Electronics Design

Introduction to Kicad interface

For creating new project: Files >> New Project

When you create a new project in KiCad, it automatically generates the project folder along with the schematic file and the PCB file.

Schematic Editor interface

A schematic is used to draw and plan an electronic circuit before creating the actual PCB. It shows components using standard electronic symbols and uses wires (lines) to connect them, representing how electricity flows in the circuit.

In simple terms, a schematic is the blueprint of your electronics project, helping you clearly organize connections and avoid mistakes before designing the physical PCB.

Shortcut Keys for Schematic Editor

Shortcut keys	Purpose
A	Place symbols(add)
M	For moving symbols
R	Rotate a symbols, press 'R' again to rotate in different direction
Y	Mirror a symbol vertically, top-bottom
X	Mirror a symbol horizontally, left-right
Ctrl + L	For placing or giving a global label to symbols
E	Edit properties
Q	Place no connection Flag
G	For dragging a symbol with the connected wire
Delete	Remove a symbol
W	Start a wire
~	For checking symbol connection

PCB (Printed Circuit Board) Editor

The PCB Editor in KiCad is used to design the physical layout of your circuit board. After creating the schematic, you import it into the PCB Editor, where you place the components, arrange them properly, and draw copper tracks to connect them.

The right toolbar contains tools to add footprints, draw tracks, add text, and create board outlines, while the top toolbar allows you to rotate, mirror components, edit footprints, run checks, import/update from the schematic editor and open the 3D viewer.

Shortcut Keys for Schematic Editor

Shortcut keys	Purpose
X	To draw track
Ctrl+Shift+X	To draw fill zone
A	Place footprint
Alt+3	To view pcb in 3d viewer
F8	Update the pcb from schematic editor

Installation of Fablib

FabLib is a KiCad library made for Fab Academy that includes most components from the Fab Lab inventory, so their symbols and footprints can be easily added, ensuring a 1:1 match for PCB designing.

Go to Tools >> Plugin and Content Manager (or press Ctrl + M) >> Open the Libraries tab >> Search for KiCad FabLib >> Click Install >> Click Apply Pending Changes

From Schematic to PCB Layout and 3D View

Our instructor introduced us to KiCad and explained what can be done using the software. To understand the workflow, we created a simple project starting from circuit design, then moved to the PCB layout, and finally viewed it in 3D view. For this circuit, we used ATtiny412, LEDs, two resistors, an FTDI header, and a capacitor.

Here is the workflow:

---

Creating the Circuit in the Schematic Editor

Once you create the project file, open the schematic editor.

Adding a symbol

Then press A on the keyboard or select Place Symbol from the right toolbar. A dialog box will open where you can search for components.

Search for attiny412 fab and select it. On the right side, you will see the symbol and footprint. Make sure the component has a footprint assigned, because this footprint will be used later when switching to the PCB editor.

Attiny412: Microcontroller

source: Pinout Datasheet

Components and their symbols used:

Methods of Connecting Components: Wire connection and Global label

There are two ways to connect component symbols in the schematic: either by drawing wires between the components or by using labels, such as global labels, to connect them logically. It also allows to use both methods together in the same schematic editor.

1. Wire Connection: Components are connected by drawing wires directly between their pins, which visually shows how each component is linked in the circuit.

At the bottom, there is an option called Selection Filter. By ticking just the "Wires", and unselecting others; only the wires in the schematic can be selected. This allows wires to be selected and deleted easily without accidentally selecting symbols or other elements, no mess of clicking on each wire individually.

2. Global Labels: Instead of drawing long wires, labels with the same name are used to connect points logically. The same label should be used on the microcontroller pin and the component pin to create the connections.

Place a global lablel is like giving a global variable, which can me used through out. For that either press "ctrl + L" or from the right tool select "place gloabl label."

LED Series Resistor Calculator

As I was using an LED on my PCB, I needed to find out what the appropriate resistor value to limit the current and protect the LED. For that, I used this calculator by DigiKey .

source: Digikey

Adding values to components

To rename or give a value to a resistor or capacitor, double-click on the name like R or C_1206 and change it to the value you want. For example, I wanted 1k resistor and 1 µf capacitor. This is just for labeling in the schematic, so we know which value component to use. It does not actually set the value, it only shows the value in the design.

