Altium component library standards for creating consistent electronic components across multiple projects

1. Altium Component Library Standards
hoani.net

2. Component Library
The component library includes schematic symbols and PCB footprints.
Simulation models are not covered here.

3. Component Designators
Use consistent designator assignments across all projects
Component Designator Component Designator Component Designator Component Designator
BJT Q? Diode D? LED D? Solenoid M?
Buzzer B? Fan M? MOSFET Q? Speaker B?
Capacitor C? Ferrite Bead FB? Motor M? Switch S?
Cap Array CA? Fiducial FID? Oscillator X? Thermistor R?
Chokes L? Fuse F? Relay K? Transformer T?
Connector J? IC U? Resistor R? TVS D?
Crystal X? Inductor L? Res Array RA? Zener D?
DIAC D? Jumper J? SIDAC D?

4. Component Pins
Pin numbers follow the datasheet
When provided, pin numbering shall follow the
manufacturer’s datasheet.
Two row connector pin numbering zig-zags
When two row connectors are not given default
numbering, numbering shall increment in zig-zags down
the connector, with odd numbers down one row and
even numbers down the opposite row.
Default pin numbering is counter clockwise
When a part’s pin numbering is ambiguous, numbering shall increment counter clockwise about
the component’s center.
Name pins the same as the datasheet
All component pin names shall match the component’s datasheet.

5. Schematic Symbols
A new symbol for each part number
Every schematic symbol item shall model one real world component.
While it may be tempting to want to represent multiple alternative parts under the same library symbol, this
gets complicated. For example, a chip capacitor has:
● Capacitance
● Voltage rating
● Temp. coefficient
● Temp. rating
● Package size
● Low ESL etc.

6. Schematic Symbol Drawing
Use consistent drawing primitives
All symbols shall be made up of the same basic primitives and share the same color scheme:
● Free form symbols are made up of a combination of pins and blue lines/arcs.
● Package symbols (such as ICs, connectors etc) are a combination of pins and rectangles.
● Pin designators start at 1, and count up.
● Drawing grid must be 10 when placing pins.
● Pin size must be a multiple of 10.
Drawing Element Color RGB Hex Code
Pin Black #000000
Symbol Primitives Blue #0000FF
Box Outline Dark Red #800000
Box Fill Light Yellow #FFFFB0

7. Schematic Symbol Properties

8. Schematic Symbol Properties
Component identifiers are the part number
A component’s Design Item ID and comment field shall be its part number.
This ensures a unique Desing Item ID and is consistent with the Supplier Links feature.
Use Digi-Key descriptions
The Description field should have the Digi-Key description when possible.
If the part cannot be purchased on Digi-Key, then try your best to describe the part in a consistent way to
the rest of the library items.

9. Schematic Symbol Properties - Parameters
A component’s parameters depend on the component type.
Components of the following types shall have additional parameters as defined in the table below:
Component Parameter Description
BJT Vce Max collector-emitter voltage
Capacitor/
Capacitor Array
Value Set to capacitance
VRating Capacitor voltage rating
Crystal/Oscillator Frequency Component frequency
DIAC/SIDAC Vbr Breakover voltage
Diode VReverse Reverse voltage rating
IForward Maximum forward current
Ferrite Bead Value Set to <Impedance@Freq> for
example: 150@10MHz
Component Parameter Description
Fuse IRated Holding current rating
Inductor Value Inductance
IRated Max current or saturation
current, whichever is lower
Mosfet Vds Max drain-source voltage
Resistor/
Resistor Array
Value Set to resistance
Thermistor RNominal Nominal resistance at 25°C
TVS/Zener Vz Zener voltage (or breakdown
voltage)

10. PCB Footprint - Drawing 1 of 2
Draw from the top layer
All PCB footprints shall use the top layer and/or multilayer as the primary pad layers.
In special cases, such as edge connectors, a footprint may use both top and bottom layers. Don’t use
bottom pad layers on their own - doing this is can cause a bottom layer component to end up being listed
as a top layer component which will confuse assembly.
Silkscreen clarifies placement
Silkscreen may be used to:
● Show component shape
● Show polarity of components
● Indicate pin 1 of a component (use a dot at least 0.15mm or 6 mil in diameter)
Don’t make silkscreen too thin
Silkscreen primitives shall be 0.15mm (6 mil) or thicker.

