104 lines
8.7 KiB
ReStructuredText
104 lines
8.7 KiB
ReStructuredText
.. Automatically generated by KiBot, please don't edit this file
|
|
|
|
.. index::
|
|
pair: DXF (Drawing Exchange Format); dxf
|
|
|
|
DXF (Drawing Exchange Format)
|
|
~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
|
|
|
|
Exports the PCB to 2D mechanical EDA tools (like AutoCAD).
|
|
This output is what you get from the File/Plot menu in pcbnew. |br|
|
|
If you use custom fonts and/or colors please consult the `resources_dir` global variable. |br|
|
|
|
|
Type: ``dxf``
|
|
|
|
Category: **PCB/export**
|
|
|
|
Parameters:
|
|
|
|
- **comment** :index:`: <pair: output - dxf; comment>` [string=''] A comment for documentation purposes. It helps to identify the output.
|
|
- **dir** :index:`: <pair: output - dxf; dir>` [string='./'] Output directory for the generated files.
|
|
If it starts with `+` the rest is concatenated to the default dir.
|
|
- **layers** :index:`: <pair: output - dxf; layers>` [list(dict)|list(string)|string] [all,selected,copper,technical,user,inners,outers]
|
|
List of PCB layers to plot.
|
|
|
|
- Valid keys:
|
|
|
|
- ``description`` :index:`: <pair: output - dxf - layers; description>` [string=''] A description for the layer, for documentation purposes.
|
|
A default can be specified using the `layer_defaults` global option.
|
|
- ``layer`` :index:`: <pair: output - dxf - layers; layer>` [string=''] Name of the layer. As you see it in KiCad.
|
|
- ``suffix`` :index:`: <pair: output - dxf - layers; suffix>` [string=''] Suffix used in file names related to this layer. Derived from the name if not specified.
|
|
A default can be specified using the `layer_defaults` global option.
|
|
|
|
- **name** :index:`: <pair: output - dxf; name>` [string=''] Used to identify this particular output definition.
|
|
Avoid using `_` as first character. These names are reserved for KiBot.
|
|
- **options** :index:`: <pair: output - dxf; options>` [dict] Options for the `dxf` output.
|
|
|
|
- Valid keys:
|
|
|
|
- **output** :index:`: <pair: output - dxf - options; output>` [string='%f-%i%I%v.%x'] Output file name, the default KiCad name if empty.
|
|
IMPORTANT! KiCad will always create the file using its own name and then we can rename it.
|
|
For this reason you must avoid generating two variants at the same directory when one of
|
|
them uses the default KiCad name. Affected by global options.
|
|
- **plot_sheet_reference** :index:`: <pair: output - dxf - options; plot_sheet_reference>` [boolean=false] Include the frame and title block. Only available for KiCad 6+ and you get a poor result
|
|
(i.e. always the default worksheet style, also problems expanding text variables).
|
|
The `pcb_print` output can do a better job for PDF, SVG, PS, EPS and PNG outputs.
|
|
- **scaling** :index:`: <pair: output - dxf - options; scaling>` [number=1] Scale factor (0 means autoscaling).
|
|
- ``custom_reports`` :index:`: <pair: output - dxf - options; custom_reports>` [list(dict)] A list of customized reports for the manufacturer.
|
|
|
|
- Valid keys:
|
|
|
|
- ``content`` :index:`: <pair: output - dxf - options - custom_reports; content>` [string=''] Content for the report. Use ``${basename}`` for the project name without extension.
|
|
Use ``${filename(LAYER)}`` for the file corresponding to LAYER.
|
|
- ``output`` :index:`: <pair: output - dxf - options - custom_reports; output>` [string='Custom_report.txt'] File name for the custom report.
|
|
|
|
- ``dnf_filter`` :index:`: <pair: output - dxf - options; dnf_filter>` [string|list(string)='_none'] Name of the filter to mark components as not fitted.
|
|
A short-cut to use for simple cases where a variant is an overkill.
|
|
|
|
- ``drill_marks`` :index:`: <pair: output - dxf - options; drill_marks>` [string='full'] [none,small,full] What to use to indicate the drill places, can be none, small or full (for real scale).
|
|
- ``edge_cut_extension`` :index:`: <pair: output - dxf - options; edge_cut_extension>` [string=''] Used to configure the edge cuts layer extension for Protel mode. Include the dot.
|
|
- ``exclude_edge_layer`` :index:`: <pair: output - dxf - options; exclude_edge_layer>` [boolean=true] Do not include the PCB edge layer.
|
|
- ``exclude_pads_from_silkscreen`` :index:`: <pair: output - dxf - options; exclude_pads_from_silkscreen>` [boolean=false] Do not plot the component pads in the silk screen (KiCad 5.x only).
