
== Generating outputs

KiCad can generate and export files in a number of different formats useful for manufacturing PCBs
and interfacing with external software.  This functionality is available in the File menu in a few
different sections.

* The **Fabrication Outputs** section contains the most common operations needed to prepare a PCB for fabrication.
* The **Export** section contains tools for generating files that can be read by external software.
* The **Plot** function allows you to export 2D line drawings of the PCB in various formats.
* The **Print** function allows you to send a view of the PCB to a 2D printer.

=== Fabrication outputs and plotting

KiCad uses Gerber files as its primary plotting format for PCB manufacturing.  To create Gerber
files, open the **Plot...** dialog from the **File** menu, or select **Gerbers (.gbr)...** from the
**Fabrication Outputs** section of the **File** menu.  The Plot dialog will open, allowing you to
configure and generate Gerber files.

image::images/plot_dialog.png[scaledwidth="70%"]

The **Plot** button generates output files according to the selected options. Messages from the plotting
process are shown in the Output Messages panel, and can be filtered by the checkboxes.

The **Generate Drill Files...** button opens the <<drill-files,Generate Drill Files dialog>>. **Run DRC...** 
opens the <<design-rule-checking,Design Rules Checker>>.

==== Plotting options

* **Include Layers:** Check that every layer used on your board is enabled in the list.  Disabled
  layers will not be plotted.

* **Plot on All Layers:** Selected layers will be included in the plot for each layer selected in the
  **include layers** list. The additional layers are plotted on top of the base layer. You can
  reorder these layers using the arrow buttons at the bottom; items that are lower in the list are
  plotted after (on top of) items that are higher in the list.

* **Output directory:** Specify the location to save plotted files.  If this is a relative path, it
  is created relative to the project directory. Use the image:images/icons/small_new_window_16.png[] button
  to open the output directory in a file browser.

* **Plot drawing sheet:** If enabled, the drawing sheet border and title block will be
  plotted on each layer.  This should usually be disabled when plotting Gerber files.

* **Subtract soldermask from silkscreen:** When enabled, silkscreen will be automatically removed
  from board areas that aren't covered by soldermask.

* **Indicate DNP on fabrication layers:** If enabled, fabrication layers (`F.Fab` and `B.Fab`) will
  indicate when a footprint has the DNP (Do Not Populate) attribute set. DNP footprints
  are either not plotted on the fabrication layers (**Hide**) or are plotted with an X drawn through them
  on the front and back fabrication layer (**Cross-out**).

* **Sketch pads on fabrication layers:** If enabled, the outlines of footprint pads will be drawn on
  fabrication layers (`F.Fab` or `B.Fab`). If **Include pad numbers** is enabled, pad numbers will be
  drawn as well.

* **Drill marks:** For plot formats other than Gerber, marks may be plotted at the location of all
  drilled holes.  Drill marks may be created at the actual size (diameter) of the finished hole, or
  at a smaller size.

* **Scaling:** For plot formats that support scaling other than 1:1, the plot scale may be set.  The
  Auto scaling setting will scale the plot to fit the specified page size.

* **Plot mode:** For some plot formats, filled shapes may be plotted as outlines only (sketch mode).

* **Use drill/place file origin:** When enabled, the coordinate origin for plotted files will be the
  drill/place file origin set in the board editor.  When disabled, the coordinate origin will be the
  absolute origin (top left corner of the worksheet).

* **Mirrored plot:** For some plot formats, the output may be mirrored horizontally when this option
  is set.

* **Negative plot:** For some plot formats, the output may be set to negative mode.  In this mode,
  shapes will be drawn for the empty space inside the board outline, and empty space will be left
  where objects are present in the PCB.

* **Check zone fills before plotting:** When enabled, zone fills will be checked (and refilled if
  outdated) before generating outputs.  Plot outputs may be incorrect if this option is disabled!

