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 quoteWhere 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
Convection from the surface
The enclosure and mounting
| Material | Typical thermal conductivity (general values) | What it means in practice |
|---|---|---|
| Copper | About 380–400 W/m·K | The main heat spreader on any board. Thicker and wider copper spreads heat further. |
| FR-4 laminate | About 0.3 W/m·K through the thickness | Acts almost like an insulator. Heat crosses it mainly through plated vias. |
| Solder | About 50–60 W/m·K | Good enough for joints, but voids under exposed pads reduce heat flow. |
| Thermally conductive dielectric (metal-core boards) | Typically 1–3 W/m·K or more | A thin, better-conducting insulating layer that lets heat reach a metal base quickly. |
| Aluminium | About 130–230 W/m·K, depending on the alloy | Used as the base of metal-core boards and in heatsinks. |
The basic relation
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
Copper thickness
Inner planes work too
Keep planes continuous
| Copper option | What our online calculator offers | Thermal effect (general guidance) |
|---|---|---|
| Outer copper | 1 oz or 2 oz on most layer counts; 2-layer boards can also be ordered with 2.5, 3.5 or 4.5 oz | Thicker outer copper spreads heat from surface-mount pads and carries more current. |
| Inner copper (4+ layers) | 0.5, 1 or 2 oz | Heavier inner planes improve spreading on power and motor-drive boards. |
Trace current and temperature rise
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.
| Parameter | Common starting point (general guidance) | Why |
|---|---|---|
| Drill size | About 0.2–0.35 mm finished hole | Small enough to limit solder loss into the hole, large enough to plate reliably. |
| Pitch | About 1.0–1.2 mm grid | More vias lower thermal resistance, but packing them too tightly weakens the pad and the plane. |
| Count | As many as fit the grid inside the pad | Each 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 hole | Plated wall typically around 20–25 µm | The plated barrel, not the hole, carries the heat. Filled vias add a little more conduction. |
| Bottom-side copper | A pour the same size as the pad or larger | Gives the heat somewhere to go. Vias into a tiny island help very little. |
| Via treatment | Solder wicking during reflow | Notes |
|---|---|---|
| Untented (open) | High — solder can drain through the holes | Can leave the pad starved and create voids or solder balls on the other side. |
| Tented (covered by solder mask) | Reduced on the tented side | Common for vias next to pads. Tenting the bottom side of in-pad vias limits solder escaping. |
| Plugged | Low | The hole is closed so solder stays on the pad. |
| Epoxy filled and capped | Very low — the pad surface is flat and plated over | The usual choice for via-in-pad under fine-pitch parts and exposed pads. |
| Copper paste filled and capped | Very low | Like epoxy fill but with a more conductive fill, which helps heat flow slightly. |
Via covering in our online calculator
- 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
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
Decide how to stop solder loss
Either fill and cap the vias, or keep them small and tent them on the opposite side. - 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
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
Protect sensitive parts
Respect the airflow
Use the board edges carefully
Leave room for a heatsink
Think about vertical boards
Assembly side of placement
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 property | What it describes | Why it matters thermally |
|---|---|---|
| Tg | Temperature where the resin turns from glassy to rubbery | Keep 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 down | Relevant for lead-free reflow, which typically peaks around 240–260 °C. |
| Z-axis expansion (CTE) | How much the board grows in thickness when heated | Lower expansion means less stress on via barrels during reflow and thermal cycling. |
| Time to delamination | How long the board survives at a high fixed temperature before layers separate | Indicates margin for multiple reflow passes and rework. |
When a higher Tg helps
What our online calculator offers
Moisture and reflow
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.
| Substrate | How it moves heat | Typical uses | Trade-offs |
|---|---|---|---|
| FR-4 with heavy copper and thermal vias | Copper spreads heat, vias carry it through | Most power supplies, motor drivers, chargers | Lowest cost; limited by via count and copper area. |
| Aluminium core (insulated metal substrate) | Thin dielectric bonds the circuit to an aluminium base | LED modules, lighting, simple power stages | Usually single-sided; through-hole parts and routing are restricted. |
| Copper core | Same idea with a copper base, which conducts heat better | High-power LEDs and power electronics | Heavier and more expensive than aluminium. |
| Ceramic substrates | Ceramic conducts heat well and insulates electrically | High-temperature or high-power modules | Specialist process; brittle and costly. |
How to get a metal-core board priced
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.
| Connection | Soldering | Heat flow and current | Use it for |
|---|---|---|---|
| Thermal relief (spokes) | Easier — the pad heats up quickly | Lower, limited by spoke width and count | Through-hole pins on planes, small SMD pads on large pours, parts that may need rework |
| Solid (direct) connection | Harder — needs more heat and time | Highest | Exposed thermal pads, power device tabs, high-current pins |
Common spoke rules of thumb
Avoid the tombstone trap
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
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
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
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
Order a prototype
Order a small batch (minimum 5 PCBs) so you can test before committing to volume. See PCB prototyping. - 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
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.
| Item | Where to set it | What to check |
|---|---|---|
| Copper weight (outer and inner) | Online calculator | Matches the copper used for your trace and pour calculations. |
| Material type and TG | Online calculator | Higher TG for hot, thick or multi-reflow boards. |
| Via covering | Online calculator | Filled and capped, plugged or tented for vias inside exposed pads. |
| Which vias need filling | Drill file and a fabrication note | Mark in-pad vias clearly if only some vias should be filled. |
| Metal-core or other substrate | Choose the material and send for a quote | Our team prices it and confirms the build. |
| Stencil openings for exposed pads | Paste layer in your Gerber | Divided windows for large pads; see the assembly guides. |
How this fits ordering at Microplacer
Thermal design FAQ
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.