Even-though Kicad is quite intuitive and allows to start right away to draw schematics and then layout the PCB, at some point there will be an issue with the component libraries. Components might simply not be found in the libraries, Kicad might not find its libraries. Opening an old Kicad project with a new Kicad version might have library issues.

If no troubles appear then this section can be skipped. If troubles appear then this section might give the answer.

Kicad creates cache files containing a copy of the library components used in the design.

Kicad has a big evolution with its libraries. This caused some library incompatibilities..

The libraries are in /usr/share/kicad. Under Linux regular users do not have the permission to mess around in this directory. Create a custom libraries where frequently backups are made.

Recently the libraries can also be found on GitHub but since they move around on GitHub the default Kicad installation might have dangling links and not finding its libraries. As common with git the libraries from GitHub can be cloned as regular files and directories to the local computer and used from there as any other local library.

https://www.digikey.com/ created a GitHub kicad library https://github.com/digikey/digikey-kicad-library containing components from their stock.

Kicad can import eagle component libraries.

#
# 07-HEX-V
#
DEF 07-HEX-V S 0 40 Y Y 1 L 
<here comes the stuff that you better edit in the graphical editor>
ENDDEF

$Comp
L CONN_12X2 P14
<stuff where and how to put it on the page> 
$EndComp

$INDEX
HEX-V-Switch
LCD_20x4
<other footprints>
$EndINDEX
$MODULE LCD_20x4
<the footprint definition better to edit in the gui>
$EndMODULE  LCD_20x4

$MODULE pin_array_12x2
<everything seen on the board>
$EndMODULE  pin_array_12x2

From the KiCad main window EESchema (Schematic editor) opens the schematic editor and when saved, the *.sch file is created (plus some less important cache files). As with many drawing programs working with a grid is necessary, but often creates frustrating results when the components can not be placed onto the grid. Use as grid of the schematics 50mil, then check by clicking on the components that they use also a 50mil grid.

To verify that the wires connect, click on the components and drag them pressing the G key, so the wire will become a rubber band, when connected. However a weak point is that the wires can not be edited and can become ugly stretched. Select the wires and break them and delete not desired part or if it is really bad delete the complete wire. When moving instead (M key), the wires to the component will detach. With the R key you can rotate the component. The Insert key is also quite useful, it works as a repeat last command key.

Figure 2.1. KiCad schematics

Before proceeding further, some steps are required or strongly recommended:

First click on Schematic Annotation, so every component gets an unique name.

Multi-part components are components as the 7400 containing 4 identical gates (=units) that can be placed everywhere on the schematic page. During annotation those units are packeted into a single physical component. Also other components as relays make use of it this method, allowing to place the relays coil on a different location than the relays contacts. Selecting the component and do edit component > unit lets you switch between relays coil and contacts. IC's might have an extra unit that contains the power supply pins.

The Schematic Electric Rule Check will mark all connection points that are not connected. When placing components they need to be annotated otherwise they are like ghosts and it might be not possible to connect them with wires. The errors and warnings caused by the schematic electric rule check produce small arrows that can be clicked to see their reasons. The errors and warnings do not to be removed to proceed.

Some errors that usually pop up are:

Mounting holes appear also in the schematics, since they can be done using the 1pin footprint and then edit its parameters.

To create the net list using the schematic editor Netlist Generation, the *.net file is created.

There is a new way and an old way to go.

In the project window click on Cvpcb to link schematic components (*.lib files) to physical packages (foot prints *.mod or *.kicad_mod files). Click on Display the filtered footprint list for the current component, to make the list of available footprints smaller. For the components that have no footprint assigned (or where you like to change the default footprint, click on the desired footprint. To know what got selected click as well on View selected footprint. When done all is added to the Netlist and a *.cmp file is created listing all components.

There are many options to help making useful links:

Start PCBnew from the project window. Then browse netlist and load netlist. A *.brd file is created. Use the command move new modules to get them apart.

Figure 2.2. KiCad PCB

The PCB has different layers, not all layers are copper layers. Everything is a layer as the silk screen and soldering mask and what comes next the “Edges PCB” layer that defines the boards dimension to be drawn using graphic lines or a polygon. Since the board dimensions must be precise press the space bar to get the origin 0 for the relative coordinates shown on the status bar. The comment, drawings, ECO1 and ECO2 are layers for documentations as to show mechanical dimensions (e.g. drawing layer).

When placing the modules on the PCB, un-hide modules rats nest to see rubber bands attached to the module and get a feeling where it connects.

People write books about how to use the mouse. Mostly it is intuitive, but certain things not, therefore here, the how to use the mouse:

Click and release, then move the line, click and release to extend the line.

Press space to set the origin from where the relative distances to the cursor are measured.

To change track width, just modify the default value, the list of track widths will expand.

For mounting holes add the "1pin" footprint, then edit the pad in order to have the correct size (pad diameter and drill value). To have it consistent with the schematic the CONN_1 could be added to the schematics. This gives a plated hole.

