RF PCB Engineering Tools

Thermal Via Calculator | Via Array Thermal Resistance

Use this thermal via calculator to determine how many vias your thermal pad needs and what thermal resistance each via contributes, based on via diameter, plating thickness, board thickness and copper conductivity.

Thermal via array under a QFN pad on a PCB with plated copper vias

What a Thermal Via Calculator Tells You

A thermal via calculator computes the thermal resistance of a single plated via and the number of vias needed under a thermal pad to conduct a target heat flux from a component to an opposite-side heat sink or copper plane. The key inputs are via diameter, plating thickness, board thickness and copper’s thermal conductivity (roughly 385 W/m·K for electrodeposited copper). The output is a per-via thermal resistance in °C/W and a recommended via count for your power dissipation budget.

Getting this right matters because an undersized via array creates a thermal bottleneck that no amount of external heatsinking can fix, while an oversized array wastes board real estate and can compromise signal routing or structural integrity.

Thermal Resistance of a Single Via

PCB cross-section showing copper-filled thermal vias through board layers

A plated through-hole via is essentially a hollow copper cylinder. Its thermal resistance is governed by the same geometry as electrical resistance, scaled by thermal conductivity instead of electrical conductivity:

R_thermal = L / (k × A_copper)

  • L — board thickness (the via’s heat-path length), typically 1.0–2.4 mm (39–94 mil)
  • k — thermal conductivity of copper, ~385 W/m·K
  • A_copper — cross-sectional area of the copper annulus: π × (r_outer² − r_inner²), where r_inner = r_outer − plating thickness

For a common 0.3 mm (12 mil) drill with 25 µm (1 oz) plating in a 1.6 mm board, A_copper ≈ 0.0216 mm² and R_thermal ≈ roughly 193 °C/W per via. Filling the via with copper paste or solder drops this significantly because the hollow core is no longer insulating air; a fully copper-filled via of the same diameter can reach ~55 °C/W.

Use the resistance-by-geometry tool below to experiment with different plating thicknesses and drill sizes and see how the cross-sectional area changes the result:

Loading Resistance by Geometry…

After entering your copper annulus dimensions, compare the calculated resistance to the budget your thermal simulation allows per via. If a single via’s resistance is too high, increasing plating thickness from 25 µm to 35 µm cuts resistance by roughly 30 % without changing drill size—an approach that also improves via stitching performance for RF ground returns.

How Many Thermal Vias Do You Need?

Thermal vias in an array act as parallel resistors. The total array thermal resistance is:

R_array = R_single_via / N

So the required count is:

N = R_single_via / R_target

where R_target is the maximum allowable thermal resistance from pad to heatsink. For a GaN PA dissipating 10 W with a junction-to-case θ of 3 °C/W and a maximum junction temperature of 150 °C at 85 °C ambient, the entire board-level thermal path budget might be only 2–3 °C/W—demanding 60–100 vias of the 193 °C/W type, or far fewer if the vias are filled.

Enter your specific numbers in the thermal via count calculator:

Loading Thermal Via Count Calculator…

A realistic result for a 5 W MMIC on a 1.6 mm board with 0.3 mm plated-only vias and a 3 °C/W target might return around 65 vias. At a 0.6 mm center-to-center pitch (a tight but manufacturable grid), that array fits inside a 5 × 5 mm pad—tight, but feasible. If the count exceeds what your pad area allows, consider copper-filled vias, a larger drill, or a copper coin insert as an alternative.

Design Rules and Practical Limits

Parameter Typical Range Notes
Via drill diameter 0.20–0.40 mm (8–16 mil) Smaller drills cost more and plate less uniformly
Plating thickness 20–35 µm IPC-6012 Class 2 minimum is 20 µm; Class 3 is 25 µm
Via pitch (center-to-center) 0.5–1.0 mm Below 0.5 mm risks drill breakage and annular ring violations
Via fill Air / solder / copper paste / solid copper Copper-filled vias reduce R_thermal 3–4× but add process cost
Solder mask Tented or open Open vias under QFN pads risk solder wicking during reflow

For high-power RF boards, the thermal design strategy often combines a via array with heavy copper inner layers (2–4 oz) acting as lateral heat spreaders. The vias move heat vertically; the planes spread it horizontally. Both paths must be sized together.

Solder Wicking and Voiding

Open thermal vias under a QFN or BTC package can wick solder away from the pad during reflow, creating voids that increase thermal resistance—the opposite of what you intended. Common countermeasures are via-in-pad with copper fill and cap plate, or tenting the bottom side and plugging with epoxy. IPC-7093 on BTC assembly recommends limiting open via area to avoid excessive voiding.

When Vias Alone Are Not Enough

If the calculator returns a via count that cannot physically fit under the thermal pad—common above ~15 W in compact designs—consider a copper coin (a solid copper slug press-fit into a routed pocket). Coins offer thermal resistances below 1 °C/W through a 1.6 mm board, roughly 50× better than a plated-only via array of the same footprint. The trade-off is higher fabrication cost and a more complex stackup; our copper coin vs thermal via comparison breaks down the crossover point.

Quick Checklist

  1. Calculate single-via R_thermal from your drill, plating and board thickness.
  2. Determine R_target from your thermal budget (junction temp − ambient, minus package θ_jc and heatsink θ_sa).
  3. Divide to get the via count; verify the array fits inside the pad at your chosen pitch.
  4. If count is too high, switch to copper-filled vias or evaluate a copper coin.
  5. Specify via fill and solder-mask treatment in your fabrication notes to prevent solder wicking.

FAQ

What thermal conductivity should I use for via copper?

Use 385 W/m·K for bulk electrodeposited copper. Some references cite 390–400 W/m·K for pure copper, but plated copper has slightly lower conductivity due to grain structure and impurities. The 385 value is conservative and widely accepted in JEDEC JESD51-14 thermal test methods.

Are copper-filled vias always better?

Thermally, yes—they eliminate the hollow air core and reduce per-via resistance by 3–4×. But they add cost (copper fill + planarization + cap plating) and are unnecessary when plated vias at a reasonable count meet the thermal budget.

Can I use microvias for thermal management?

Laser-drilled microvias (typically 0.10–0.15 mm) have very small cross-sections and only span one layer, so their per-via thermal resistance is high. Stacked microvias through multiple layers can work but are expensive. Standard mechanical-drill vias are more cost-effective for thermal duty.

Does via pitch affect thermal performance?

Pitch determines how many vias fit under the pad, so it indirectly sets total array resistance. Tighter pitch means more vias and lower R_array, but pitches below 0.5 mm strain manufacturing tolerances and increase drill breakage risk.

Ready for a quotation?

Send your requirements for a material, stackup and manufacturing review. Price and schedule are confirmed for your project.

Upload Gerber