1 files changed, 152 insertions, 0 deletions
diff --git a/tools/quality/elec/pcb.txt b/tools/quality/elec/pcb.txt
new file mode 100644
@@ -0,0 +1,152 @@
+ Printed Circuit Board Design
+This document should gather any useful information for PCB _ design at APBTeam.
+..  Printed Circuit Board
+The software used currently for any PCB is Eagle from CadSoft. CadSoft
+distributes a freeware version running under Linux or MS Windows for
+non-profit usage, limited by the PCB size and the number of usable layers.
+In the future, we may switch to a free software solution: KiCad. But Eagle
+offers several advantages: all previously designed libraries and boards were
+using Eagle and Olimex takes directly Eagle files.
+Our boards should be suitable to be manufactured by Olimex, a low-cost
+prototype board manufacturer. They make double sided Europe size boards for
+about 30 euros, with solder mask, metallised holes and one silk screen.
+Most boards are a division of a Europe format board. Europe is 10x16cm, 1/2
+Europe is 8x10cm and 1/4 Europe is 5x8cm. Actually, a margin must be
+subtracted for panelization.
+Some components have a standard position. This include mounting holes and
+- mounting holes: MOUNT-HOLE3.3 in the holes library:
+ - at (0.15 0.15) and (0.15 2.925) for 1/4 Europe,
+ - at (0.15 0.15), (0.15 2.925), (3.65 0.15) and (3.65 2.925) for 1/2 Europe.
+For exact dimensions and positions, please see the asserv board for 1/4 Europe
+and the puiss board for 1/2 Europe.
+Here is the list of used connectors:
+- HE10 for signals, usually 10 pins
+- HE10, 6 pins for I2C
+- pin heads for servomotors
+- HE14 (TBC) for miscellaneous sensors and low pin number signals
+- HE14 (TBC) for digital board power
+- Phoenix 381 connectors for power connections
+- Micromatch SMD connectors for small size connections
+As a rule of thumb, use the pin number 1 for ground and pin number 2 for
+For board manufactured at Olimex use their DRC file for auto-routing and
+Design Rules Check!
+As the same errors occurs again and again, here is a list of items you should
+check when you design a PCB:
+ Are all the components powered? Is there a power connector?
+ Use decoupling capacitors on the power and near each components.
+ Capacitors should be the nearest possible of the components. Do not put
+ to much decoupling or the board will drain to much current when switched
+ Check text size in order to be able to read it. For Olimex: vectorial
+ font, 70 mils, 15%.
+Text on each layer
+ There should be text on each circuit layer (top and bottom). This makes
+ it easy to known if the layer is in the right direction. This is also a
+ Olimex requirement.
+ Has the board the right size? Is there extra margin for panelization?
+ Check holes types and positions.
+ Are the connector near enough of the board edge? Some connectors, like
+ Phoenix ones, use space lower than the board, if the connector is to far
+ from the edge, it will not be possible to plug it.
+ Are they at the right position ?
+ Use the largest possible tracks. Use larger tracks for power. For high
+ power tracks, the solder mask can be removed on a particular region.
+ Are the components on the right side? This is particularly hard to see
+ for through hole mounted components.
+ Check than no component override each other. Check that it is possible to
+ solder them without a master level of dexterity.
+ For board without metallised holes, use restrict layer to forbid
+ connection where soldering would be very hard (for example, it is not a
+ nice thing to try to solder a track going under a HE10 connector).
+ Always place component on the grid.
+ Check that all components are available with the right size and package.
+ This is particularly true for capacitors.
+ Double check pinout! Should TX and RX be inverted? This one is for you
+ Use pull-up or down resistors or shorts-protection resistors.
+ Use them to separate command and power.
+ERC and DRC
+ Use Eagle tools to check the board. For boards manufactured by Olimex,
+ use the file they provide for DRC.
+ Limit the use of different drill size and use standard drill size. This
+ increase the board cost. Be careful, the metalization will reduce the
+ hole size!
+ Prefer auto-routing as this is easier to make modifications.
+ Print useful information on it. Do not forget to run the Olimex provided
+ script to fix it right before sending file to them, but do not save the
+ result in the repository as this make editing harder.