KiCad Overview

An open source electronics design software package.
https://www.kicad-pcb.org

Shawn Hymel from Digikey has a good overview tutorial playlist. Here's a summary for future reference.

video

Workflow:

• Design circuit
• Create symbols (in the Symbol Editor)
• Schematic Capture (in the Schematic Layout Editor)
• Create footprints (in the Footprint Editor)
• Generate Netlist
• Board Layout (in the PCB Layout Editor)

• In the Symbol Editor: File > New Library.
  • Save the .lib file local to your project (eg: projects folder) or available to multiple projects (eg: documents > KiCad > Libraries).
• Choose Global if the symbol can be used for multiple projects or Project if it's project-specific.

• In the Symbol Editor: File > New Symbol
• Select the library you just created
• Give the symbol a name & Reference designator code. Click OK
• Shortcuts: hover mouse over object and press:
  • m (move)
  • r (rotate)
  • e (edit)
  • x (delete)
  • insert-key (duplicate current pin). If the key doesn't work, change it to something else in preferences > Hotkeys > Repeat Pin. I set it to d.
• Click 'Add pins' icon on the right (or press p), and click anywhere on the page to add a pin. Enter the name and pin number.
• Pin conventions:
  • Pin names are in capitals
  • Starting a pin name with ~ gives the pin name a horizontal bar over the name, indicating the pin is active LOW.
  • Put pins 2 grid spaces apart for legibility.
• place all pins and orient them with the little circle on the outside.
• draw box (graphic rectangle icon) touching the straight ends of the pins.
• Symbol conventions
  • Origin should be in the center
  • The Reference designator goes to the top left of the symbol
  • The part name sits in the bottom right of the symbol box
• Save and close.

Annotate schematic

• tools > annotate schematic. This replaces the question marks in the reference designators with numbers. This makes identifying specific components possible.
• Click Annotate, and then Close

Assign footprints

• tools > assign footprints. A 3 columns window pops up. On the left are the different footprint libraries. On the right, the contents of all library collections. In the middle a list of all the components.
• click on the first component. Use the filter options at the top to narrow down the footprints in the right column. Take your time here. Make sure you'll select the right footprint for the symbol.
  • THT: through hole technology
  • SMD: Surface mount technology
  • Radial: two leads coming from one side of the component (ie: a regular electrolytic capacitor)
  • Axial: leads extending through the component's core from both sides (ie: a regular transistor)
  • D: diameter
  • P: pitch
• If you found a candidate in the right column, select it and press the 'view selected footprint' in the menu bar to visually check if it's the right part.
• If it is the right component, double-click to assign it to the selected component in the middle column.

Generate netlist

• tools > Generate netlist File. Leave default settings and click Generate Netlist. Save the file in your project folder and close the Schematic Layout Editor.

• open PCB Layout Editor.
• Make sure the units are set to inches.
• set Grid to 50 mils.
• Tools > Load Netlist. Load the previously made netlist, click update PCB and click close. Put the mess of components down outside the working area.

set design rules Set following values according to PCB manufacturer. The values here are set by [Seeed Studio ](https://www.seeedstudio.com/). It's always a good idea to have larger margins. If 6 mils of trace width is specified, you could go with 10 mils to be on the safe side.

• File > Board Setup > Design Rules > Solder Mask/Paste
  • Solder mask: 16mil (0.4mm)
• File > Board Setup > Design Rules
  • Minimum track width: 10 mil
  • Minimum via diameter: 32 mil (total width of the drill hole including both sides of the annular ring)
  • Minimum via: 15 mil (The drill diameter)
• File > Board Setup > Design Rules > Net Classes. In the default net-class, change the following values:
  • Default class (for signal traces)
    • Clearance: 10 mils
    • Track Width: 10 mils
    • dPair Width: 10 mils
    • dPair gap: 9,8 mils
    • Via size: 32 mils
    • Via Drill: 15 mils
  • Power class (for power and GND traces)
    • Clearance: 12 mils
    • Track Width: 30 mils
    • dPair Width: 30 mils
    • dPair gap: 19,8 mils
  • Assign the right class for each net by selecting it in the drop down menu on the right of each item.
• click OK
• Read manufacturers specifications and panelization pages carefully.

Part layout

• move your parts to the locations you'd like them to be. Hover your mouse over a part and press m.
• Try to make the air-wire structure as simple as possible. (At least as possible crossovers).
• Using the 'route tracks' icon, change the air-wires into actual traces. It's best to do this manually.
  • choose the layer (F.cu = front copper, B.cu = back copper)
  • Use d on elements of the traces to move them around
• Keep space for fingers in mind when using connectors
• keep conductive things underneath the PCB in mind (for example: programming pins or the USB connector on a microcontroller). Make sure you don't get unwanted connections
• When layout is finalised perform a design rule check: Inspect > Design Rules Checker
• Arrange the silkscreen elements to give info when the PCB is made.