Component Creation
Templates
All components shall use their respective templates when being created. Templates may specify required parameters, these must be filled in.
There shall be no additional parameters for a component other than the ones specified in the template, unless it is necessary to capture a unique property of high importance.
Manufacturer part search
The “Acquire” feature to import a component to our library shall not be used from manufacturer part search. It may be used only from the Altium Celestial library if installed, and only for active components for which standard symbols and footprints do not exist.
A part choice may be used to auto-fill parameters present in a component template. You may “fix” parameters to map the property names used in the template to those used by the manufacturer. Only parameters in templates shall be imported. Symbols, footprints, and data sheets shall not be imported.
Component Name
In general, the component name should be the “Description” field from Digikey. By default, it will be the MPN which is meaningless for most people. However, naming conventions exist for the following type of components. The Digikey description will often, but not always match these conventions.
Resistors
“RES [value][unit prefix] OHM [tolerance]% [power fraction]W [package]”
Examples:
“RES 1K OHM 1% 1/10W 0603”
“RES 10m OHM 1% 1W AXIAL”
Capacitors
“CAP [type] [value][unit prefix]F [voltage]V [dielectric] [package]”
Examples:
“CAP CER 0.1UF 25V X7R 0603”
“CAP ALUM POLY 47UF 20% 35V SMD”
Symbol and Footprint Usage
Symbols and footprints for all common components shall use the standard symbols available in our library. You must choose to use an existing model during component creation, and choose from the ones available at Managed Content/(somewhere).
Only if a standard model does not exist, such as for ICs, you may create one. Models shall not be imported from the manufacturer part search, however they may be imported from the Altium Celestial library if installed.
Please reach out to a lead if you believe a new standard model for commonly used components should be created!
Symbol Creation
Symbols shall only be created when no suitable models already exist. This will be the case most often for ICs.
Designators
Keep designators to commonly used values. A list can be found at https://en.wikipedia.org/wiki/Reference_designator#Designators. If there is already similar component, use the same designator!
Pin Arrangement
Pins should be arranged to prioritize schematic readability over being representative of their physical location. The “typical application” section of a data sheet usually has a good arrangement of pins that lead to readable schematics.
Pin Type
Pins shall be of the “passive” type. It’s too much of a hassle to deal with maintaining the proper logic required for other pin types across all our schematics.
Pin length shall be 200 mils.
Parameters
Symbols shall have the following visible parameters:
Integrated Circuit: Name, MPN
Capacitor: Value, Voltage, Dielectric
Resistor: Value, Power, Tolerance
Inductor: Value, Continuous Current
FET: Name or (Current, Vdsmax)
Footprint Creation
Footprints shall only be created when no suitable models already exist.
Footprints shall follow IPC conventions and be made to the “Medium Density” specification. It is encouraged to use the Altium IPC compliant footprint wizard.
All footprints must have a detailed STEP model of the part, unless one cannot be obtained from the manufacturer or generated by the wizard. In that case, a rough approximation must be created using primitive shapes in Altium.
For IPC compliant packages where the manufacturer recommended footprint differs from the IPC standard, follow the IPC standard unless specific conditions exist where it would not be feasible to do so.