Altium Designer

Altium Designer is an advanced schematic and PCB design software.

• PCB Design

Base settings

• Text height: 30mil [1]
• Text width: 8mil
• Grid snap: 5mil

Layer Standards

• Mechanical 1 – Board Outline (along with the Keep-Out Layer, but that can be used for other things also)
• Mechanical 2 – PCB Info (manfacturing info, added as text)
• Mechanical 11 – Top Layer Dimensions <paired with M12>
• Mechanical 12 – Bottom Layer Dimensions <paired with M11>
• Mechanical 13 – Top Layer Component Body Information (3D models and mechanical outlines) <paired with M14>
• Mechanical 14 – Bottom Layer Component Body Information (3D models and mechanical outlines) <paired with M13>
• Mechanical 15 – Top Layer Courtyard and Assembly Information <paired with M16>
• Mechanical 16 – Bottom Layer Courtyard and Assembly Information <paired with M15>

Libraries

• Add the following libraries to get a good base to start from - edit the symbols or footprints to fit your need
• Libraries:
  • Miscellaneous Devices and Miscellaneous Connectors
  • Altium 10 libraries - all major manufacturers covered
  • SparkFun Altium PCB Library - selection of common parts
  • siliconvalleygarage.com - good selection
  • altium designer addons - tons of scripts and libraries

New project

• Add a new PCB group by in the File menu

New Schematic

• Create a schematic and add it to the PCB group by dragging it in the Projects panel
• Save the board in a new project folder

New PCB

• Create a new PCB board using the PCB Wizard on the Files panel and drag the PCB into the PCB group in the Projects panel
• Right-click the sheet and select Options, Board Options and uncheck Display Sheet
• Add the necessary design rules before transferring the schematic, i.e. thicker power traces for power nets
• Save the board in the same folder as the schematic

Edit schematic symbols

• Create a new Schematic Library to collect the new symbols, save it to a common location
• Open the other Integrated Library or Schematic Library from the File menu and in the Project panel pick the SchLib file
• Switch over to the SCH Library panel to view all the symbol drawings
• In Tools, select Copy component to save it to your own Schematic Library from the list
• Make the changes to the symbol and save it
• To use the new symbol, open the Schematic and place a new component, select your own SchLib file to view the list of all the components

Edit footprint

• Create a new PCB Library for the new footprints
• Open the other PCB Library, from the File menu, with the footprint you want to edit and pick it from the Projects panel
• Switch to the PCB Library panel to view all the footprints, pick the right one
• In Edit, pick Copy Component to copy the entire footprint
• Switch over to your own PCB Library in the Projects panel, the PCB Library, and right-click in the Components list to Paste 1 Components to the library
• Edit the footprint and save it for later use

Make generic footprint

• Open your PCB Library and switch over to PCB Library panel
• In Tools, pick IPC Compliant Footprint Wizard to make common SMD footprints or Component Wizard for all other kinds
• The footprint is automatically added to your current open PCB library

Define footprints for components

• In the schematic, select Footprint manager in the Tools menu
• Go through the list to by clicking Add and Browse to pick the correct footprint for each component
• Right-click to select Set As Current to make it active

Transfer design

• Compile the schematic in the Project menu and watch the System, Messages window for error messages, double-click the line to focus on the fault
• In the schematic, select the Design menu and Update PCB to transfer the design
• Click Validate Changes and Execute Changes, watch for errors after the transfer has been performed
• All the components footprints will now be placed besides the PCB board outline ready to be placed and routed

If one of the transfers fails with a message "unknown pin", do:

• Open the PCB Library for the footprint and find the footprint in the PCB Library panel
• Change the name and designator to match the schematic symbol, i.e. pin 1 in the symbol should be pin 1 on footprint
• Save and switch over to the footprint manager to change to the new footprint/make sure the pin designators has been updated

Routing board

Traces

• Place the components in a favorable way with common components grouped close together to minimize trace length
• Use Interactive Routing from the Place menu to lay the traces
• It might be useful to perform a Autoroute to check if there is problems or better ways to place the components, undo the autoroute
• Shortcut for Interactive Routing is P+T

• Routing a net reference

Re-routing board

• Use the Interactive Routing tool to place a new trace, the old one will automatically be erased when the new on is laid
• To unroute a trace use T+U+C

Adding via and changing layer automatically

• While routing a trace, press "+" and click to add a via and change signal layer

Quickly change via or trace size

• Press the 3 and 4 button while placing a via or trace to change to to preferred, max or min according to the set rules

Ground pour

• Place a Polygon Pour from the Place menu
• Select Solid and change the Net to GND
• Click the four corners of the board to mark the area where the copper should pour/remain
• To make it easier to place and route the board, hide the pour by right-clicking on the board, Options, Show/Hide, and Hide Polygons
• After moving parts, update the pour in Tools Polygon Pour and Repour All Polygons

Board shape

• Select Design, Board Shape, Redefine Board Shape and click on the 4 corners to outline the board size
• Then select Create Primitives From Board Shape, 4mil width, put the board outline on the Keep-out layer (Gerber friendly, GKO file)

Fabrication files

• To get standard Gerber manufacturing files, open the PCB and select File, Fabrication Output and Gerber files
• Select Format 2:5, clock Plot Layers and Used on, deselect Paste, Mechanical, and Pad Master layers and enable the GKO Board Outline layer when sending to a PCB manufacturer
• Click OK and get the Gerber files
• Then for the drill files, go to File, Fabrication Output and NC Drill files
• Select Format 2:5 and click OK to export the drill text file

References

• Alitum tricks and standards