Altium Designer Notes and PCB Design Guidelines
How to design a standard PCB layout using Altium Designer
This document is currently in a work in progress.
Table of Contents
Shortcut Keys
All Altium Designer Shortcut Keys [Download]
+400 Shortcuts for Altium Designer [View]
Schematic Designer
- General
Ctrl + M: Measure.C Then C: Compile the active project.D Then U: Update the PCB with any schematic changes.D Then O: Open the “Document Options” window.Q: Toggle the measurement unit system between metric and imperial.T Then C: Cross-probe a net, pin or component between the schematic and the PCB.
- Schematic Routing
P Then W: Start placing wires.
- Component Placement
J Then C: Jump to component.J Then N: Jump to net.T Then A Then A: Open the “Annotate” window.T Then A Then U Open the “Quick Annotate” window.
PCB Designer
- General
D Then I: Import changes from schematic to PCB.T Then D Then R: Run DRC (Design Rule Checks).Q: Toggle the measurement unit system between metric and imperial.T Then C: Cross-probe a net, pin or component between the schematic and the PCB.
- Routing
P Then T: 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 Then G Then A: Repour all polygons.
- Component Placement
L: Flip a component.Spacebar: Rotate object by 90°.J Then C: 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 Then M Then M: 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 Then B: 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 Then S / Ctrl + H: Enables you to select a section of connected copper. Stops the selection at a via, pad or intersection.D Then T Then <letter>: Select a view configuration. These views and their key shortcuts are user configurable.
D Then T Then U: Selects the “up” configuration (all top layers).D Then T Then D: Selects the “down” configuration (all bottom layers).
D Then O: 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.
Schematics
- Draw circuits from left to right and top to bottom.
- Draw circuits in functional block and use Net Labels for connecting blocks to each other.
- Use standard 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 the Cover 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 with clear and short 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.
- Use distinctly and clear names for schematics.
- Add useful Design 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 schematic close to the pins where they should be located on PCB.
- For example: bypass capacitors.
- Generate PDF of the completed schematic.
Setup Before Layout
Rules
- Clearance
D Then R > Design Rules > Electrical > Clearance- Clearance = 0.2 mm
- Routing
D Then R > Design Rules > Routing > Width- Min Width = 0.254 mm
- Preferred Width = 0.3 mm
- Max Width = 0.5 mm
D Then R > Design Rules > Routing > Width_PWR- Min Width (PWR) = 0.254 mm
- Preferred Width (PWR) = 1 mm
- Max Width (PWR) = 4 mm
D Then R > Design Rules > Routing > Routing Via Style- Via Diameter = 0.6 mm
- Via Hole Size = 0.3 mm
- Mask
D Then R > Design Rules > Mask > Solder Mask Expansion- Solder Mask Expansion = 0.1 mm
- Manufacturing
D Then R > Design Rules > Manufacturing > Hole To Hole Clearance- Hole to Hole Clearance = 0.3 mm
D Then R > Design Rules > Manufacturing > Minimum Solder Mask Silver- Minimum Solder Mask Silver = 0.3 mm
D Then R > Design Rules > Manufacturing > Silk to Solder Mask Clearance- Silk to Solder Mask Clearance = 0.1 mm
D Then R > Design Rules > Manufacturing > Silk to Silk Clearance- Silk to Silk Clearance = 0.1 mm
- Placement
D Then R > 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
Stackup
Design > Layer Stack Manager- Change Layer Names to L1 and L2, and etc.
- Thickness of Dielectric (PCB Thickness) = 1.6 mm
Set Net Colors
View > Panels > PCBPCB Panel > <Net Name> > Right-Click > Change Net ColorPCB 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
Placement
- Plan layout first, then placement.
- Start with BMC (Big, Main and Critical) components. e.g. MCU and clock devices.
- Place predefined location of components and connectors.
- Isolate analog and digital power supply sections.
- Place clock driver close to clock oscillator.
- Arrange components in rows and columns.
- Arrange components with uniform orientation, e.g. diodes and polarized capacitors.
- Indicate polarity on silk screen.
- Place all components on top side of the PCB. On complex and compact designs place short height and/or low 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
- Place bypass capacitors as close to IC as possible, use combination of 10uF and 100nF, place smaller cap closer to IC.
- Place connectors on one edge of the board.
- Place at least four mounting holes.
- Make sure enough space around mounting holes for screw heads to sit on and try placing big components around PCB.
- Keep more space around headers/connectors.
- Place hot components on the top side of the PCB.
- Must place test points on all power nets and optional critical signals and programming pins if needed.
Useful Links
评论