Repository files navigation

How to design a standard PCB layout using Altium Designer
This document is currently in a work in progress.

• General Information
• Shortcut Keys
• Components
• Schematics
• Setup Before Layout
  • Rules
  • Stackup
  • Set Net Colors
• Placement
• Layout
• High Speed Tips
• Useful Links

All Altium Designer Shortcut Keys [Download]
+400 Shortcuts for Altium Designer [View]

• General
  • Ctrl +M: Measure.
  • C ThenC: Compile the active project.
  • D ThenU: Update the PCB with any schematic changes.
  • D ThenO: Open the “Document Options” window.
  • Q: Toggle the measurement unit system between metric and imperial.
  • T ThenC: Cross-probe a net, pin or component between the schematic and the PCB.
• Schematic Routing
  • P ThenW: Start placing wires.
• Component Placement
  • J ThenC: Jump to component.
  • J ThenN: Jump to net.
  • T ThenA ThenA: Open the “Annotate” window.
  • T ThenA ThenU Open the “Quick Annotate” window.

• General
  • D ThenI: Import changes from schematic to PCB.
  • T ThenD ThenR: Run DRC (Design Rule Checks).
  • Q: Toggle the measurement unit system between metric and imperial.
  • T ThenC: Cross-probe a net, pin or component between the schematic and the PCB.
• Routing
  • P ThenT: Begin routing a track.
  • Tab (while routing): Brings up routing options/properties windows.
  • Shift +Space: Change the track routing style (e.g. from straight to 45 to curved and back again).
  • Shift +W: Set the track width to something from the predefined track width list.
  • T ThenG ThenA: Repour all polygons.
• Component Placement
  • L: Flip a component.
  • Spacebar: Rotate object by 90°.
  • J ThenC: Jump to component.
  • Ctrl +Shift +C: Align horizontal centers.
  • Ctrl +Shift +T: Align horizontal tops.
  • Ctrl +Shift +B: Align horizontal bottoms.
  • Ctrl +Shift +V: Align vertical centers.
  • Ctrl +Shift +L: Align vertical lefts.
  • Ctrl +Shift +R: Align vertical rights.
  • E ThenM ThenM: Move component (useful for when you can’t select it because it’s ontop of other components).
• Visualisation
  • Shift +S: Hide all but selected layer.
  • V ThenB: Flip board.
  • MouseScroll: Move up/down.
  • Shift +MouseScroll: Move left/right.
  • Ctrl +MouseScroll: Zoom in/out.
  • Ctrl +M: Measure.
  • + /-: Increment/Decrement through the enabled layers.
  • *: Increment/Decrement through routing layers only.
  • S ThenS /Ctrl +H: Enables you to select a section of connected copper. Stops the selection at a via, pad or intersection.
  • D ThenT Then<letter>: Select a view configuration. These views and their key shortcuts are user configurable.
    • D ThenT ThenU: Selects the “up” configuration (all top layers).
    • D ThenT ThenD: Selects the “down” configuration (all bottom layers).
  • D ThenO: Open Board Options window.
  • Ctrl +G: Open the Grid Editor window.
  • L: Show the Layers dialog box to adjust the visible layers and/or enable/disable layers.
  • G: Cycle through the predefined grids.

• Draw circuits fromleft to right andtop to bottom.
• Draw circuits in functional block and useNet Labels for connecting blocks to each other.
• Usestandard designators:
  • IC: IC or U
  • Resistor: R
  • Capacitor: C
  • Inductor: L
  • Transistor: Q or T
  • Diode/LED: D
  • Crystal: Y/XTAL
  • Pin headers: J
  • Jumper: JP
  • Fuse: F
  • Ferrite Bead: FB
  • Fiducial: FD
  • Test point: TP
• Add theCover Page to the schematic:
  • Project name
  • Date
  • Re/version number
  • All the names of schematics
  • Notes legend
  • Company information
  • Schematic status with date (Draft, Preliminary, Checked, Released)
    • Draft: Blocks, just the structure of the schematic.
    • Preliminary: Connections done, Quiet close to final.
    • Checked: No mistakes in schematic.
    • Released: PCB sent for fab.
• Don't connect 4 wires at one junction.
• Place all labels, designators, pins, text etc.horizontally.
• Don't fill up the whole sheet.
• Name schematics withclear andshort name.
  • For example: Use CPU_HDMI and CPU_LVDS instead of CPU1 and CPU2.
• Use "+...V..." for power nets
  • Never use "VCC" as net name!
  • For example: +12V, +5V, +3V3, +2V5, and etc.
• Fill information in Title block.
• Usedistinctly andclear names for schematics.
• Add usefulDesign Notes on the schematic.
• If you suspect that there are parts in the circuit, place them. If you do not need them, you can remove them later!
• Double check RX & TX pins.
  • Never use "TX" & "RX" as net name alone!
  • For example: Use MCU_TX or GPS_RX instead of TX or RX alone!
• Put enough and useful Test Points (TPs) for circuit debugging.
• Place components in the schematicclose to the pins where they should be located on PCB.
  • For example: bypass capacitors.
• GeneratePDF of the completed schematic.

