Altium-Designer-Notes-and-PCB-Design-Guidelines
Altium-Designer-Notes-and-PCB-Design-Guidelines copied to clipboard
How to design a standard PCB layout using Altium Designer
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
- General Information
- Shortcut Keys
- Components
- Schematics
-
Setup Before Layout
- Rules
- Stackup
- Set Net Colors
- Placement
- Layout
- High Speed Tips
- Useful Links
Shortcut Keys
All Altium Designer Shortcut Keys [Download]
+400 Shortcuts for Altium Designer [View]
Schematic Designer
-
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.
-
PCB Designer
-
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.
-
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
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
-
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
>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
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.