11. PCB Footprint - Drawing 2 of 2
Follow Altium’s Wizard Mechanical Layers
PCB footprints shall use the following mechanical layers:
● Layer 13 - Component body
● Layer 15 - Courtyard
These layer choices are compatible with Altium’s IPC footprint wizard.
Position 0,0 is the footprint’s center
The center of a component should generally be placed in the middle of the courtyard.
With the exception of 1-pin footprints (such as test points or fiducials), the center should never be placed
on pin 1. This is because it makes using automatic centering of designators harder to read.

12. PCB Footprint - Naming 1 of 3
Standard chip naming is 0803C_N
Chip footprint naming shall follow <imperial package><type>_<density>. Where:
● <imperial package> is the imperial package (eg. 0402, or 1206).
● <type> is the component type:
○ C is capacitor
○ D is diode or LED
○ F is ferrite bead
○ L is inductor
○ R is resistor
● <density> is the placement density of the component:
○ L is “Least” (or high density)
○ N is “Normal” (or medium density)
○ M is “Most” (or low density)

13. PCB Footprint - Naming 2 of 3
Standard footprint naming is SOIC-8_L
Any footprint following an IPC standard shall be named <standard>_<density>
For example:
● SOT23-3_M is a “Most” (or low density) SOT23-3 footprint
● SOIC-8_L is a “Least” (or high density) SOIC-8 footprint
Manufacture Specific footprint naming is STM_8-DFM-5x6
Any manufacturer specific footprint shall be named <manufacturer>_<package>
For example:
● SEMTECH_16-QFN is a 16-QFN footprint from SemTech
● STM_8-DFM-5x6 is an 8-DFM footprint from STMicroelectronics

14. PCB Footprint - Naming 3 of 3
Non-standard footprint naming uses the part number
Non-standard component footprints shall be named <partnumber> or
manufacturer>_<partnumber>
Non-component footprint naming is freeform
All non-component footprints should use descriptive freeform names

15. Component Libraries - Symbol Libraries
Group symbol libraries by component types.
Schematic symbol libraries shall be defined as shown in the table below.
Library Name Component Types Library Name Component Types
Capacitor Capacitor, Capacitor Array Oscillator Crystal, Oscillator, Clock Modules
Connector Connector, Jumper Processor Microcontroller, Microprocessor, FPGA, Processor
Module
Diode Rectifier Diode, Diode Array, DIAC, LED, Zener Protection TVS Diodes, TVS Modules, Fuses
Display Display IC, Display Modules, LED Modules Resistor Resistor, Resistor Array
Filter Filter IC, Filter module, Ferrite Bead Sensor Sensor IC, Sensor Module
Fuse Fuse Switch Relay, Switch
Inductor Inductor Thermistor PTC, NTC
Transistor MOSFET, JFET, BJT, IGBT, SCR, TRIAC Transducer Buzzer, Fan, Motor, Solenoid, Speaker
Misc Anything that doesn’t fit elsewhere Transformer Common Mode Chokes, Transformer

16. Component Libraries - PCB Libraries
Have a chip footprint library
All IPC standard chip footprints shall be in a single dedicated footprint library.
Have a mechanical library
Footprints which do not represent electronic components shall be placed in a dedicated mechanical
library.
Examples include: Mounting holes, mouse bites, logos, net ties and test points.
Group common IPC standard footprints in libraries
IPC standard footprints shall be grouped in footprint libraries specific to the type of footprint.
Examples include: DO (diode SMA, SMB, SMC etc), SOIC (small outline ICs) and SOT-23
Any other footprints are grouped by component types
Non-standard or manufacturer specific component footprints shall be grouped in footprint libraries
based on their component types.