PCB Basics: Layers, Copper Weight, FR-4 Laminate and Vias Explained
A printed circuit board (PCB) does two jobs at once. It holds components mechanically, and it connects them electrically through copper tracks instead of loose wires. Before you open KiCad and start drawing, it helps to know what the board is physically made of, because almost every design rule you will meet later comes from these materials and from how a fabrication house processes them.
This article walks through the layers of a typical board from top to bottom, explains what copper weight means, why FR-4 is the default material, and how vias carry signals between layers. By the end you should be able to read a fab's capability page and understand every line on it.
What a Two-Layer Board Is Made Of
The most common hobby and student board is a two-layer board, 1.6 mm thick. If you cut one in half and looked at the edge under a magnifier, you would see the following stack, listed from the top surface downward.
| Layer | Material | Purpose |
|---|---|---|
| Top silkscreen | Epoxy ink, usually white | Reference designators, logos, polarity marks |
| Top solder mask | Liquid photo-imageable polymer, usually green | Insulates copper and stops solder from spreading |
| Top copper | Copper foil, typically 35 um | Tracks, pads and copper pours |
| Core | FR-4 glass-epoxy laminate | Mechanical strength and insulation between copper layers |
| Bottom copper | Copper foil | Second routing layer, often a ground plane |
| Bottom solder mask | Polymer | Same as top |
| Bottom silkscreen | Ink | Optional markings on the underside |
In KiCad these physical layers appear with names such as F.Cu and B.Cu for front and back copper, F.Mask and B.Mask for solder mask, and F.Silkscreen and B.Silkscreen for the printed markings. There are also non-manufactured helper layers such as F.Courtyard and F.Fab that guide placement and documentation but are not printed on the board. The board outline lives on Edge.Cuts.
Copper Weight: What 1 oz Means
Copper thickness is specified by weight rather than by thickness. One ounce copper means one ounce of copper spread evenly over one square foot of board area. That works out to a thickness of roughly 35 micrometres, or about 1.37 mil. Doubling the weight doubles the thickness.
| Copper weight | Approximate thickness | Typical use |
|---|---|---|
| 0.5 oz | about 17.5 um | Inner layers of fine-pitch multilayer boards |
| 1 oz | about 35 um | Default for most two-layer and four-layer boards |
| 2 oz | about 70 um | Power boards, motor drivers, high current tracks |
Thicker copper carries more current for the same track width, but it is harder to etch finely, so fabs usually require wider minimum track and gap widths for 2 oz boards. For your first projects, 1 oz outer copper is the sensible choice. Later in this series we use copper weight directly in the IPC-2221 track width calculation.
FR-4: The Default Board Material
FR-4 is a grade designation for woven fibreglass cloth bonded with flame-retardant epoxy resin. It is cheap, stiff, a good insulator and easy to drill, which is why nearly every low-cost fab uses it as standard. A few properties matter to a designer.
- Thickness: 1.6 mm is the standard finished thickness. Thinner options such as 0.8 mm or 1.0 mm are common for small or wearable boards.
- Glass transition temperature (Tg): the temperature at which the resin starts to soften. Standard FR-4 sits around 130 to 140 degrees C; high-Tg grades are used for boards that see repeated lead-free reflow or high operating temperatures.
- Dielectric constant (Er): roughly 4 to 4.7 depending on the resin, glass weave and frequency. It sets the impedance of tracks, which matters for USB, Ethernet and RF.
- Alternatives: aluminium-core boards for LED lighting, polyimide for flexible circuits, and specialised laminates for microwave work.
Vias: Moving Between Layers
A via is a small drilled hole whose wall is plated with copper, connecting a track on one layer to a track or plane on another. A via is described by two numbers: the drill (hole) diameter and the pad (annular ring) diameter. The annular ring is the copper left around the hole; it must be wide enough that a slightly off-centre drill does not break out of the pad.
Annular ring = (via pad diameter - drill diameter) / 2 Example: pad 0.6 mm, drill 0.3 mm Annular ring = (0.6 - 0.3) / 2 = 0.15 mm
| Via type | Connects | Cost and use |
|---|---|---|
| Through-hole via | Top to bottom, through every layer | Cheapest; the only type most hobby boards need |
| Blind via | An outer layer to an inner layer | Extra cost; dense multilayer boards |
| Buried via | Inner layers only, invisible from outside | Extra cost; high density designs |
| Microvia | Adjacent layers, laser drilled | HDI boards such as phones |
Through-hole component pads are plated holes too, so a two-layer board gets free layer changes at every through-hole pin. Vias can also be covered (tented) by solder mask so they do not short to anything and do not wick solder during assembly.
Common Beginner Misunderstandings
- Assuming the board edge is wherever the copper ends. The outline must be a closed shape on
Edge.Cuts, or the fab cannot cut the board. - Choosing tiny vias to save space when the board has plenty of room. Larger vias such as 0.3 mm drill with 0.6 mm pad are cheaper to make reliably.
- Forgetting that copper weight affects minimum spacing. A track gap that is fine on 1 oz copper may be rejected on 2 oz.
- Treating silkscreen as electrical. Ink on top of a pad is clipped by the fab and can make a board look messy, but it never connects anything.
Summary
A standard PCB is a 1.6 mm FR-4 core with copper foil on each side, protected by solder mask and labelled with silkscreen. Copper weight in ounces sets the foil thickness, with 1 oz being about 35 um. Vias are plated holes that join layers, defined by drill and pad diameter, and the annular ring between them must satisfy your fab's minimum. With these basics in place, the next step is learning the KiCad workflow that turns a schematic into exactly this physical stack.