• Clearance
  • D ThenR >Design Rules >Electrical >Clearance
  • Clearance = 0.2 mm
• Routing
  • D ThenR >Design Rules >Routing >Width
  • Min Width = 0.254 mm
  • Preferred Width = 0.3 mm
  • Max Width = 0.5 mm
  • D ThenR >Design Rules >Routing >Width_PWR
  • Min Width (PWR) = 0.254 mm
  • Preferred Width (PWR) = 1 mm
  • Max Width (PWR) = 4 mm
  • D ThenR >Design Rules >Routing >Routing Via Style
  • Via Diameter = 0.6 mm
  • Via Hole Size = 0.3 mm
• Mask
  • D ThenR >Design Rules >Mask >Solder Mask Expansion
  • Solder Mask Expansion = 0.1 mm
• Manufacturing
  • D ThenR >Design Rules >Manufacturing >Hole To Hole Clearance
  • Hole to Hole Clearance = 0.3 mm
  • D ThenR >Design Rules >Manufacturing >Minimum Solder Mask Silver
  • Minimum Solder Mask Silver = 0.3 mm
  • D ThenR >Design Rules >Manufacturing >Silk to Solder Mask Clearance
  • Silk to Solder Mask Clearance = 0.1 mm
  • D ThenR >Design Rules >Manufacturing >Silk to Silk Clearance
  • Silk to Silk Clearance = 0.1 mm
• Placement
  • D ThenR >Design Rules >Placement >Component Clearance
  • Component Clearance (Vertical) = 0.2 mm
  • Component Clearance (Horizontal) = 0.2 mm
• Via
  • DXP >Prefs >PCB Editor >Defaults >Via
  • Via Diameter = 0.6 mm
  • Via Hole Size = 0.3 mm

• Design >Layer Stack Manager
• Change Layer Names to L1 and L2, and etc.
• Thickness of Dielectric (PCB Thickness) = 1.6 mm

• View >Panels >PCB
• PCB Panel ><Net Name> >Right-Click >Change Net Color
• PCB Panel ><Net Name> >Right-Click >Display Override > Selected ON
• Net Color for GND = Blue (236)
• Net Color for PWR = Orange (4) or Pink (1)
• F5 = Toggle Net Colors

• Plan layout first, then placement.
• Start withBMC (Big, Main and Critical) components. e.g. MCU and clock devices.
• Placepredefined location of components and connectors.
• Isolateanalog and digital power supply sections.
• Placeclock driver close to clock oscillator.
• Arrange components in rows and columns.
• Arrange components withuniform orientation, e.g. diodes and polarized capacitors.
• Indicate polarity on silk screen.
• Place all components ontop side of the PCB. On complex and compact designs placeshort height and/orlow thermal dissipation components go on bottom, never place tall components on the bottom side else it will increase the total height of the PCB.
• Keep 1mm (40mil)space between components and 2.5 and/or 3 (100mill and/or 120mil) from component to edge
• Placebypass capacitors as close to IC as possible, use combination of 10uF and 100nF, place smaller cap closer to IC.
• Placeconnectors on one edge of the board.
• Place at least fourmounting holes.
• Make sureenough space around mounting holes for screw heads to sit on and try placing big components around PCB.
• Keep more space aroundheaders/connectors.
• Placehot components on the top side of the PCB.
• Must placetest points on all power nets and optional critical signals and programming pins if needed.

• Open Source Altium libraries
• 3D and 2D CAD Models
• PCB Trace Max Current Calculators
• Trace Width Calculators
• PCB Trace Resistance Calculator
• Impedance Calculators