Crossing unconnected pins

After connecting the symbols, some ports were left unconnected. So i used Place No Connect Flag (Q) , which comes with a cross symbol and placed it on those pins. It indicates that the pin is intentionally left unconnected, which helps avoid ERC (Electrical Rules Check) warnings and errors in the schematic.

Organizing the Schematic for better documentation

To organize the schematic, I used the Rectangle tool to group components. At first, I tried dragging directly, thinking it would draw the rectangle, but that only worked for selection, not for creating the rectangle. So the correct way was to click once from where it needed to start and then dragged it, making the component circuit inside the rectangle. After placing the rectangle, I clicked on it to change its properties, such as the line type, color, width, border style, or making it filled.

For adding text, I used the Text tool (T). After placing the text, I could change the font type, color, and size from the text properties. This helped label and organize the schematic clearly.

Connection Check

Using ~ (tilde, the key above Tab): to check the components connected to the microcontroller.

Place the pointer over a component's symbol and press ~, the component turns pink, and the connection of that to the microcontroller also turns pink. This shows where the connection goes and which components are connected to it, helping verify that the microcontroller connections are correct.

Run ERC (Electrical Rules Check)

Then run ERC (Electrical Rules Check) to find errors or warnings like missing connections or unconnected pins before moving to the PCB editor. Some warnings can be ignored if you have proper reason for that, as mentioned by the instructor, but errors should not be ignored.

Final Schematic Design

Download: schematicdesign

Converting the Circuit to PCB Layout

Using switch to PCB Editor and open the PCB in the PCB Editor window from the schematic window.

Using Update PCB from Schematic Editor, the symbols from the schematic are brought into the PCB editor as footprints. This tool is also useful later if any changes or updates are made in the schematic editor, as it allows the PCB to be updated again while iterating on the design.

As it got updated, closed the pcb update tab; I was like where is my pcb footprints. It turned out to be in the top left corner, far from work area. Just move them to work area, for moving a component press "M".

Board Setup: Design Rule setup >> Constraints

Before routing the tracks, the constraints were updated according to the milling capabilities of our lab machine.
So I went to Board Setup >> Design Rules >> Constraints and updated the values.

Then in Predefined Sizes, the track width was set to 0.4 mm and saved.

This was done because the milling tool in the lab has a minimum width it can safely cut. If the tracks or clearances are too small, the machine may not mill them properly or the traces may get damaged.

Route Tracks: Tracing

Route Tracks(X): Draws the copper connections between components on the PCB.
This step took me hours because each track had to find a path without crossing others. It felt like solving a tricky puzzle. At first, it was fun. Later, it became tiring when the connections didn't get solved easily. After trying different arrangements and adjusting tracks, I finally managed to connect everything. Finally, I felt a great sense of relief.
The routing was done on the F.Cu layer (Front Copper layer).

Board boundary: Edge cut drawing

After routing, a board boundary was created so the system knows the shape of the PCB and were the components is placed on, which is also needed for the 3D view and milling.

For that, I used the Rectangle tool, making sure the rectangle was placed on the F.Edge.Cuts layer, otherwise KiCad will not understand it as the board cut.

To give the board rounded corners, I right-clicked on the rectangle and selected Shape Modification >> Fillet Lines, then entered a value for the fillet.
I also wanted a hole in the board, so I used the Circle tool on the F.Edge.Cuts layer to create it.

DRC: Design rules checker

Design Rule Check (DRC) verifies the PCB layout by automatically checking for design errors and manufacturing rule violations. It helps identify issues such as unconnected nets, insufficient clearances, overlapping objects before the PCB is fabricated.

The warning was a silkscreen clipping warning for the SW1 reference. This warning was ignored as the PCB was fabricated without a silkscreen layer.

Final PCB Layout

3D Viewer

Using the 3D Viewer, a new window opens where I can see the 3D visualization of the designed PCB.

Desgning circuit in Schematic Editor

I started the circuit design using a XIAO RP2040, NeoPixel LED, resistor, capacitor, button, I2C pin, and a 1x6 pin header.

