Automation

[derwana]

This thread is for showing all of my automation attempts.

I just dived into KiBot and KiAuto for generating PDF, Gerber and STEP files.

So i installed current releases of both repos and put the following cm4_matx.kibot.yaml file into the projects root folder.

# documentation at https://github.com/INTI-CMNB/kibot

kibot:
  version: 1

preflight:
  # [boolean=false] Zones are filled before doing any operation involving PCB layers
  check_zone_fills: true
  # [list(dict)] A list of entries to filter out ERC/DRC messages
  #filters: 
  #  - filter: 'Filter description'
  #    error: '10'
  #    regex: 'Regular expression to match'
  # [boolean=false] Option for `run_drc`. Ignores the unconnected nets. Useful if you didn't finish the routing
  #ignore_unconnected: true
  # [boolean=false] Runs the DRC (Distance Rules Check). To ensure we have a valid PCB
  #run_drc: true
  # [boolean=false] Runs the ERC (Electrical Rules Check). To ensure the schematic is electrically correct
  #run_erc: true
  # [boolean=false] Update the XML version of the BoM (Bill of Materials).
  update_xml: true


outputs:
  ### GERBERS ######################################################
  - name: 'gerbers'
    comment: "Exporting the PCB to Gerbers."
    type: 'gerber'
    dir: 'gerber'
    options:
      # generic layer options
      exclude_edge_layer: false
      exclude_pads_from_silkscreen: false
      plot_sheet_reference: false
      plot_footprint_refs: true
      plot_footprint_values: true
      force_plot_invisible_refs_vals: false
      tent_vias: true
      line_width: 0.15
      # gerber options
      use_aux_axis_as_origin: false
      subtract_mask_from_silk: true
      use_protel_extensions: false
      gerber_precision: 4.5
      create_gerber_job_file: true
      use_gerber_x2_attributes: true
      use_gerber_net_attributes: false
    layers:
      - 'F.Cu'
      - 'B.Cu'

  - name: 'gerber_drills'
    comment: 'Exporting drillings of PCB to Gerbers.'
    type: 'gerb_drill'
    dir: 'gerber'
    options:
      # [dict|string] [hpgl,ps,gerber,dxf,svg,pdf] format for a graphical drill map.
      # Not generated unless a format is specified
      map:
        # [string='%f-%i%v.%x'] name for the map file, KiCad defaults if empty (%i='PTH_drill_map'). Affected by global options
        output: ''
        # [string='pdf'] [hpgl,ps,gerber,dxf,svg,pdf] format for a graphical drill map
        type: 'gerber'
      # [string='%f-%i%v.%x'] name for the drill file, KiCad defaults if empty (%i='PTH_drill'). Affected by global options
      output: ''
      # [boolean=false] use the auxiliar axis as origin for coordinates
      use_aux_axis_as_origin: false

  - name: 'position'
    comment: 'Generating position information for the PCB components.'
    type: 'position'
    dir: 'gerber'
    options:
      # [list(dict)|list(string)] which columns are included in the output
      #columns:
        # [string=''] [Ref,Val,Package,PosX,PosY,Rot,Side] Internal name
      #  id: ''
        # [string=''] Name to use in the outut file. The id is used when empty
      #  name: ''
      # [string|list(string)=''] Name of the filter to mark components as not fitted.
      # A short-cut to use for simple cases where a variant is an overkill
      #dnf_filter: ''
      # [string='ASCII'] [ASCII,CSV] format for the position file
      format: 'CSV'
      # [boolean=true] only include the surface mount components
      only_smd: true
      # [string='%f-%i%v.%x'] output file name (%i='top_pos'|'bottom_pos'|'both_pos', %x='pos'|'csv'). Affected by global options
      output: 'positions.csv'
      # [boolean=true] generate two separated files, one for the top and another for the bottom
      separate_files_for_front_and_back: true
      # [string='millimeters'] [millimeters,inches] units used for the positions
      units: 'millimeters'
      # [string=''] Board variant to apply
      #variant: ''

  ### PDFs ##########################################################
  - name: 'pdf-sch'
    comment: 'Exporting the PCB to PDF. Suitable for printing.'
    type: 'pdf_sch_print'
    dir: 'pdf' 
    options:
      # [string|list(string)=''] Name of the filter to mark components as not fitted.
      # A short-cut to use for simple cases where a variant is an overkill
      #dnf_filter: ''
      # [string='%f-%i%v.%x'] filename for the output PDF (%i=layers, %x=pdf). Affected by global options
      output: 'CM4_MATX_SCH.pdf'
      # [string=''] Board variant to apply
      #variant:

