Design and order your first PCB

1. The path from idea to board

Write the idea down first in one sentence and a short list: supply voltage, current, size, connectors, how it will be mounted. Decide the board shape and mounting holes early, because they are hard to change once parts are placed. Expect to go round the loop more than once; a first board usually needs a second revision.

Software. KiCad is free and open source and runs on Windows, macOS and Linux; this guide uses it as the worked example. Others exist: EasyEDA (browser-based, with an ordering link to its own fab; verify its current terms), Autodesk Eagle and Fusion Electronics (licence and free-tier limits change, verify), CircuitMaker (Altium's free community tool, Windows; verify), and more. The ideas below are the same in all of them; only the menus differ, so menu names are described rather than quoted. Check each tool's current licence and file-export options before committing to it.

2. Schematic

• Start from the parts' datasheets, especially the "typical application" circuit. Copy it, then adjust.
• Draw power flow left to right if you can, one block per function (power, microcontroller, sensors, connectors). Label nets (names like 3V3, GND, SDA) instead of drawing every wire.
• Add a decoupling capacitor (typically 100 nF, ceramic) to every supply pin of every chip, plus a larger bulk capacitor (for example 10 uF) near where power enters. Check the datasheet for the value it wants.
• Add test points for power, ground and the signals you will want to probe, and a power LED with a resistor.
• Add reset and boot-mode pull-ups or pull-downs exactly as the chip's datasheet or reference design says; wrong strapping pins are a classic reason a board will not start.
• Run the tool's ERC (electrical rules check). It finds unconnected pins, outputs shorted together, and power pins nothing drives. Read each warning; do not just silence them. For power nets the tool often needs a "power flag" symbol to know a rail is supplied.
• Fill in a value and part number for every symbol now. It becomes your bill of materials (BOM).

3. Footprints: through-hole vs SMD

Each schematic symbol is assigned a footprint, the copper pad pattern that the real part is soldered to. Most wrong boards trace back to a wrong footprint, so check each one against the datasheet's land-pattern drawing and, if you can, print the layout 1:1 on paper and lay the real part on it.

Careful with names: an imperial code such as 0603 and a metric code such as 0603 mean different sizes (the metric 0603 is the imperial 0201). Always say which one. Sizes are nominal.

• Through-hole (resistors with legs, DIP chips, pin headers, big connectors): easy to solder and robust, good for first boards and for parts that take mechanical stress (connectors, switches).
• SMD (surface mount): smaller, cheaper, and what assembly services use. Start with 0805 or 0603 passives and chips with pin pitch 0.5 mm or more (SOIC, TSSOP, QFP). QFN/BGA parts with hidden pads need hot air or a reflow oven.
• Where a datasheet gives several footprint variants (nominal / most / least land protrusion, in IPC terms), the nominal one is a sound default for hand soldering.

4. Layout

Board outline and placement

Draw the board edge on its own layer, place connectors and mounting holes first, then the main chip, then the parts that must be close to it (decoupling capacitors, crystal, regulator capacitors). Group parts by function and keep connections short. Leave a few millimetres from copper to the board edge.

Layers: 2-layer vs 4-layer

• 2-layer (top and bottom copper): cheapest and enough for most hobby boards. Use the bottom as a mostly unbroken ground plane and route signals mainly on top.
• 4-layer (typical stack: signal / ground / power / signal): costs more but makes clean ground and power much easier. Worth it for fast processors, DDR memory, USB 3, or dense BGA parts. Ask the fab for its stack-up and impedance data before routing controlled-impedance lines.

Ground planes and return paths

Current flows in a loop: out along the signal and back along the ground. At higher frequencies the return current follows right underneath the signal. So: keep the ground under signals unbroken, do not route a fast signal across a gap or slot in the plane, and where you must change layers put a ground via next to the signal via. Keep switching converters' high-current loops (input capacitor, switch, inductor) small and tight.

Trace width and spacing: rules of thumb

• Signals that carry little current: 0.2 to 0.25 mm (8 to 10 mil) is a comfortable choice. Many cheap fabs manage 0.15 mm (6 mil) or finer, but wider is more forgiving.
• Power: size from the current with the calculator below; as a quick feel, 1 A on 1 oz external copper with a 10 degC rise is about 0.3 mm, and it is cheap to go much wider. Prefer a plane or a wide pour for main supply.
• Spacing: at least the fab's minimum, and more where you can (0.2 to 0.3 mm). For voltages above a few tens of volts, increase it; see "clearance" below.
• Use 45 degree or rounded corners rather than sharp 90 degree ones (mostly manufacturing neatness; electrically it matters little at hobby speeds).

Vias

A via connects layers with a plated hole. A common cheap size is about 0.3 mm drill with a 0.6 mm pad; 0.4 / 0.8 mm is more forgiving (verify your fab's minimum). Each via adds a little resistance and inductance; use several in parallel for power, and a via-in-pad only if the fab supports it (it may cost extra, since it needs filling). Avoid vias inside pads that will be hand-soldered, because solder wicks into them. Tenting (covering the via with solder mask) is common.

Decoupling placement

Place each small capacitor as close as you can to the chip's supply pin, with the path pin -> capacitor -> ground as short as possible, ideally with the capacitor between the pin and its ground via, rather than a long trace out and back. A bigger capacitor a little farther away is fine.

Power routing

Route power as wide traces or planes, using star or tree routing from the entry point so heavy loads do not share thin sections with sensitive ones. Put the input protection (fuse or polyfuse, reverse-polarity protection, TVS diode where appropriate) right at the connector. Keep noisy loads (motors, relays, LEDs strips) off the same thin branch as analog sensors or the microcontroller's reference voltage. Use a flyback diode across relays and motors.

