From Schematic to Board: The Complete KiCad 8 Workflow Step by Step
KiCad is a free, open-source electronics design suite that is good enough for professional products and simple enough for a first project. Its tools are separate programs that share one project, and beginners often get lost because they do not know which tool comes next. This article gives you the map: the order of steps, which window each step happens in, and what file each step produces.
We will use a small example throughout: a 555 timer LED blinker powered from a 2-pin header. It has about ten parts, which is enough to exercise every stage without getting lost in the circuit itself.
The KiCad 8 Project and Its Files
Start KiCad and choose File > New Project. Give it a name such as blinker. KiCad creates a folder containing three key files. The project manager window then shows buttons for each tool.
| File or tool | Purpose |
|---|---|
| blinker.kicad_pro | Project settings, net classes and design rules |
| blinker.kicad_sch | The schematic drawn in the Schematic Editor |
| blinker.kicad_pcb | The board layout drawn in the PCB Editor |
| Symbol Editor | Create or edit schematic symbols |
| Footprint Editor | Create or edit physical land patterns |
| Gerber Viewer | Inspect the manufacturing files you generate |
| Calculator Tools | Track width, via, regulator and impedance calculators |
Stage 1: Capture the Schematic
Open the Schematic Editor. Place parts with Place > Add Symbol (hotkey A). For the blinker you need an NE555P from the Timer library, two resistors R, a capacitor C for timing, a 10 nF control capacitor, a current-limiting resistor and LED, and a Conn_01x02 header for power. Add power symbols with Place > Add Power (hotkey P) and choose +5V and GND.
Draw wires with W, rotate with R and move with M. When the circuit is complete, run Tools > Annotate Schematic so every part gets a unique reference such as R1, R2 and C1. Then run Inspect > Electrical Rules Checker and fix every error before going further. ERC catches unconnected pins and power nets with no driver, which are much easier to fix now than on the board.
Stage 2: Assign Footprints
A symbol only describes the electrical pins. The footprint describes the copper pads that the real part will be soldered to. Open Tools > Assign Footprints. On the left you see footprint libraries, in the middle your symbols, and on the right the matching footprints. For the blinker, reasonable choices are:
| Part | Footprint |
|---|---|
| NE555P | Package_DIP:DIP-8_W7.62mm |
| Resistors | Resistor_THT:R_Axial_DIN0207_L6.3mm_D2.5mm_P10.16mm_Horizontal |
| Ceramic capacitors | Capacitor_THT:C_Disc_D5.0mm_W2.5mm_P5.00mm |
| LED | LED_THT:LED_D5.0mm |
| Power header | Connector_PinHeader_2.54mm:PinHeader_1x02_P2.54mm_Vertical |
Always check the footprint against the datasheet of the part you will actually buy. Pin pitch, hole size and body size vary between manufacturers, and a wrong footprint is the most common reason a first board cannot be assembled.
Stage 3: Transfer to the PCB Editor
- Open the PCB Editor and choose File > Board Setup. Under Board Stackup set two copper layers and 1.6 mm thickness; under Design Rules > Constraints enter your fab's minimum clearance and track width.
- Run Tools > Update PCB from Schematic (F8). All footprints arrive in a bundle, connected by thin ratsnest lines that show which pads must be joined.
- Select the
Edge.Cutslayer and draw the board outline with Place > Draw Rectangle, for example 40 mm by 30 mm. - Drag footprints into position. Put the power header on an edge and the LED where it will be visible. Rotate with R and flip to the bottom with F only if you mean to.
- Route tracks with Route > Route Single Track (X). Use 0.5 mm for power and 0.25 mm for signals on this simple board.
- Add a ground pour with Place > Add Filled Zone on
B.Cu, assign it to the GND net, then press B to fill all zones. - Run Inspect > Design Rules Checker and clear every error and unconnected item.
Press Alt+3 to open the 3D Viewer. It is a quick sanity check that parts are on the correct side, nothing overlaps, and the LED faces the right way.
Stage 4: Fabrication Outputs
Once DRC is clean, use File > Fabrication Outputs > Gerbers and File > Fabrication Outputs > Drill Files to generate the files the fab needs, then open them in the Gerber Viewer to check them. Zip the output folder and upload it to your fab. A later article covers the exact settings.
Going Back and Forth
Design is rarely linear. If you change a value or swap a part in the schematic, simply save and press F8 again in the PCB Editor. KiCad updates only what changed and keeps your placement and routing. Never edit connections directly on the board without changing the schematic, because the two will drift apart and DRC will report schematic parity errors.
Common Workflow Mistakes
- Skipping ERC because the schematic looks right. A missing junction dot can leave a wire visually touching a pin but electrically open.
- Forgetting to assign footprints, which makes Update PCB from Schematic report errors and skip parts.
- Drawing the board outline on a copper or silkscreen layer instead of
Edge.Cuts. - Routing before placement is final. Moving parts later turns neat routing into a tangle.
- Ignoring DRC warnings about unconnected items; each one is an open circuit on the real board.
Summary
The KiCad 8 flow is schematic, ERC, footprint assignment, Update PCB from Schematic, outline, placement, routing, zones, DRC and finally fabrication outputs. Each stage has a check built in, and passing each check before moving on saves days of rework. The rest of this series zooms into each stage in detail, starting with how to draw a clean, readable schematic.