  - name: 'pdf-pcb'
    comment: "Exporting the PCB as PDF"
    type: 'pdf_pcb_print'
    dir: 'pdf'
    options:
      # [string|list(string)=''] Name of the filter to mark components as not fitted.
      # A short-cut to use for simple cases where a variant is an overkill
      #dnf_filter: ''
      # [string='full'] what to use to indicate the drill places, can be none, small or full (for real scale)
      drill_marks: 'full'
      # [boolean=false] print mirrored (X axis inverted). ONLY for KiCad 6
      mirror: false
      # [boolean=false] print in black and white
      monochrome: false
      # [string='%f-%i%v.%x'] filename for the output PDF (%i=layers, %x=pdf). Affected by global options
      output: 'CM4_MATX_PCB.pdf'
      # `output_name` is an alias for `output`
      # [boolean=true] include the title-block
      plot_sheet_reference: true
      # [number=1.0] scale factor (0 means autoscaling)
      scaling: 1.0
      # [boolean=false] print layers in separated pages
      separated: false
      # [string=''] Board variant to apply
      #variant: ''
    layers: 'all'

  ### STEP ##########################################################
  - name: 'step'
    comment: 'Exporting the PCB as a 3D model.'
    type: 'step'
    dir: 'step'
    options:
      # [string|list(string)=''] Name of the filter to mark components as not fitted.
      # A short-cut to use for simple cases where a variant is an overkill
      #dnf_filter: ''
      # [boolean=true] use metric units instead of inches
      metric_units: true
      # [number=-1] the minimum distance between points to treat them as separate ones (-1 is KiCad default: 0.01 mm)
      min_distance: -1
      # [boolean=false] used to exclude 3D models for components with 'virtual' attribute
      no_virtual: false
      # [string='grid'] determines the coordinates origin. Using grid the coordinates are the same as you have in the design sheet.
      # The drill option uses the auxiliar reference defined by the user.
      # You can define any other origin using the format 'X,Y', i.e. '3.2,-10'
      origin: 'grid'
      # [string='%f-%i%v.%x'] name for the generated STEP file (%i='3D' %x='step'). Affected by global options
      output: 'CM4_MATX.step'
      # [string=''] Board variant to apply
      #variant: ''

By running kibot -b ./KiCad/CM4_MATX.kicad_pcb from the root folder it creates the folders gerber, pdf and step and populates these with the generated files. It also generates a BoM file named CM4_MATX.csv at the projects root.

It can also be used as Github Action on push or merge (needs Docker).

[derwana]

Also added a little python script for generating a jpg from pdf:

# needs packages pdf2image, pillow

# import modules
import os
from pdf2image import convert_from_path 
from PIL import Image 

  
# open pdf 
images = convert_from_path('./CM4_MATX_PCB.pdf') 

# convert to jpg
for img in images: 
    img.save('./CM4_MATX_PCB_tmp.jpg', 'JPEG')

# open jpg
img = Image.open(r"./CM4_MATX_PCB_tmp.jpg") 

# set cropping (px) 
left = 200
top = 100
right = 2300
bottom = 2200

# crop image  
img_cropped = img.crop((left, top, right, bottom)) 

# save image
img_cropped.save("./CM4_MATX_PCB.jpg")

# remove *tmp.jpg
os.remove("./CM4_MATX_PCB_tmp.jpg")

[TheGuyDanish]

Looks good. I'll try and get to testing putting this into the repo in the next couple of days. I'm more looking towards the automated PCB and schematic files than anything at the moment, since we aren't in a state to pass ERC/DRC checks anyway.

[derwana]

In the config for KiBot i disabled run_drc, run_erc so it does not throw any warnings and errors - just generates the files.

[derwana]

Run KiBot prior to the Python script, else no PDFs are found.

[derwana]

Python function for exporting a VRML file: ExportVRML_File()

[derwana]

VRML exporting is yet not supported via Python.

[TheGuyDanish]

IT LIVES

https://github.com/TheGuyDanish/CM4_MATX/runs/1617944772

[TheGuyDanish]

I'm pretty sure it can be put anywhere. Maybe in .github for simplicity. I'm not sure how much value it will have though. Since it doesn't put the final image in the repo, just as a artifact of the build.

[derwana]

Isn't the JPG used in the ReadMe?

[derwana]

If the extra script bothers you - the script content can be put directly into the YML file.

run: python -c "line one of code; line two of code; etc."

[TheGuyDanish]

It is, but the artifacts of the workflow aren't added to the commit. They're put into the resulting build for download.

[derwana]

oh, my fault - day is already too long for me.