Thermal relief

Pads connected directly to a big copper area soak up heat and are hard to hand-solder. A thermal relief connects the pad through a few thin spokes so soldering is easy; most tools do this by default for zone fills. For parts that need to shed heat (regulators, power MOSFETs, exposed pads) use a larger copper area and several thermal vias, and follow the datasheet's thermal pad advice.

Clearance and creepage

Check your fab and the voltage. The spacing needed between conductors depends on voltage, altitude, pollution and coating, and is set by standards. At 5 V and 12 V the fab's minimum is enough; above roughly 50 V, give copper much more room and read the relevant standard; for mains do not design your own.

Silkscreen

Label connectors, pin 1 marks, polarity, board name and revision, and test points. Keep text off pads and at a readable size (about 0.8 to 1 mm high, with a stroke of around 0.15 mm, is a common minimum; verify with the fab). Silkscreen on pads is usually clipped, so move it.

Antenna keep-outs

Wi-Fi/Bluetooth modules with a PCB antenna need a keep-out: no copper, ground pour, tracks or components under or immediately around the antenna area, and the antenna end sits at the board edge with nothing metal nearby. The module's datasheet or hardware design guide draws the exact area; follow it literally. Do not put a battery, metal enclosure part or big connector right next to it.

5. Trace width calculator

6. High-speed basics (short version)

• Treat a trace as a transmission line when its length is a noticeable fraction of the signal's rise time distance. Fast edges, not clock frequency alone, are what matter.
• USB 2.0 full-speed is forgiving; high-speed USB, Ethernet, HDMI, DDR and radio need controlled impedance: the fab's stack-up (copper, dielectric thickness, dielectric constant) plus trace width and spacing set it. Use the fab's own impedance calculator or a field solver; do not guess.
• Route differential pairs together with constant spacing, equal length, and an unbroken reference plane under them. Avoid stubs and avoid placing vias unevenly.
• Keep crystal traces short, with ground under and around, away from noisy lines.
• When in doubt, copy a manufacturer's reference layout for the chip.

7. Checks before you order

• DRC (design rules check): set the rules (minimum trace, space, drill, annular ring, clearance to the board edge) to your fab's capabilities before routing, run the check at the end, and fix every error. Understand any warning you leave.
• ERC on the schematic and a check that the layout matches the schematic (update the board from the schematic and confirm no unrouted nets remain).
• Look at the 3D view for part collisions, connectors facing the wrong way, and mounting-hole fit.
• Print 1:1 and place the real parts on the paper.
• Open the generated Gerbers in a viewer (KiCad includes one; free online viewers also exist) and compare them with what you expect, including drill files and board outline.

Design-for-manufacture checklist

• Trace width, space and drills at or above the fab's minimums (with margin).
• Annular ring (copper around a drilled hole) at least the fab's minimum; pad bigger than the drill by that ring on every side.
• Copper and silkscreen kept away from the board edge; the edge-cut outline is a single closed shape.
• Solder-mask openings and a minimum mask bridge between fine-pitch pads (otherwise the fab may merge them; verify).
• Fiducials and a clear border if you will have it assembled by machine.
• Polarised parts (diodes, electrolytics, ICs) marked on silkscreen with pin 1.
• Panelising and tooling rails only if the assembler asks for them.

8. Files to send

KiCad can generate Gerbers, drill files, position files and a BOM; fabs often publish a profile or settings page for their preferred output options. Whatever you use, upload to the fab's own online viewer and look at every layer before paying.

9. Reading a fab house's capabilities table

Every fab publishes a table of what it can make. Typical entries (generic; the numbers vary and change, so read your fab's own table):

Customs duty, shipping time and minimum-quantity rules vary by country and fab. Prices are deliberately not listed here.

10. Assembly

• By hand: solder low and small parts first, then taller ones; see the soldering guide. Order the process so that the hardest parts (fine-pitch chips) go first.
• By the fab (PCBA): send BOM and pick-and-place with the Gerbers. Choose parts the assembler stocks, check the stock before finishing the design, and review their placement preview for rotated parts.
• First power-up: look for solder bridges, check with a multimeter that the power rail is not shorted to ground (resistance reading), then power from a current-limited bench supply (set a low limit first), and measure the rails before connecting sensitive chips.

11. Making a board yourself

For simple one- or two-layer boards you can make your own. Ordering is usually cheaper and better looking, but DIY is quick for tiny experiments.

• Toner transfer: print the mirrored layout with a laser printer onto glossy paper, iron it onto clean copper-clad board, soak the paper off, and etch. Fiddly; fine lines are hard.
• Photo-resist: use pre-sensitised board, expose it under UV through a transparent printout, develop, then etch. Gives finer, repeatable results.
• CNC milling (isolation routing): a small machine cuts around the traces. No chemicals, but needs a machine, dust control and eye protection.

12. Common beginner mistakes

• Wrong footprint (mirrored connector, wrong pin pitch, SOIC-8 narrow vs wide); check against the datasheet and print 1:1.
• No decoupling capacitors, or placed far from the chip.
• Ground plane cut up by routing, or signals crossing gaps.
• Traces too thin for the current, or too close for the voltage.
• Leaving the pin-1 or polarity marker off the silkscreen.
• 3.3 V and 5 V parts joined without level shifting.
• Forgetting test points, a programming header, or a way to power the board safely.
• Ordering a bare board before checking that the parts are in stock.
• Antenna keep-out ignored (poor range).
• Not checking the Gerbers in a viewer before paying.

Next steps: the electronics pages on this site include Electronics calculators for resistor values and similar, the Circuit cookbook for tried circuits to copy, and the Electronics cheat sheet. To pick a board for a project first, use the hardware board chooser.

Mentioned tools and their licences, free tiers and fab capabilities change over time: verify on the maker's own page. Last checked November 2026.