NOTE: Versions of KiCad before 9.0 had a global control for tenting vias while plotting. In KiCad 9.0,
      via tenting is globally controlled in <<board-setup,Board Setup>>, and can be overridden in the
      <<track-and-via-properties,properties dialog>> for each via.

==== Gerber options

* **Use Protel filename extensions:** When enabled, the plotted Gerber files will be named with file
  extensions based on Protel (`.GBL`, `.GTL`, etc).  When disabled, the files will have the `.gbr`
  extension.

* **Generate Gerber job file:** When enabled, a Gerber job file (`.gbrjob`) will be generated along
  with any Gerber files.  The Gerber job file is an extension to the Gerber format that includes
  information about the PCB stackup, materials, and finish.  More information about Gerber job files
  is available at link:https://www.ucamco.com/en/gerber/gerber-job-file[the Ucamco website].

* **Coordinate format:** Configure how coordinates will be stored in the plotted Gerber files.  Check
  with your manufacturer for their recommended setting for this option.

* **Use extended X2 format:** When enabled, the plotted Gerber files will use the X2 format, which
  includes information about the netlist and other extended attributes.  This format may not be
  compatible with older CAM software used by some manufacturers.

* **Include netlist attributes:** When enabled, the plotted Gerber files will include netlist
  information that can be used for checking the design in CAM software.  When X2 format mode is
  disabled, this information is included as comments in the Gerber files.

* **Disable aperture macros:** When enabled, all shapes will be plotted as primitives rather than by
  using aperture macros.  This setting should only be used for compatibility with old or buggy CAM
  software when requested by your manufacturer.

==== PostScript options

* **Scale factor:** Controls how coordinates in the board file will be scaled to coordinates in the
  PostScript file.  Using a different value for X and Y scale factors will result in a stretched / 
  distorted output.  These factors may be used to correct for scaling in the PostScript output device
  to achieve an exact-scale output.

* **Track width correction:** A global factor that is added (or subtracted, if negative) from the
  size of tracks, vias, and pads when plotting a PostScript file.  This factor may be used to correct
  for errors in the PostScript output device to achieve an exact-scale output.

* **Force A4 output:** When enabled, the generated PostScript file will be A4 size even if the KiCad
  board file is a different size.

==== SVG options

* **Precision:** Controls how many significant digits will be used to store coordinates.

* **Output mode:** Controls whether the generated SVG file is in color or black and white.

* **Fit page to board:** When enabled, the generated SVG will have the same size as the board outline.

==== DXF options

* **Plot graphic items using their contours:** Graphic shapes in DXF files have no width.  This
  option controls how graphic shapes with a width (thickness) in a KiCad board are plotted to a DXF
  file.  When this option is enabled, the outer contour of the shape will be plotted.  When this
  option is disabled, the centerline of the shape will be plotted (and the shape's thickness will not
  be visible in the resulting DXF file).

* **Use KiCad font to plot text:** When enabled, text in the KiCad design will be plotted as graphic
  shapes using the KiCad font.  When disabled, text will be plotted as DXF text objects, which will
  use a different font and will not appear in exactly the same position and size as shown in the
  KiCad board editor.

* **Export units:** Controls the units that will be used in the DXF file.  Since the DXF format has
  no specified units system, you must export using the same units setting that you want to use for
  importing into other software.

==== HPGL options

* **Default pen size:** Controls the plotter pen size used to create graphics.

==== PDF options

* **Output mode:** Controls whether the generated PDF file is in color or black and white.

* **Generate property popups for front footprints:** When enabled, interactive popups will be added
  to the generated PDF containing part information for each footprint on the front of the board.

* **Generate property popups for back footprints:** When enabled, interactive popups will be added
  to the generated PDF containing part information for each footprint on the back of the board. For
  details, see the xref:../eeschema/eeschema_generating_outputs#interactive-pdf-features[Schematic Editor documentation].

