
Thermal relief (spokes)Easier — the pad heats up quicklyLower, limited by spoke width and countThrough-hole pins on planes, small SMD pads on large pours, parts that may need rework
Solid (direct) connectionHarder — needs more heat and timeHighestExposed thermal pads, power device tabs, high-current pins

Common spoke rules of thumb

Four spokes, each a few tenths of a millimetre wide, with a small air gap around the pad. Make the spokes wider (or add more) for pins that carry current. IPC-2221 discusses thermal relief in general terms.

Avoid the tombstone trap

Small two-terminal parts with one pad on a solid plane and the other on a thin trace can heat unevenly and stand up during reflow. Give both pads similar copper, or use relief on the plane side.

Checking a design: estimating and testing

You do not need simulation software for most boards. A quick estimate during layout and a measurement on the first prototype catch most problems.

  1. 1

    List the power in each part

    Regulator loss is roughly (input − output voltage) × current for linear regulators; for switching parts use the efficiency curve. MOSFET loss is roughly current² × on-resistance plus switching losses.
  2. 2

    Estimate junction temperature

    Junction temperature ≈ ambient + power × θJA. Datasheet θJA values are measured on standard JEDEC JESD51 test boards, so your board may be better or worse; treat them as a guide.

    Tip: Use the hottest ambient the product will see, including the warm air inside the enclosure, not room temperature.

  3. 3

    Compare with the limits

    Check the part’s maximum junction temperature, any derating rule your project uses, and the laminate Tg. Leave margin for parts tolerance and dust.
  4. 4

    Order a prototype

    Order a small batch (minimum 5 PCBs) so you can test before committing to volume. See PCB prototyping.
  5. 5

    Measure under real load

    Run the board at full load in its enclosure until temperatures settle, then measure with a thermocouple taped to the part or a thermal camera. Note that shiny metal surfaces read wrongly on thermal cameras unless covered with matt tape or paint.
  6. 6

    Adjust copper, vias or airflow

    If a part is too hot, the usual fixes in order of cost are: more copper and vias, a heatsink or thermal pad to the case, airflow, and finally a different substrate.

What to specify when you order

Most thermal decisions are made in your design files, but a few options are set in our online calculator or in your notes.

ItemWhere to set itWhat to check
Copper weight (outer and inner)Online calculatorMatches the copper used for your trace and pour calculations.
Material type and TGOnline calculatorHigher TG for hot, thick or multi-reflow boards.
Via coveringOnline calculatorFilled and capped, plugged or tented for vias inside exposed pads.
Which vias need fillingDrill file and a fabrication noteMark in-pad vias clearly if only some vias should be filled.
Metal-core or other substrateChoose the material and send for a quoteOur team prices it and confirms the build.
Stencil openings for exposed padsPaste layer in your GerberDivided windows for large pads; see the assembly guides.

How this fits ordering at Microplacer

FR-4 and flex boards up to 16 layers get an instant online price that includes GST and shipping, and bare boards are typically delivered in 10–15 working days, including express shipping in India. Every board gets a free 100% flying-probe electrical test. Production notes in your files are read and compared with our options, and engineers check the files before production. For assembled boards, the instant PCBA price is calculated from solder pads; designs with BGA, LGA or 0201 parts go to engineering review. See the online ordering FAQ and PCB assembly.

Thermal design FAQ

Start with the datasheet recommendation. If there is none, a regular grid at about 1.0–1.2 mm pitch that fills the pad is a common starting point. More vias help, but only if they connect to a real copper area on another layer.

Filling and capping gives the flattest pad and stops solder draining away, which is the most predictable option. Small open vias tented on the opposite side are a lower-cost alternative that works for many parts. Both are choices in our online calculator.

It spreads heat better and carries more current, but it costs more and makes very fine traces and spaces harder to produce. Many boards use 2 oz only where the power is, or rely on inner planes on multilayer boards.

When the heat is concentrated in many small parts, such as LED arrays, and FR-4 with copper and vias cannot keep them cool, an aluminium core is often the simpler answer. Metal-core boards are quoted by our team.

No. TG does not change how well the board conducts heat. It raises the temperature the laminate can tolerate, which matters for hot environments and repeated soldering.

Open vias in a pad can pull solder away from the joint. Filling, plugging or tenting them, and splitting the paste opening, avoids most issues. Our engineers check files before production.

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