Skip to content

NOTES.md

Latest commit

 

History

History
107 lines (82 loc) · 4.21 KB

NOTES.md

File metadata and controls

107 lines (82 loc) · 4.21 KB
Raw

Notes for KiCad

  • Install the correct version
sudo add-apt-repository ppa:kicad/kicad-8.0-releases
sudo apt update
sudo apt install kicad

  • Open KiCad and choose File > New Project.... Select the project location. Un-check "Create a new folder for the project," and type the project name (here: sb-sca). If asked for confirmation, choose "Yes" to continue.

  • Launch the Schematic Editor. Accept "Copy default global symbol library table (recommended)" if prompted. Choose File > Page Settings..., select "Size: USLetter 8.5x11in", and press "OK." Save the schematic.

  • Next, open the Symbol Editor by choosing Tools > Symbol Editor from the Schematic Editor.

  • Using the Symbol Editor, choose File > New Library... and choose the "Project" scope when prompted. Enter the project name (here: sb-sca).

  • Import the .kicad_sym files from the components/ directory. New symbols can be obtained from componentsearchengine.com (free account required). Select File > Import > Symbol... and save in the project library.

  • Open the Footprint Editor. Accept "Copy default global footprint library table (recommended)" if prompted. Choose File > New Library... and choose the "Project" scope when prompted. Enter the project name (here: sb-sca).

  • Import the .kicad_mod files from the footprints/ directory. New footprints can be obtained from componentsearchengine.com. Select File > Import > Footprint... and save in the project library.

  • For each footprint, associate the corresponding .stp 3D model file from the 3d-models/ directory. Choose File > Footprint Properties... and specify the path to the 3D model file under the 3D Models tab.

  • Lay out the schematic in the Schematic Editor. Set the label values.

  • From the Schematic Editor, select Tools > Annotate Schematic... and choose "Scope: Entire schematic;" "Options: Keep existing annotations;" "Order: Sort symbols by X position;" and "Numbering: Use first free number after: 0." Leave "Recurse into subsheets" checked. Select "Annotate."

  • Also from the Schematic Editor, choose Tools > Assign Footprints... and set the footprints.

  • Specify footprints that cannot be set automatically: Conn_01x04_Socket : sb-sca:SB_SCA_MountingHoles, and Conn_01x16_Socket : sb-sca:SB_SCA_VSOL_PADS, and Solar_Cell : sb-sca:KXOB25-02X8TF

  • Open the PCB Editor and choose File > Page Settings... to select "Size: USLetter 8.5x11in"

  • Choose File > Board Setup... and under "Board Stackup > Physical Stackup," choose Copper layers: 4. Enter the layer information from the fabrication company.

  • Under "Board Stackup > Board Editor Layers," enable F.Paste, F.Silkscreen, F.Mask, F.Cu, In1.Cu, In2.Cu, B.Cu, B.Mask, B.Silkscreen, and B.Paste.

  • Under "Board Stackup > Solder Mask/Paste," set the Solder mask minimum web width to the value provided by the manufacturer.

  • Add the PCB outline with graphic lines.

Graphic Lines for PCB Edge

Create the following in the Edge.Cuts layer:

  • Start: (120, 80); End: (170, 80)

  • Start: (120,130); End: (170,130)

  • Start: (120, 80); End: (120, 80)

  • Start: (170, 80); End: (170,120)

  • From the PCB Editor, choose Tools > Update PCB from Schematic and choose Update PCB.

  • Place the components, vias, and tracks.

    • J1: (145.00, 105.00) @ 0.0
    • J2: (145.00, 105.00) @ 0.0
    • Etc.

Generating Gerbers

  • Ensure that fill zones have been redrawn by running the Design Rules Checker
  • Choose File > Plot... from the PCB Editor
    • Output directory: ../gerbers/
    • Included Layers: F.Cu, In1.Cu, In2.Cu, B.Cu, F.Paste, B.Paste, F.Silkscreen, B.Silkscreen, F.Mask, B.Mask, Edge.Cuts
    • General Options: Plot footprint values, Plot footprint reference designators, Plot footprint text, Check zone fills before plotting, Tent vias
    • Gerber Options: Generate Gerber job file, Use extended X2 format, Include netlist attributes
  • Choose "Plot"
  • Choose "Generate Drill Files..."
    • Output folder: ../gerbers/
    • Drill File Format: Excellon, Oval Holes Drill Mode: Use alternate drill mode
    • Map File Format: Gerber X2
    • Dill Origin: Absolute
    • Drill Units: Millimeters
    • Zeros Format: Decimal format (recommended)
  • Choose "Generate Drill File"