KiCad

From RepRapWiki
Jump to: navigation, search

Contents

KiCad

RepRap is using KiCad for electronic design. The KiCad homepage is http://www.kicad-pcb.org/ .

KiCad is an open source (GPL) software for the creation of electronic schematic diagrams and printed circuit board artwork. Users are making complex boards with it, as boards of 4 layers or more, with ARM microcontrollers running at 450MHz.

See Useful Software Packages#CAD software for electronics for comparisons with other software for electronics.

Installation

Installation instructions for GNU/Linux are here. Windows installation should be fairly easy.


We highly recommend that you read a tutorial in the KiCad website. They also have very good documentation in Open Office format included with the installation. This will solve many of your questions.

General Kicad Tips

You do 95% of your work with right click. Remember that and you'll be fine.

PCBNew

Setting Defaults
First, you'll want to be in inches as your unit. Thats what most board houses operate on and is the easiest. Most measurements are in mil which is .001 inches. It has nothing to do with millimeters. One exception to this rule is any sort of mechanical mounting (like the mounting holes on a PCB). Those should be on a metric grid to interface more easily with the rest of RepRap. Kicad flips between imperial and metric with a single button click; you may want to set a User Grid size to suit what you want.

Most manufacturers have minimum trace size and minimum spacing requirements. Find these out and then enter them into Kicad. A safe bet is a minimum of 10 mil traces and 10 mil spacing. Enter these in the Dimensions -> Tracks and Via's menu. The fields are track width and clearance. For a board you're etching at home, crank those numbers up.

Next, you'll want to set your grid size to 10 mil. Its a size with good detail, but allows you pretty fine control.

Preparing Board For Manufacture
Getting boards made at a PCB shop is the easiest way to get a board done, however its somewhat expensive for small runs and you only have one chance to get it right. For prototype boards, we have been using batchpcb.com. They are reliable, fastish and support the Maker community. To prepare your board for them you have to follow the steps above (they have an 8mil track and 8mil clearance minima). If you want to make your own prototype boards we have instructions here.

First, you need to get your board laid out. Once you have it how you want it, make sure it passes both the DRC check and the Connected test. Your board must pass both of those to work. Additionally, there are some design guidelines that will help ensure that your board is ready to go the first time and will pass the manufacturers DRC also.

Adding Ground Planes / Zone Fills
Now, you can add zones to your board. Click the zone tool, then find your ground path on the board. Right click it and choose 'Select Net'. This will make the traces part of the zone. Right click and choose 'Fill Zone'. You will want to use these values:

  • Grid: 0.01 minimum. 0.005 is too small.
  • Pad options: include pads. or thermal, depending on taste
  • Zone clearance value: 0.05. actually, .04 - .06 are acceptable
  • Zone edges: any

Adding Board Text
After you've added your fill, you'll probably want to add some text. At a bare minimum, we add www.RepRap.org or RepRap.org and also the board name and version: My Board v2.3 Use the text tool, and add it to either the SilkS Cmp or SilkS Cop layers. These are the silkscreen layers, so you can put your text wherever there are no components and not have to worry about wires.

Generating GERBER Files
Most professional board houses need GERBER files to produce your board. Kicad can easily generate theses, and also has a nice viewer that will allow you to double check that your board looks right. To generate them, click the Plot icon which pulls up the plot screen. You'll want to use the following options:

Layers

  • Copper
  • Component
  • SilkS Cmp
  • Mask Copp
  • Mask Cmp

Other Settings

  • Leave the print $foo settings alone... most should be on and defaults are fine
  • Plot format: GERBER
  • Plot origin: absolute
  • Spot min: 0.015 (default)
  • Lines Width: 0.001 (default)

Click Save Options so you dont have to re-do it, and then click Plot. It will create .pho files in your board directory which are your GERBER files. You will need to send these to your manufacturer. Feel free to open them with the gerbview program Kicad provides. They look cool =)

Generating Drill Files
Bring up the Plot dialog again. This time, you will want to click the Create Drill File option. This will bring up another dialog. The settings in this dialog are very important. You will want to use:

  • Units: inches
  • Zeros Format: suppress trailing zeros
  • Precision: 2.4
  • Drill origin: absolute
  • Drill sheet: none
  • Via drill: .025 (default)
  • Mirror Y axis: off
  • Minimal header: on

Then click the execute button. Your drill file will be created. It will have the extension .drl Its a text file, so feel free to take a look at it and marvel at the wonder of automation.

Congratulations, you just prepared your board for manufacture! Generally you will create a zip file with the .pho and .drl files and send that off to the manufacturer. batchpcb.com has a great web tool that will run DRC checks and report any errors back to you. It is very handy indeed.

Further reading