Tutorials

• ​https://forum.kicad.info/t/tutorial-introduction-to-pcb-design-with-kicad-version-5-1-getting-started/20600
• KiCAD5SchematicTips - getting started with schematics in KiCAD 5 (Eric's notes)
• KiCAD5SchematicToLayout - moving from schematic to layout (Eric's notes)
• KiCAD5LayoutTips - getting started with layout in KiCAD 5 (Eric's notes)

Other Random Notes

No Global Symbols/Footprints

If you find that you don't have global symbols/footprints available or you get the dreaded "rescue" dialog, you probably didn't allow KiCAD to create the default library paths the first time you ran it. To fix this (on Linux):

  $ cd .config/kicad
  $ mv fp-lib-table fp-lib-table-save
  $ mv sym-lib-table sym-lib-table-save

Now start KiCAD and select Preferences->Manage Symbol Libraries. A dialog box will pop up offering to create the default paths. Leave that selected and click OK twice.

Same thing for Preferences->Manage Footprint Libraries.

Buses

Buses are groups of signals. See ​https://www.baldengineer.com/kicad-bus-labels-and-global-labels.html

Here are a few observations:

• On a sheet, a bus (heavy blue line) must be named as e.g. name[0..3]. The order doesn't seem to matter.
• If the groups of signals have different net labels e.g. (A_0,A_1...A_n) and (B_0,B_1...B_n), then the bus connecting them needs to have both those net labels assigned (A_[0..n] and B_[0..n] respectively). If the groups of signals have the same net labels for the wires, assigning the bus a net label is not necessary.
• Buses can be used to connect different groups of signals directly as well as with hierarchical pins and global labels. Buses can be connected between sheets in a similar manner to normal (Green) wires.

Cut/Paste between schematics (KiCAD 5)

Open schematic editor from shell (type eeschema). Then you can open one schematic, copy a block, open another schematic and paste. The claim is that in KiCAD 6 everything is re-done and re-broken and this will be different :(

"Append Schematic Sheet Content" can also be used to copy a whole schematic onto the sheet. Go to File > Append Schematic Sheet Content and select the schematic file that needs to be copied.

Bill of Materials (KiCAD 5.1.10)

Be sure you have xsltproc installed.

Just click the "BOM$" icon on the schematic. If there are no plugins installed, click the "+" icon and navigate to /usr/share/kicad/plugins and add the bom2csv.xsl and bom2csv-grouped.xsl plugins. They work fine "out of the box" in my experience.

On the schematic, set the properties on each symbol as follows. Use Tools->Edit Symbol Fields for editing of all symbols on a schematic in a spreadsheet-like way.

Below is a suggested convention for the fields to produce a useful BOM.

Field Name	Use	Example	Notes
Reference	Part Reference	C1	Required on all symbols, usually automatic
Value	Passive Value	33UF 350V	Required on all symbols
	or part number	DMN2004DMK, 74LS04
Footprint	-filled in automatically-
Datasheet	URL of data sheet if available		Useful but not required
CatNo	Catalog Number	493-12996-1-ND	Either CatNo or MfgNo required for BOM
Vendor	Supplier Name	Digi-Key	Useful but not required
Mfgr	Manufacturer	Nichicon	Useful but not required
MfgNo	Manufacturer P/N	UVY2V330MHD1TO	See above

Note that you will have to add various fields by hand. Usually Reference, Value and CatNo or MfgNo are visible and the others are hidden. This is up to you to set correctly.

Solder mask pull-back

To adjust the pullback of the solder-mask, open pcbnew and go to "Dimensions" pull-down and select "Pads Mask Clearance". Then you can change the pullback around pads for when the gerbers are generated. (Helpful hint: Cirexx likes 40 mils (0.004"))