Selecting with the mouse a module and use the keystrokes M for move and R for rotate prevent the numerous mouse clicks using the menu. The + and – key select different copper layers. You need to get familiar with different track edit operations, read the manual for that (deleting segments, Backspace key to undo last click, brake track and move via, brake track and move node … ).

When you are done you deserve a 3D view of the result.

If you create a board with more than 2 layers, it might happen that some modules are just for 2 layer, if creating zones, then those holes are not present and causing DRC errors, also it is not possible to wire up inner layer to them. In such cases edit the module. Go to edit pads global, check if the dimensions are ok (pad size 0.056” drill 0.036”), then click on change module and save it to the board.

Figure 2.3. KiCad 3D

If your preferred PCB manufacturer supports kicad then you can send directly the kicad files. If not then Gerber data has to be produced.

Nowadays the manufacturing process usually will not use films anymore that have to be manually placed onto the board to be exposed to light, so there is no need to add fiducial marks, alignment marks and dimensions to the design. For some manufacturers those stuff outside of the board might even disturb and cause additional work or maybe you get a larger board with a higher price, where you have to cut those things off. It is enough to submit the data in an electronically form. However make sure to not to exclude the PCB-Edges layer when creating the board, since this layer defines the outline.

Figure 2.4. kiCad drill

To create Gerber data, just plot the board to Gerber format. For each selected layer a separate file is produced (*.pho). Consider also to generate the drill file (*.drl) that contains all diameters of the holes. Otherwise you might end up drilling the holes your self!

With Gerber data it is simply a must to use a Gerber viewer. KiCad includes a Gerber viewer to verify it. However it is still not guaranteed that you get what you expected, since Gerber files depend on a tool set (aperture and drill tables). Last but not least every layer is usually a file and you could end up having the bottom layer as top layer, so for surface mount components the PCB would be useless. So a Gerber viewer that can pack everything together in a single file that is understand by the PCB manufacturer verified by yourself is the way to go.

To be safe, check with your PCB manufacturer, if it supports a viewer project file that puts everything together. As example:

A PCB producer services that will not be scared when ordering little quantities is:

http://www.pcb-pool.com/. The Gerber data can be submitted using GC-prevue down-loadable for free of charge on their site (so is KiCad).

The original place of GC-prevue is: http://www.graphicode.com/

Figure 2.5. GCprevue

The *.gwk file can be uploaded to get the PCB. Only drawback, GC-prevue is not a Linux application. However GC-prevue can be installed under Linux using wine. After installing it do a:

cd ~/.wine/drive_c/GCPREVUE followed by:

wine gcprevue.exe to have it running. Don't forget to copy your Gerber data and drill file somewhere under ~/.wine/drive_c or better make a link from ~/.wine/drive_c to where the kicad data is, so it is in reach of wine. To not confuse the manufacturer, rename and order the layers for a 2 layer board as follows:

The layers can be imported and the GC-prevue is able to detect automatically what it is. Importing the drill gets probably errors. So do not load the drill automatically, load as drill and a window with options pops up. Check KiCads export options if they are different from its defaults and adjust them to the GC-prevue's Load Drill data window. Additionally you need to manually create the drill diameter table in GC-prevue. Therefore create and open the KiCad Drill report file.

Figure 2.6. Drill data

To have the layers end up in GC-prevue's window, you need also to set an offset (x-offset 1” y-offset 10”) you can do it either under edit or when loading the layers.

Then you can observe the result an when happy save all to get a a *.gwk file to be e-mailed to the PCB manufacturer. Restore all will read *gwk files at later stage.

Check limits of the PCB manufacturer and set the PCB Design Rule Checks accordingly. This should be the first thing when you do a PCB, but putting it right at the beginning would complicate the stuff unnecessary, since most PCB manufacturers can work with the KiCad default rules.

To have nice drawings that are even in 1to1 scale do a plot to postscript first. Then using something as kgostview or gsview to convert it to pdf.

Plot silkscreen on component layer to get an assembly drawing. If the drawings are big as A2 print them first in a A2 pdf and then print them again to shrink.

Or print to SVG and open it using inkscape and convert there to PDF or print from there.

There is no renaming project command in KiCad but it can be done manually thanks to have the KiCad files as Ascii. Rename the pro, brd, sch, lib, cmp, mod files and then open pro, sch, in an Ascii editor and make search old name replace with new name.

emerge -pv =sci-electronics/kicad-meta-5.1.12 and add the following to /etc/portage/package.accept_keywords

=sci-electronics/kicad-meta-5.1.12 ~amd64
=sci-electronics/kicad-5.1.12 ~amd64
=sci-electronics/kicad-symbols-5.1.12 ~amd64
=sci-electronics/kicad-footprints-5.1.12 ~amd64
=sci-electronics/kicad-packages3d-5.1.12 ~amd64
=sci-electronics/kicad-templates-5.1.12 ~amd64
=sci-electronics/kicad-i18n-5.1.12 ~amd64