Here are some points mentioned during the tutorial.
To obtain an Altium Designer license for use on your computer, please check the official Altium at EPFL page.
You can download a cheatsheet with the most useful keyboard shortcuts.
You can download the DXPSymbols.ttf font, which contains the EPFL logo and some other potentially useful symbols to use on PCBs. The EPFL logo (required by the ACI when producing printed circuits) corresponds to the E character.
Altium Designer libraries
A collection of libraries is installed on the computers available in MEB 494 on C:\Users\Public\Documents\Altium\Library (see here for the source files). They are relatively old and don't feature the most recent components, however they provide a very useful collection of standard PCB footprints. For up-to-date component libraries, check the Unified Components page on Altium web site (account required for download).
The standard IPC footprints for discrete SMD components could be found here:
- Pcb\IPC-7350 Series\IPC-7352 Discrete\IPC-7352 Chip_Resistor_N.PcbLib
- Pcb\IPC-7350 Series\IPC-7352 Discrete\IPC-7352 Chip_Capacitor_N.PcbLib
- Pcb\IPC-7350 Series\IPC-7352 Discrete\IPC-7352 Chip_Inductor_N.PcbLib
The sizes are indicated in metric dimensions; on components these sizes are often indicated in fraction of inches. Here is a short conversion table (the commonly used sizes for hand-soldered boards are indicated in bold):
|01005||0402||0.4 × 0.2 mm|
|0201||0603||0.6 × 0.3 mm|
|0402||1005||1.0 × 0.5 mm|
|0603||1608||1.6 × 0.8 mm|
|0805||2012||2.0 × 1.25 mm|
|1008||2520||2.5 × 2.0 mm|
|1206||3216||3.2 × 1.6 mm|
|1210||3225||3.2 × 2.5 mm|
|1806||4516||4.5 × 1.6 mm|
|1812||4532||4.5 × 3.2 mm|
|2010||5025||5.0 × 2.5 mm|
|2512||6432||6.4 × 3.2 mm|
A file with the definition of DRC rules for use in Altium Designer could be downloaded here: ACI.rul. To import it in Altium Designer: click on Rules in the Design menu, then right click in the rules list and select Import Rules.... Make sure you select all rules in the window that appears (you can click any of them and then press Ctrl+A to select all). Then specify the file to import, and answer Yes when asked if you want to erase the existing rules.
You can download a schematic template for Altium, with EPFL logo and place for document title, author, etc. Those parameters can be modified in the Document parameters window.
Exporting data for production
The PCB workshop (ACI), as many other PCB manufacturers, accepts Gerber files (Extended Gerber, RS-274X) as source data for PCB production.
Gerber files can be exported from Altium Designer (in the File menu, select Fabrication outputs then Gerber Files). The required layers are Top Layer and Bottom Layer (copper layers), Top Solder and Bottom Solder (if you want a soldermask, which is generally a good idea), and Mechanical 1 (external contour milling of the PCB and internal milling if needed). Make sure you do not check any mechanical layer in the list of layers to be included on all copper layers.
For the drilling files, you have to export them by choosing NC Drill Files under Fabrication Outputs. Make sure you select the right file format for the drill file (the standard values in the ACI order form are Millimeters, 4:3, Suppress Leading Zeroes, Reference to absolute origin). The generated TXT file is the one to be submitted.
To generate the 1:1 PDF file, you can simply print out the PCB to a PDF (using the Print function, after setting the print scale to 1 in the Page Setup window).
The ACI order form is here: https://aci-commandes.epfl.ch/.