|
|
- ``force_plot_invisible_refs_vals`` :index:`: <pair: output - dxf - options; force_plot_invisible_refs_vals>` [boolean=false] Include references and values even when they are marked as invisible.
|
|
- ``individual_page_scaling`` :index:`: <pair: output - dxf - options; individual_page_scaling>` [boolean=true] Tell KiCad to apply the scaling for each layer as a separated entity.
|
|
Disabling it the pages are coherent and can be superposed.
|
|
- ``inner_extension_pattern`` :index:`: <pair: output - dxf - options; inner_extension_pattern>` [string=''] Used to change the Protel style extensions for inner layers.
|
|
The replacement pattern can contain %n for the inner layer number and %N for the layer number.
|
|
Example '.g%n'.
|
|
- ``metric_units`` :index:`: <pair: output - dxf - options; metric_units>` [boolean=false] Use mm instead of inches.
|
|
- ``plot_footprint_refs`` :index:`: <pair: output - dxf - options; plot_footprint_refs>` [boolean=true] Include the footprint references.
|
|
- ``plot_footprint_values`` :index:`: <pair: output - dxf - options; plot_footprint_values>` [boolean=true] Include the footprint values.
|
|
- ``polygon_mode`` :index:`: <pair: output - dxf - options; polygon_mode>` [boolean=true] Plot using the contour, instead of the center line.
|
|
You must disable it to get the dimensions (See https://gitlab.com/kicad/code/kicad/-/issues/11901).
|
|
- ``pre_transform`` :index:`: <pair: output - dxf - options; pre_transform>` [string|list(string)='_none'] Name of the filter to transform fields before applying other filters.
|
|
A short-cut to use for simple cases where a variant is an overkill.
|
|
|
|
- ``sketch_pad_line_width`` :index:`: <pair: output - dxf - options; sketch_pad_line_width>` [number=0.1] Line width for the sketched pads [mm], see `sketch_pads_on_fab_layers` (KiCad 6+)
|
|
Note that this value is currently ignored by KiCad (6.0.9).
|
|
- ``sketch_pads_on_fab_layers`` :index:`: <pair: output - dxf - options; sketch_pads_on_fab_layers>` [boolean=false] Draw only the outline of the pads on the \\*.Fab layers (KiCad 6+).
|
|
- ``sketch_plot`` :index:`: <pair: output - dxf - options; sketch_plot>` [boolean=false] Don't fill objects, just draw the outline.
|
|
- ``tent_vias`` :index:`: <pair: output - dxf - options; tent_vias>` [boolean=true] Cover the vias.
|
|
- ``uppercase_extensions`` :index:`: <pair: output - dxf - options; uppercase_extensions>` [boolean=false] Use uppercase names for the extensions.
|
|
- ``use_aux_axis_as_origin`` :index:`: <pair: output - dxf - options; use_aux_axis_as_origin>` [boolean=false] Use the auxiliary axis as origin for coordinates.
|
|
- ``variant`` :index:`: <pair: output - dxf - options; variant>` [string=''] Board variant to apply.
|
|
|
|
- **type** :index:`: <pair: output - dxf; type>` 'dxf'
|
|
- ``category`` :index:`: <pair: output - dxf; category>` [string|list(string)=''] The category for this output. If not specified an internally defined category is used.
|
|
Categories looks like file system paths, i.e. **PCB/fabrication/gerber**.
|
|
The categories are currently used for `navigate_results`.
|
|
|
|
- ``disable_run_by_default`` :index:`: <pair: output - dxf; disable_run_by_default>` [string|boolean] Use it to disable the `run_by_default` status of other output.
|
|
Useful when this output extends another and you don't want to generate the original.
|
|
Use the boolean true value to disable the output you are extending.
|
|
- ``extends`` :index:`: <pair: output - dxf; extends>` [string=''] Copy the `options` section from the indicated output.
|
|
Used to inherit options from another output of the same type.
|
|
- ``groups`` :index:`: <pair: output - dxf; groups>` [string|list(string)=''] One or more groups to add this output. In order to catch typos
|
|
we recommend to add outputs only to existing groups. You can create an empty group if
|
|
needed.
|
|
|
|
- ``output_id`` :index:`: <pair: output - dxf; output_id>` [string=''] Text to use for the %I expansion content. To differentiate variations of this output.
|
|
- ``priority`` :index:`: <pair: output - dxf; priority>` [number=50] [0,100] Priority for this output. High priority outputs are created first.
|
|
Internally we use 10 for low priority, 90 for high priority and 50 for most outputs.
|
|
- ``run_by_default`` :index:`: <pair: output - dxf; run_by_default>` [boolean=true] When enabled this output will be created when no specific outputs are requested.
|
|
|