From 64ab20e68e4acadf4134cc846620753bd02fd551 Mon Sep 17 00:00:00 2001 From: "Salvador E. Tropea" Date: Tue, 24 Mar 2020 12:18:21 -0300 Subject: [PATCH] Finished the options documentation --- README.md | 148 +++++++++++++++++++++++++++++++++++++++++++++++++++++- 1 file changed, 147 insertions(+), 1 deletion(-) diff --git a/README.md b/README.md index 685f1996..4afd4a48 100644 --- 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: