Finished the options documentation

2020-03-24 12:18:21 -03:00 · 2020-03-24 12:18:21 -03:00 · 64ab20e68e
parent 397cae4373
commit 64ab20e68e
1 changed files with 147 additions and 1 deletions
--- a/README.md
+++ b/README.md
@ -79,7 +79,7 @@ The available values for *type* are:
 - Plot formats:
    - `gerber` the gerbers for fabrication.
    - `ps` postscript plot
-    -`hpgl` format for laser printers
+    - `hpgl` format for laser printers
    - `svg` scalable vector graphics
    - `pdf` portable document format
    - `dxf` mechanical CAD format
@ -95,6 +95,152 @@ The available values for *type* are:
    - `kibom` BoM in HTML or CSV format generated by [KiBoM](https://github.com/INTI-CMNB/KiBoM)
    - `ibom` Interactive HTML BoM generated by [InteractiveHtmlBom](https://github.com/INTI-CMNB/InteractiveHtmlBom)

+Here is an example of a configuration file to generate the gerbers for the top and bottom layers:
+
+```
+kiplot:
+  version: 1
+
+preflight:
+  run_drc: true
+
+outputs:
+
+  - name: 'gerbers'
+    comment: "Gerbers for the board house"
+    type: gerber
+    dir: gerberdir
+    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
+      check_zone_fills: 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:
+      - layer: F.Cu
+        suffix: F_Cu
+      - layer: B.Cu
+        suffix: B_Cu
+```
+
+Most options are the same you'll find in the KiCad dialogs.
+
+### General options for plot formats
+
+- `exclude_edge_layer` do not include the PCB edge layer
+- `exclude_pads_from_silkscreen` do not plot the component pads in the silk screen
+- `plot_sheet_reference` currently without effect
+- `plot_footprint_refs` include the footprint references
+- `plot_footprint_values` include the footprint values
+- `force_plot_invisible_refs_vals` include references and values even when they are marked as invisible
+- `tent_vias` cover the vias
+- `check_zone_fills` currently without effect
+
+Note that each layer is generated in a separated file.
+
+### Gerber options
+
+- `line_width` for objects without width (floating point value in mm)
+- `use_aux_axis_as_origin` use the auxiliar axis as origin for coordinates
+- `subtract_mask_from_silk` substract the solder mask from the silk screen
+- `use_protel_extensions` use legacy Protel file extensions
+- `gerber_precision` this the gerber coordinate format, can be 4.5 or 4.6
+- `create_gerber_job_file` creates a file with information about all the generated gerbers. You can use it in *gerbview* to load all gerbers at once.
+- `use_gerber_x2_attributes` use the extended X2 format
+- `use_gerber_net_attributes` include netlist metadata
+
+### PS options
+
+- `line_width` for objects without width (floating point value in mm)
+- `mirror_plot` plot mirrored
+- `negative_plot` invert black and white
+- `scaling` scale factor
+- `drill_marks` what to use to indicate the drill places, can be `none`, `small` or `full` (for real scale)
+- `scale_adjust_x` fine grain adjust for the X scale (floating point multiplier)
+- `scale_adjust_y` fine grain adjust for the Y scale (floating point multiplier)
+- `a4_output` force A4 paper size
+
+### SVG and PDF options
+
+- `line_width` for objects without width (floating point value in mm)
+- `mirror_plot` plot mirrored
+- `negative_plot` invert black and white
+- `drill_marks` what to use to indicate the drill places, can be `none`, `small` or `full` (for real scale)
+
+### HPGL options
+
+- `mirror_plot` plot mirrored
+- `scaling` scale factor
+- `drill_marks` what to use to indicate the drill places, can be `none`, `small` or `full` (for real scale)
+- `pen_width` default trace width
+
+### DXF options
+
+- `drill_marks` what to use to indicate the drill places, can be `none`, `small` or `full` (for real scale)
+- `polygon_mode` plot using the contour, instead of the center line
+
+### General drill options
+
+- `use_aux_axis_as_origin` use the auxiliar axis as origin for coordinates
+- `map` this is an optional subsection to indicate the format for a graphical drill map.
+The valid formats are `hpgl`, `ps`, `gerber`, `dxf`, `svg` and `pdf`. Example:
+```
+      map:
+        type: 'pdf'
+```
+- `report` this is an optional subsection to indicate the name of the drill report, example:
+```
+      report:
+        filename: 'Project-drl.rpt'
+```
+
+### Excellon drill options
+
+- `metric_units` use metric units instead of inches.
+- `pth_and_npth_single_file` generate one file for both, plated holes and non-plated holes, instead of two separated files.
+- `minimal_header` use a minimal header in the file
+- `mirror_y_axis` invert the Y axis
+
+### Position options
+
+- `format` can be `ascii` or `csv`.
+- `units` can be `millimeters` or `inches`.
+- `separate_files_for_front_and_back` generate two separated files, one for the top and another for the bottom.
+- `only_smd` only include the surface mount components.
+
+### pdf_pcb_print options
+
+- `output_name` filename for the output PDF
+
+### KiBoM options
+
+- `format` can be `html` or `csv`.
+
+### IBoM options
+
+- `blacklist` regular expression for the components to exclude (using the Config field)
+- `name_format` format of the output name, example: `%f_%r_iBoM` will generate a file with revision and *_iBoM*.
+
+### pdf_sch_print options
+
+- `output` filename for the output PDF
+
+
 ## Using KiPlot

 You can call `kiplot` directly, passing a PCB file and a config file: