RF PCB Engineering Tools

PCB Thickness Calculator | Core Prepreg Copper Stack

Calculate your finished PCB thickness by stacking core, prepreg and copper layers with interactive tools. This guide covers standard and RF stackups, tolerance budgets and the factors that shift your final number.

Cross-section of a multilayer PCB showing core, prepreg and copper layers

How a PCB Thickness Calculator Works

A PCB thickness calculator sums every physical layer in your stackup—cores, prepregs, copper foils and surface finishes—to predict the finished board thickness before fabrication. For a standard 4-layer FR-4 board the result is typically 1.57 mm (62 mil), but RF and microwave designs using Rogers, Isola or PTFE laminates often land on non-standard values that must be verified layer by layer. Getting this number right matters because it controls impedance, connector fit, card-edge compliance and thermal performance.

Layer-by-Layer Breakdown

Hybrid RF PCB showing Rogers and FR-4 material regions

Copper Foil

Copper is specified by weight per unit area. The most common weights and their nominal thicknesses are:

Copper Weight Nominal Thickness (µm) Nominal Thickness (mil)
½ oz 17.5 0.69
1 oz 35 1.38
2 oz 70 2.76

After plating, inner-layer copper stays at its starting weight, but outer layers gain roughly 20–25 µm from the electroplating process. Your calculator should account for this plated copper addition on the two outer faces. If your design also carries high-current traces, a trace width calculator helps you verify that the chosen copper weight can handle the load.

Core

A core is a cured laminate with copper already bonded to both sides. Standard FR-4 cores come in fixed thicknesses—0.1 mm, 0.2 mm, 0.36 mm, 0.51 mm, 0.71 mm, 1.0 mm and 1.2 mm are the most common. RF-grade cores such as Rogers RO4350B are available in 6.6 mil (0.168 mm), 10 mil (0.254 mm), 20 mil (0.508 mm) and 30 mil (0.762 mm), among others. The core thickness listed on a datasheet is the dielectric only, excluding the copper cladding on each face.

Use the tool below to look up standard core dielectric thicknesses for your chosen material family.

Loading Core Thickness Finder…

For example, selecting a 10 mil RO4350B core with 1 oz copper on each side gives a per-core subtotal of 0.254 mm + 2 × 0.035 mm = 0.324 mm. In an RF stackup where dielectric thickness directly sets characteristic impedance, even a 1 mil deviation here shifts a 50 Ω microstrip by roughly 2–3 Ω—so always confirm the core thickness against the manufacturer’s datasheet rather than relying on a generic catalog value. More on how thickness choices affect RF performance is covered in our guide on how thick an RF PCB should be.

Prepreg

Prepreg is the partially cured glass-resin sheet that bonds cores together during lamination. Its pressed thickness depends on the glass style (106, 1080, 2116, 7628 are common), the number of plies, and the resin content of the prepreg, which also shifts Dk and Df in RF designs. A single sheet of 7628 prepreg presses to roughly 0.18 mm (7.1 mil), while a single 1080 sheet presses to about 0.065 mm (2.6 mil). Fabricators often stack two or three sheets between core pairs to hit a target bond-line thickness, so always specify the pressed thickness you need rather than just the glass style.

Surface Finish

Surface finish adds a small but non-negligible amount. ENIG adds roughly 3–6 µm of nickel plus 0.05–0.13 µm of gold. HASL adds 1–25 µm of solder depending on pad geometry. For most stackup calculations, surface finish contributes less than 0.5 mil per side and can be treated as a rounding factor, but for tight-tolerance assemblies (card-edge connectors, press-fit pins) it should be included explicitly.

Calculate Your Finished Board Thickness

Enter each layer—cores, prepregs, copper foils and finish—into the accumulator below. It sums them and reports the finished thickness in both mm and mil.

Loading Board Thickness Accumulator…

A typical result for a 6-layer hybrid stackup (two 10 mil RO4350B cores, two 4 mil bond plies, two FR-4 cores at 0.36 mm, 1 oz copper throughout, ENIG finish) might read around 1.45 mm (57 mil). If your target is the standard 1.57 mm card-edge slot, you would increase the FR-4 core pair or add a prepreg ply. If the result overshoots, switching from 7628 to 2116 prepreg can shave 3–4 mil per bond line.

IPC Tolerances on Finished Thickness

IPC-6012 defines finished-thickness tolerances based on the nominal value. For boards ≤ 0.78 mm the tolerance is ±0.08 mm; for boards 0.78–2.36 mm it widens to ±0.13 mm; above 2.36 mm it is ±10 %. These are Class 2 (standard) values—Class 3 (high reliability) tightens them further. Always compare your calculator output against these bands before releasing Gerbers, because a stackup that theoretically hits 62 mil can land anywhere from 57 to 67 mil in production if prepreg flow and copper distribution are not controlled. Consult the IPC-6012 specification for the full tolerance tables by class and board type.

Common Pitfalls

  • Ignoring copper distribution. Areas with heavy copper fill press down prepreg less than sparse areas. The result is local thickness variation that a single-number calculator cannot capture. Ask your fabricator for a pressed-thickness simulation on complex RF boards.
  • Mixing metric and imperial. Rogers datasheets list core thickness in mils; many FR-4 vendors use millimeters. A unit mismatch in your stackup spreadsheet can introduce a 30 % error on a single layer.
  • Forgetting plated copper on outer layers. Plating adds ~25 µm per side (roughly 1 mil). On a thin 0.8 mm board, that is 6 % of total thickness.
  • Assuming prepreg thickness equals the datasheet “cured” value. Actual pressed thickness depends on copper voids the resin must fill. More voids mean thinner pressed prepreg.

From Thickness to Cost

Board thickness affects panel yield, drill aspect ratio and lamination cycle time—all direct cost drivers. A 0.8 mm board allows smaller via diameters but may require thinner cores that cost more per sheet. A 3.2 mm board needs back-drilling for high-speed vias and longer press cycles. Once your stackup is locked, run it through an RF PCB cost estimator to see how material and layer count choices move the price.

FAQ

What is the standard PCB thickness?

The most common standard is 1.6 mm (approximately 62 mil, or 63 mil before finish). This originated from the NEMA-grade laminate era and remains the default for most 2- to 6-layer FR-4 boards.

Does copper weight count toward board thickness?

Yes. Each ounce of copper adds 35 µm (1.38 mil) per layer. On a 4-layer board with 1 oz copper on every layer, copper alone accounts for about 0.14 mm—nearly 9 % of a 1.6 mm board.

How accurate is a PCB thickness calculator?

A well-configured calculator is typically within ±2–3 % of the measured result. The main source of error is prepreg flow variation due to copper pattern density, which requires a fabricator’s lamination model to predict precisely.

Can I use a thickness calculator for RF laminates like Rogers?

Yes, provided you enter the correct core and bond-ply thicknesses from the laminate datasheet. Rogers publishes pressed-thickness data for each prepreg type; using generic FR-4 values will give incorrect results.

Ready for a quotation?

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

Upload Gerber