* **Generate metadata from AUTHOR and SUBJECT variables:** Sets the Author and
  Subject PDF document properties for the generated PDF based on the `AUTHOR`
  and `SUBJECT` <<board-setup-text-variables,project text variables>>, if you have
  defined them.

* **Single document:** When enabled, each layers will be plotted as an individual sheet within a single
  PDF document. When disabled, each layer will be plotted as a separate PDF file.

[[drill-files]]
=== Drill files

KiCad can generate CNC drilling files required by most PCB manufacturing processes in either
Excellon or Gerber X2 format.  KiCad can also generate a drill map: a graphical plot of the board
showing drill locations.  To open the dialog, select the **Drill Files (.drl)...** option from the
**Fabrication Outputs** section of the **File** menu, or click the **Generate Drill Files...**
button in the Plot dialog.

image::images/generate_drill_files_dialog.png[scaledwidth="70%"]

* **Output folder:** Choose the folder to save generated drill and map files to.  If a relative path
  is entered, it will be relative to the project directory.

* **Drill file format:** Choose whether to generate Excellon drill files (required by most PCB
  manufacturers) or Gerber X2 files.

* **Mirror Y axis:** For Excellon files, choose whether or not to mirror the Y-axis coordinate.  This
  option should in general not be used when having PCBs manufactured by a third party, and is
  provided for convenience for users who are making PCBs themselves.

* **Minimal header:** For Excellon files, choose whether to output a minimal header rather than a
  full file header.  This option should not be enabled unless requested by your manufacturer.

* **PTH and NPTH in single file:** By default, plated holes and non-plated holes will be generated in
  two different Excellon files.  With this option enabled, both will be merged into a single file.
  This option should not be enabled unless requested by your manufacturer.

* **Use alternate drill mode for oval holes:** Controls how oval holes are represented in an Excellon
  drill file. When not enabled, a route command is used to represent oval holes. This is correct for
  most manufacturers. Only choose the **Use alternate drill mode** setting if requested by your
  manufacturer.

* **Generate map:** Choose whether to generate a drill map and, if so, in which format. Supported formats
  are Postscript, Gerber X2, DXF, SVG, and PDF.

* **Origin:** Choose the coordinate origin for drill files.  **Absolute** will use the page 
  origin at the top left corner.  **Drill/place file origin** will use the origin specified in the
  board design.

* **Drill units:** Choose the units for drill coordinates and sizes.

* **Zeros:** Controls how zeroes are formatted in an Excellon drill file.  Select an option
  here based on your manufacturer's recommendations.

[[ipc-2581-export]]
=== IPC-2581 files

IPC-2581 files are XML files that contain complete fabrication and assembly data for a board design.
If your manufacturer accepts IPC-2581 files, these can replace Gerber files, drill files, and
component placement files. To create an IPC-2581 file, select **IPC-2581 File (.xml)...** from the
**Fabrication Outputs** section of the **File** menu.

image::images/generate_ipc_2581_files_dialog.png[scaledwidth="70%"]

IPC-2581 output has the following options:

* **File:**  Choose the filename for the generated IPC-2581 file. If a relative path is entered, it will be relative to the project directory.

* **Units:** Choose the units for the generated file. Can be **millimeters** or **inches**.

* **Precision:** Choose the number of digits after the decimal point for numbers in the generated file.

* **Version:** Choose the IPC-2581 standard version (B or C).

* **Compress output:** If enabled, the generated file will be compressed as a ZIP file.

* **Internal ID:** Choose the footprint field to use for the BOM's internal ID column. This can be a generated unique ID or set to any footprint field in the design.

* **Manufacturer P/N:** Choose the footprint field to use for the BOM's manufacturer part number column. This can be omitted or set to any footprint field in the design.

* **Manufacturer:** Choose the footprint field to use for the BOM's manufacturer column. This can be
  omitted or set to any footprint field in the design.

* **Distributor P/N:** Choose the footprint field to use for the BOM's distributor part number column. This can be omitted or set to any footprint field in the design.

