An Intro to KiCad – Part 4: Create a Footprint | DigiKey

Creating Custom Footprints in KiCad

Introduction to Footprint Creation

• The process begins after drawing a schematic in Eeschema, where the next step is associating schematic symbols with footprints.

• If a footprint for a component like the 7555 timer is unavailable, creating a custom footprint is necessary before proceeding to layout.

Finding Component Data Sheets

• To find the data sheet for the 7555 timer, visit digikey.com and search for "7555."

• Carefully review categories in search results; select "Clock/Timing, Programming Timers and Oscillators" as it aligns with your needs.

Filtering Search Results

• Apply filters such as "Through Hole" to narrow down options from nine parts to three that are currently in stock.

• Sort results by descending quantity available to identify popular components; Intersil's 7555 timer appears favorable due to its stock and price.

Accessing Data Sheets

• Click on the part name to access its page and locate the data sheet link; some sheets provide footprint dimensions while others may not.

• For common packages like DIP, dimensions can be assumed standard based on pin count; sufficient information exists here to start creating a footprint.

Creating a New Footprint

• Open KiCad's Footprint Editor via Tools > Run Footprint Editor and create a new footprint by selecting File > New Footprint.

• Consider IPC standards for naming footprints but opt for simpler names like ICM7555-PDIP for ease of use in small projects.

Saving Your Custom Library

• Save your new footprint into a unique library by selecting File > Save Footprint in New Library, ensuring it points to your project directory.

• Manage libraries through Preferences > Footprint Libraries Manager; append your new library using Append with Wizard.

Setting Active Libraries

• Choose whether the library will be usable across all projects or just locally; it's recommended to keep it local unless curating an extensive library.

• Set your active library by navigating through File > Set Active Library and confirming selection of your newly created library.

Understanding Units in PCB Layout

• Be aware that PCB layouts may use different units (millimeters vs. inches); many manufacturers prefer imperial measurements.

Footprint Creation in Ki-Cad

Setting Up the Footprint Editor

• The Footprint Editor should be set to inches; users can switch to metric by selecting the millimeter button. A grid setup of 10 mils is recommended for easier movement of components.

Moving Components and Establishing Origin

• To reposition parts, hover over the part name and press the M key. It's advisable to center the origin for easier placement and rotation during layout.

Drawing Component Body and Pin Orientation

• For an eight lead PDIP package, a top-down view representation is drawn, marking pin locations with a plus symbol at the origin. An orientation marker indicates pin one.

Understanding Dimensions from Data Sheets

• Ki-Cad's coordinate system has positive X to the right and positive Y downwards. The distance between pins on one side is 0.1 inches, leading to calculated coordinates for each pin based on data sheet specifications.

Calculating Hole Sizes and Component Body Reference

• Maximum pin width is 22 mils; thus, a hole size of 30 mils is deemed sufficient. The longest component part measures 0.4 inches while the widest measures 0.28 inches, guiding dimensions for layout.

Creating Pads in Footprint Editor

Placing Initial Pad

• In the Footprint Editor, select "Place" then "Pad" to add a pad at specified coordinates (-0.15, +0.15). Ensure drill size is set to 0.03 inches with an annular ring width of 0.015 inches.

Duplicating Pads for Additional Pins

• To create additional pads, duplicate existing ones by right-clicking or using Control + D shortcut keys while adjusting their coordinates accordingly (e.g., pad two at (-0.05, +0.15)).

Completing Pin Layout

• Continue placing pads following DIP numbering conventions: pins are numbered in a U-shape starting from pin one near the cutout notch through eight across rows.

Drawing Component Outline

Outlining on Fabrication Layer

• Draw an outline of the component body on the top fabrication layer for visual reference against other components and future silkscreen outlines; this aids in board population clarity during assembly processes.

Footprint Design in Ki-Cad

Setting Up the Initial Coordinates

• Begin by establishing coordinates for X and Y: 0.2 for X and 0.14 for Y, maintaining the starting X value to draw a vertical line.

• Adjust the end Y coordinate to -0.14 by flipping its sign, and set the line thickness to 0.004, which is typically between two and ten mils.

• Change the layer to F.Fab (front fabrication), noting that "top layer" refers to this same front layer in Ki-Cad.

Duplicating Lines and Adjusting Properties

• Duplicate the initial line, moving it left of the pins; ensure it starts at (-0.2, 0.14) and ends at (-0.2, -0.14).

• Create another horizontal line connecting previous lines' bottoms with coordinates (0.2, 0.14), flipping X to -0.2 while keeping Y constant.

Adding Orientation Indicators

• To indicate part orientation due to a notch on the DIP package, place a semi-circle arc on the left side of the part outline using Place > Arc on F.Fab layer.

• Start drawing at negative coordinates (-0.2, 0), placing temporary markers as needed while ensuring absolute coordinates are used when entering values manually.

Finalizing Arc Properties

• Draw an arc from (-0.2, 0) to (-0.2, -0.05); edit properties afterward to set an angle of 180 degrees (1,800 units of 0.1 degrees).

• Match arc thickness with other lines at 0.004; this creates a clear notch representation in your part outline.

Incorporating Silkscreen Elements

• In Footprint Editor, add graphic lines on F.SilkS layer for silkscreen design; avoid pin areas but outline other sides of the part.

• Edit silkscreen line width to be slightly larger than fabrication lines (set width to 0.008).

Enhancing Part Identification

• Duplicate silkscreen lines as necessary for clarity; consider adding indicators like circles near pin one for easier identification during assembly or debugging.

• Instead of copying arcs directly onto silkscreen layers (which may not be visible post-placement), create small circles marking pin one’s location.

Organizing Reference Designators

• Position reference designator above footprint centered along Y-axis; move part name below footprint also centered along Y-axis.

• Note that REF** will automatically update based on associated schematic symbols later in Ki-Cad workflow.

Saving Your Work

• Save your completed footprint in Active Library via File > Save Footprint; alternatively load existing footprints from Digi-Key libraries if needed.

This structured approach provides a comprehensive overview of designing footprints within Ki-Cad while emphasizing key steps and considerations throughout the process.

Footprint Editor Overview

Exploring SMD Footprints

• The speaker suggests opening a SOIC footprint to examine a well-designed SMD footprint, emphasizing its quality and structure.

• For those creating similar designs, starting from an existing footprint can simplify the process; modifications can be made as needed.

• After making changes, users are encouraged to save their work into a new library or their current active library for future use.

• The session does not involve editing at this moment; instead, the focus is on understanding the utility of existing footprints.