Version 9 (modified by Eric Hazen, 9 months ago) (diff)


Up to KiCAD Notes

Table of Contents

Starting a new layout in KiCAD 5:

Board Setup

Select the "in" icon at the top left to switch the units to inches.

Click the "Board Setup" Icon under the word "Edit" in Pcbnew

  1. Start with Layers. Set the number of copper layers (usually 2 or 4)
  1. Select Design Rules and fill in as below

  1. Select Layers->Text & Graphics.

Set it something like the example below:

  1. Select Design Rules->Net Classes

  1. Select Design Rules->Tracks & Vias

This depends a bit on the design, but the selection below is a good start.

Component Placement

Please use a grid when placing components. There are a few exceptions.

When you start a layout, you should decide if the grids will in general be in mm (metric) or inch (imperial/English) units. We prefer inches here in the USA.

When placing parts, follow these rules, in order of priority:

  1. Place components with known locations (e.g. connectors where you are given an exact location from a mechanical drawing). This is rare.
  1. Set the grid to 0.1" (100 mils) and place "large" components. Generally this includes connectors and any component with one dimension larger than about 0.5" (500 mils). Do your best to plan a logical signal flow when placing parts. Align similar components vertically and horizontally in neat rows if there is no other consideration.
  1. Set the grid to 0.025 (25 mils) and place smaller components. This would include anything down to about an 0805 or maybe 0603 passive or things of similar size. Place smaller components so as to minimize trace length and crossings. Again, align similar components in rows and columns where possible.
  1. Finally, for "tiny" parts (0402) you can use an 0.005" (5 mil) grid, but be careful to align parts relative to each other vertically and horizontally.

Some other general considerations:

  • Think about power and ground connections. If you are doing a two-layer board, you need to consider this carefully so that the ground in particular can be well-connected, either with traces or a copper area.
  • For ICs and connectors, locate pin 1 consistently (e.g. in upper left). For passives (R's and C's) this is less important, and they should be rotated to minimize trace crossing and length.
  • Leave some space between components for routing.
  • Don't place components closer than 0.05" (50 mils) from the board edge in general.
  • Always place filter/bypass capacitors near power pins on ICs
  • Leave the corners of the board free for mounting holes

Trace Routing

This is a complex topic which cannot be summarized easily, but here are some general guidelines:

  • Decide on the number of layers. For simple boards, this should be 2 (top/bottom only). Discuss with an engineer. This determines whether a board is "two layer" or "multilayer".
  • Choose a minimum trace width. If you set up the design rules according to the suggestions in this guide, the minimum width would be 0.007" (7 mils). This is reasonable for signal traces. On a low-density board, 0.012" (12 mils) is a more conservative choice.
  • Choose a routing grid. If you are given no other information, start with a grid of 0.025" (25 mils).

Power Supply Routing for Two Layer boards

  • A reasonable plan for low-density boards is to use filled areas for ground (and potentially power). You don't need to do this before you start routing, but keep in mind that you have to leave some clear space around ground pins for the filled area to connect.
  • Route short traces from power supply pins to the nearest bypass capacitor. Use a trace which is slightly narrower than the component pads for SMT parts, or 25-50 mils for through-hole parts.
  • If there are a small number (maybe up to 3) different power supplies and you can place the components to separate them into contiguous areas, you can potentially use filled areas for power as well.
  • If you aren't using filled areas for power, route wider traces from the power supplies (voltage regulators or input connector) to the power bypass capacitors. If the overall current is reasonably high, use vias larger than the smallest size (maybe 60 mil via with 25 mil hole) for power traces. Discuss with an engineer

Power Supply Routing for Multi-Layer boards

For a multi-layer board (4 or more layers) usually one inner layer is ground, and the other(s) are for power supplies. You will need to place fill areas on the power and ground layers, and place vias to make connections to these layers for SMT parts. If you have only one power layer and multiple power supplies, you need to divide up the power layer into multiple filled areas to cover all the power pins. You can also route traces on the signal layers if needed to deliver power.

General Routing Strategies

  • Choose preferred layer directions for routing: one layer for "vertical" and one layer for "horizontal"
  • Route all traces which are not trivially short as horizontal and vertical segments with vias (you can remove extra vias later). When you start to work in congested areas you will see why this is a good idea.
  • Remember that for SMT (surface-mount) parts that if you want to make a connection to a different layer from the one the part is on that you need a via for each connection. Never put vias through component pads or touching them; always route a short trace and then place the via. (there are exceptions like thermal vias, but an engineer will tell you if these are needed).