/altium

A collection of Altium libraries and DRC rules collected over time

Altium

A collection of standardized Altium libraries and DRC rules collected over time. Below are the repository guidelines.

Schematic Libraries

  • Schematic libraries are to be named Schematic_Category.SchLib where Category groups parts with similar function (diode, MCU, connector, etc).
  • Each part is to be populated with parameter, descriptive, and ordering information using Altium's manufacturer part search feature. The symbol itself should not contain vendor-specific information (such as vendor part number).
  • Do include information such as I2C addresses, or anything else that might be useful on the symbol.
  • Inputs should be on the left side of the part, and outputs should be on the right side of the part for parts with obvious input-output relationships.
  • Related pins should be grouped together on the schematic symbol (see the Group column if using the Schematic Wizard).
  • For parts with a large pin count, the schematic symbol should be separated into multiple component parts. Consider splitting on groups such as power, I/O, etc.

Footprint Libraries

  • Footprint libraries are to be named Footprint_Category.PcbLib where Category groups parts with similar function (diode, MCU, connector, etc).
  • Footprints should be created using the IPC Compliant Footprint Wizard whenever possible, generating a STEP 3D model. Although the wizard may suggest a land pattern based on the part dimensions, these should be overridden with the manufacturer's recommended land pattern when applicable.
  • If the IPC Compliant Footprint Wizard cannot be used, Template_Footprint.PcbLib should be used as a template to build the footprint, following the recommended land pattern in the part data sheet.
  • All footprint origins should be placed at the center of their part's bounding box.
  • Footprints should inherit the suggested name if using the IPC Compliant Footprint Wizard, otherwise use the manufacturer's part name.
  • All footprints should follow the following component layer pair/mechanical layer configuration. Note that parts using the IPC Compliant Footprint Wizard will likely need portions moved from mechanical layers to component layer pairs following the style below.
    • Component Layer Pairs (must be layer type assigned)
      • Overlay
      • Solder
      • Paste
      • Assembly on layers M2/M3
      • Courtyard on layers M4/M5
      • 3D Body on layers M6/M7
    • Mechanical Layers
      • Mechanical 1 (used only for board cutouts)

Layer Guidelines

Assembly

  • The assembly layer should contain an 0.1mm line width rectangle sized to be the bounding box of the part (not pad) dimensions.
  • The assembly layer should also contain a center justified string .Designator, at the part center, with height and stroke width appropriate such that the string is easily readable and 4 characters do not intersect the aforementioned bounding box.

Courtyard

  • The courtyard layer should contain an 0.1mm line width cross (two perpendicular 1mm lines, shorter if necessary) at the part center.
  • The courtyard layer should also contain an 0.05mm line width rectangle sized to be 0.25mm larger on each size of the bounding box of the greater of the part and pad dimensions.

3D Body

  • The 3d Body layer should contain an accurate 3D model of the part if available. An attempt should be made to search for a 3D model if the IPC Compliant Footprint Wizard cannot be used.

Mechanical 1

  • Mechanical 1 should contain any board cutouts required for the part. This layer, or any other mechanical layer, should not be used otherwise.

Overlay layers

  • Overlays should use 0.2mm line width if possible, should be adequately spaced from any solder mask expansions, and should clearly indicate pin 1 if necessary.