* **Distributor:** Choose the footprint field to use for the BOM's distributor column. This can be omitted or set to any footprint field in the design.

[[odb-export]]
=== ODB{pp} files

ODB{pp} output is a database of files that contains complete fabrication and
assembly data for a board design. If your manufacturer accepts ODB{pp} files,
these can replace Gerber files, drill files, and component placement files. To
create an ODB{pp} file, select **ODB{pp} Output File...** from the
**Fabrication Outputs** section of the **File** menu.

image::images/odb.png[]

ODB{pp} output has the following options:

* **Output file:**  Choose the filename for the generated ODB{pp} file. If a relative path is entered, it will be relative to the project directory.
* **Units:** Choose the units for the generated file. Can be **millimeters** or **inches**.
* **Precision:** Choose the number of digits after the decimal point for numbers in the generated file.
* **Compression format:** Choose the type of compression for the generated output. Can be **ZIP**, **TGZ**, or **none**. If none, the output will be a folder.

=== Component placement files

Component placement files are text files that list each component (footprint) on the board along
with its center position and orientation.  These files are usually used for programming
pick-and-place machines, and may be required by your manufacturer if you are ordering
fully-assembled PCBs. To create placement files, select **Component Placement (.pos, .gbr)...**
from the **Fabrication Outputs** section of the **File** menu.

NOTE: A footprint will not appear in generated placement files if the "Exclude from position files"
      option is enabled for that footprint.  This may be used for excluding certain footprints that
      do not represent physical components to be assembled. You can also optionally exclude DNP
      components, depending on your manufacturer's requirements.

image::images/generate_placement_files_dialog.png[scaledwidth="70%"]

* **Format:** Choose between generating a plain text (ASCII), comma-separated text (CSV), or Gerber
  X3 placement file format.

* **Units:** Choose the units for component locations in the placement file.

* **Include only SMD footprints:** When enabled, only footprints with the SMD fabrication attribute
  will be included.  Check with your manufacturer to determine if non-SMD footprints should be
  included or excluded from the position file.

* **Exclude all footprints with through hole pads:** When enabled, footprints will be excluded from
  the placement file if they contain any through-hole pads, even if their fabrication type is set to
  SMD.

* **Exclude all footprints with the Do Not Populate flag set:** When enabled, footprints will be
  excluded from the placement file if they have the Do Not Populate attribute set. Check with your
  manufacturer to determine if DNP components should be included or excluded from the position file.

* **Include board edge layer:** For Gerber placement files, controls whether or not the board outline
  is included with the footprint placement data.

* **Use drill/place file origin:** When enabled, component positions will be relative to the 
  drill/place file origin set in the board design.  When disabled, the positions will be relative to
  the page origin (upper left corner).

* **Use negative X coordinates for footprints on bottom layer:** When enabled, the X coordinates will
  be flipped (negated) for footprints on the bottom layer.

* **Generate single file with both front and back positions:** When enabled, positions for front and back
  footprints will be saved in a single file. When disabled, separate files will be generated for front and
  back footprints.

=== Additional fabrication outputs

KiCad can also generate footprint report files, IPC-D-356 netlist files, and a bill of materials
(BOM) from the board design.  These output formats have no configurable options.

To generate an output in one of these formats, select the appropriate format in the **File** -> **Fabrication Outputs** menu.

NOTE: The PCB BOM export tool is included for legacy reasons and may be removed in a future version
      of KiCad. It is recommended to use the xref:../eeschema/eeschema.adoc#bom-export[Schematic Editor BOM tool]
      to generate a BOM instead.

=== Printing

KiCad can print the board view to a standard printer using the Print action in the File menu.

image::images/print_dialog.png[scaledwidth="70%"]

* **Include layers:** Select the layers to include in the printout.  Unselected layers will be
  invisible. Right-click the list for layer selection commands.

