Kicad - from schematic to production
Collected resources covering the use of Kicad for both DIY printed circuit board [PCB] production and prototype ordering from manufacturers.
Table of Contents
workflow:
Moving between schematic and pcb.
Loosely following excellent tutorial at:
http://www.kicadlib.org/Fichiers/KiCad\_Tutorial.pdf
as referenced from:
1] schematic view: eeschema
Use of EESchema to construct/edit schematic is simple enough. remember to annotate schematic - use schematic annotation icon in top bar and select annotate - this gives all components unique identifiers. then use generate netlist icon and save netlist.
Making and connecting buses
From Kicad online help:
In fact, due to the repetition command (Insert key), connections can be very quickly made in the following way, if component pins are aligned in increasing order (a common case in practice on components such as memories, microprocessors…):
Place the first label (for example PCA0)
Use the repetition command as much as needed to place members.
EESchema will automatically create the next labels (PCA1, PCA2…) vertically aligned, theoretically on the position of the other pins.
Draw the wire under the first label. Then use the repetition command to place the other wires under the labels.
If needed, place the bus entries by the same way (Place the first entry, then use the repetition command).
Which boils down to:
- Add bus [right hand bus icon]
- Add label (right hand icon)
- Insert to repeat/edit if needed
- Make first wire to bring pin close to bus
- Insert to repeat
- Add wire to bus entry (wires are purely aesthetic)
to copy and paste from one schematic to other
- select block, right click, other block commands, save block
- open next schematic - from toolbar of icons select paste
2] attach footprints: cvpcb
Schematic modules have to be associated with physical representation/footprints - run Cvpcb from icons.
We have a list of parts and we need to associate these with scrolling left hand list of footprints (double click on appropriate footproint when we have component selected). save this new netlist
3] placing and routing: pcbnew
we need to set paper size from icon and dimensions of tracks and the like from top menu item. Click read netlist button, select approrpiate list and hit read. options for ratnesting are specified in the tutorial - move modules into centre of sheet and manipulate (move, rotate) until number of crossing points is reduced. autoroute functionality appears missing as we do not have the anneal code (?). route by hand using right add tracks icon. for smd we are working on component level. to print use accurate scale 1 option.
notes
1] In Pcbnew app now we need to fix on trace sizes for non_SMT/D parts:
0.8mm track
0.8mm via drill
0.2mm clearance (or thicker 0.035inch tracks)
We set this in: Top menu: Dimensions. Then Tracks and Vias.
2] Set page-size when we start to A4 under: Top toolbar - page settings icon
3] We needed to add a module which wasn't in the netlist/schematic - it was easy to add using right hand add-module-icon but adding a track wouldn't work - to do this we needed to turn off DRC in Top menu: Preferences and the General Options (or use left hand top icon)
4] We follow tutorial instructions for fill - use right hand zones icon, trace round board size and then right click and fill but it ignores our new tracks (see 3]): (as a compromise we can use the Fill Zone include pads option which leaves the centre free)
shortcuts
PgUp and PgDn or Shift V to switch component/copper side when laying tracks and vias (to place via start on component side, drag track, right click to place via and then track continues on copper side)
F1 zoom in
F2 zoom out
F3 redraw (across also all kicad apps)
F4 centre at cursor
and further see also: http://xtronics.com/reference/kicad.html
4] pre-production checklist:
check clearances:
\includegraphics[width=34em]{/root/Wiki/images/kicad_clear.png}
Clearance/track width: 0.008 inch (0.01 inch for home production)
Drill: 0.016
check power and GND connections
run DRC (design rules check)
\includegraphics[width=34em]{/root/Wiki/images/kicad_drc.png}
check soldermask exists on both sides for through hole parts
Edit pad, check Solder mask copper:
\includegraphics[width=34em]{/root/Wiki/images/kicad_mask.png}
check GND planes on both sides
check any parts which should have no copper beneath
eg. uSD card holder
gerbv test that all layers match:
plot first:
\includegraphics[width=34em]{/root/Wiki/images/kicad_plot.png}
and generate drill file:
\includegraphics[width=34em]{/root/Wiki/images/kicad_drill.png}
[suppress leading zeroes?]
then use gerbv (apt-get install gerbv) as follows:
gerbv new_mini2-Copper.pho new_mini2-Component.pho new_mini2-MaskCmp.pho new_mini2-MaskCop.pho new_mini2-SilkSCmp.pho new_mini2.drl
\includegraphics[width=34em]{/root/Wiki/images/gerbv.png}
5] home/DIY production guide:
Using Eisen III Cloride: http://www.1010.co.uk/simple\_pcb\_guide.html
Notes for photo-etch and Natriumpersulphat:
http://www.1010.co.uk/pcb.html
6.30 to 7 minutes with standard foggy tracing paper (gives greater timing control).
6] PCB manufacture:
Using pcbcart or batchpcb:
For multiple prototypes (black silk on black mask): http://www.pcbcart.com/
For lower runs, slower (cutting of irregular outlines): http://www.batchpcb.com/
checklist:
as above more or less
produce Gerber and drill files:
specification:
- panelling: what is tab route and what is V-scoring?
from: http://www.4pcb.com/pcb-faqs-manufacturing-technical/
What is tab route? A tab route is used to create arrays, often called "route and retain". The customer can place more than one board (same or different design) up in a given area in an array or panelized configuration. This is typically for the convenience of the customer or for assembly requirements that utilize pick and place machines to load components. The PCB's are then separated by breaking or cutting the tabs. Tabs are usually 0.100" in width and are placed with at least 1 on each side of the boards.
What does "scoring" mean? This is a "v" groove cut into the top and bottom surface of an array of multiple PCB's or between a board and rails to be removed after assembly. The cut is usually 1/3 top, 1/3 bottom, leaving 1/3 uncut in the middle. This process is used when removing the tabs of a tab route is not a viable option, this does result in a less smooth finished board edge. The boards are typically set up side by side and end to end with the edges adjacent to each other. After assembly the boards are broken or snapped apart.
7] Misc Notes:
Image2Kicad
To convert images to, for example, silkscreen. From:
http://www.mige.altervista.org/index.php?mod=Download/Kicad\_Utility
[within TTconv package]
Use:
Free PCB file check (DFM):
Date: 2011-04-29 18:27:15 BST
HTML generated by org-mode 6.31trans in emacs 23