Seed Studio: XIAO-RP2040

It was like switching between the schematic editor and PCB editor, changing the pin connections in the schematic, changing headers here and there, and then switching back to the PCB editor again, going back and forth while iterating the design

SnapMagic/SnapEDA: downloading JST connector

SnapMagic/SnapEDA: Online electronic component libraries where we can download component symbols, PCB footprints, and 3D models and import to kicad.

Components and their symbols used:

Schematic Design

Designing the PCB in the PCB Editor

Don't even ask me how much time it took to figure out routing the tracks. At first, I was trying to route everything only on the top layer, which made it very difficult. Later, I placed the I2C pin on the bottom side to make routing easier.

The front layer (F.Cu) is the top copper layer of the PCB, where components and tracks can be placed. The bottom layer (B.Cu) is the bottom copper layer, where tracks can also be routed. Using both layers gives more space to route connections when the circuit becomes complex.

There was also another constraint while making this PCB: the board size. Our instructor initially said the board should be 48 mm x 70 mm. I tried resizing the sitar shape in inkscape to fit within that size. I also made a rectangle for the XIAO size (around 20 mm x 17.5 mm) to understand how much space it would take. Because the sitar shape is narrow, it was difficult to fit the components inside. Later, the instructor allowed the board to be slightly bigger, and the final board size became around 91 mm x 46 mm.

Drawing touch pads

To create the capacitive touch pads, I used the Draw Filled Zone tool (Ctrl + Shift + Z). I selected the F.Cu (Front Copper) layer because I wanted the touch pads on the top copper layer of the PCB.
After drawing a rectangular pad, I pressed B to refill the copper zone. Finally, I duplicated the pad using copy and paste to create a total of three touch pads.

2-side layer trace

Since my PCB is a 2-layer board, I routed traces on both the Front Copper (F.Cu) and Back Copper (B.Cu) layers.

• For routing, on the bottom layer press B.
• To adjust an existing trace without breaking its connections, use D (Drag)
• Use M (Move) to move objects freely

As all the components, including the Seeed Studio XIAO, were mounted and soldered on the front layer, the traces routed on the bottom layer had to be brought back to the front layer before connecting to the component pads. This was done by placing a via, which creates an drill hole , using copper wires/rivet create connection between the two copper layers during production. A via can be inserted by selecting Place Via, or while routing a track,pressing V to place a via and continue routing on the opposite layer.

DRC: Design Rules Check

While running the DRC, I found errors related to the via size and hole diameter. The default via dimensions were smaller than the board design rules, so I increased the via diameter to 1.4 mm and the hole size to 0.85 mm, which resolved the errors.

There was also errors with the Seeed Studio XIAO RP2040 footprint because its default pad hole diameter (0.8 mm) was smaller than the required 0.85 mm. I updated the pad hole diameter to 0.85 mm and circular pad diameter at 1.6 mm, and the DRC errors were cleared.

Board Boundary design in Inkscape

I used a reference image in Inkscape and converted it into a vector using the Trace Bitmap tool. After cleaning and editing the vector, I illustrated the bottom layer design using the Circle and Pen tools. Once the design was complete, I exported it as a DXF file for use in the CAD software. The bottom layer design shown here is my second iteration, as I redesigned it after an earlier version to improve the overall appearance and fit for production.

Import dxf to kicad

File >> Import >> Graphics >> Import Vector Graphics File: select the required dxf file and the layer.

3D viewer

this 3d model before changing the bottom vector design.

After changing the bottom vector design.

Gerber to PNG

In KiCad, Gerber files are used as the fabrication output files for PCB manufacturing. The Gerber and drill files generated from KiCad are used to create the toolpaths for milling the PCB traces and cutting the board.

To get the Gerber files, go to Fabrication Outputs >> Gerbers >> Plot(exporting or generating the PCB manufacturing files from design).

After plotting, Generate Drill Files to create the hole/drill data. Also it has option to choose the output folder if needed and then generate the files.

After generating the Gerber files in KiCad, the files were saved in a folder. These files were then converted to PNG using Gerber2PNG. (png file is used by the milling software to create the toolpath for cutting PCB traces and outline.)

All the generated files were uploaded to the website. By default it creates a single-sided PCB, but since my design is double-sided, I selected the double-sided option.

Then I clicked Generate All to create the PNG images. The generated PNG files can be previewed on the right side, and there is an option on the top to download all the images.

Later updates and improvement made:

This board was further improved in later assignments.