* **Output mode:** Choose whether to print in black and white or full color.

* **Print drawing sheet:** When enabled, the page border and title block will be printed.

* **Print according to objects tab of appearance manager:** When enabled, any objects that have been
  hidden in the Objects tab of the Appearance panel will be hidden in the printout.  When disabled,
  these objects will be printed if the layer they appear on is selected in the Included Layers area.

* **Print background color:** When printing in full color, this option controls whether or not the
  view background color will be printed.

* **Use a different color theme for printing:** When printing in full color, this option allows a
  different color theme to be used for printing.  When disabled, the color theme used by the board
  editor will be used for printing.

* **Drill marks:** Controls whether to show drilled holes at their actual size, at a small size, or
  hide them from the printout.

* **Print mirrored:** When enabled, the printout will be mirrored horizontally.

* **Print one page per layer:** When enabled, each layer selected in the Included Layers area will be
  printed to an individual page.  If this option is enabled, the **Print board edges on all pages**
  option controls whether to add the Edge.Cuts layer to each printed page.

* **Scale:** controls the scale of the printout relative to the page size configured in Page Setup.

=== Exporting files

KiCad can export a board design to various third-party formats for use with external software.
These functions are found in the **Export** section of the **File** menu.

==== Specctra DSN exporter

The Specctra DSN exporter creates a file suitable for importing into certain third-party autorouter
software.  This exporter has no configurable options.

==== GenCAD exporter

The GenCAD exporter creates a GenCAD file for fabrication, testing, or importing into other software.

image::images/gencad_exporter.png[]

The GenCAD exporter has several options.

* **Flip bottom footprint padstacks:** If enabled, separate flipped padstack definitions will be added
  for bottom-side footprints. This may be necessary for importing into some third-party software.

* **Generate unique pin names:** If enabled, a suffix will be added to each pin name so that no
  footprint in the generated file will have two pins with the same name.

* **Generate a new shape for each footprint instance:** If enabled, a unique footprint will be output
  for every footprint instance, even if two footprints are identical.

* **Use drill/place file origin as origin:** If enabled, coordinates in the generated file will be
  relative to the drill/place file origin.

* **Save the origin coordinates in the file:** If enabled, the selected origin coordinates will be
  included in the generated file. If not enabled, the origin in the generated file will be set to (0,0).

[[vrml-exporter]]
==== VRML exporter

The VRML exporter creates a VRML (`.wrl`) 3D model file containing the PCB and any VRML files
specified in footprints. VRML models are suitable for use in applications where visual appearance is
important and dimensional accuracy is not critical.

image::images/vrml_exporter.png[]

The VRML exporter has several options.

* **Coordinate origin options:** Selects the origin for the generated model. If **user defined origin**
  is selected, you can manually specify the origin point.

* **Units:** Selects the unit system for the generated model. Dimensions in the
  generated model will be scaled appropriately.

* **Ignore 'Do not populate' components:** If enabled, VRML files for footprints with the 'Do not populate'
  attribute set will not be included.

* **Ignore 'Unspecified' components:** If enabled, VRML files for footprints with the 'Unspecified' footprint
  type will not be included.

* **Copy 3D model files to 3D model path:** If enabled, VRML files referenced in footprints will be copied
  into a subdirectory of the directory containing the generated board VRML model, and the generated model
  will reference the copied files. The subdirectory name is set by the **footprint 3D model path** field.
  If disabled, VRML files referenced in footprints will be embedded in the generated VRML files.

* **Use relative paths to model files in board VRML file:** If enabled, references to external models will
  use paths relative to the generated board VRML file. If disabled, the references will use absolute paths.
  This option is only available when the **copy 3D model files to 3D model path** option is enabled.

[[idf-exporter]]
==== IDF exporter

The IDF exporter exports an
http://www.simplifiedsolutionsinc.com/images/idf_v30_spec.pdf[IDFv3] compliant
board (`.emn`) and library (`.emp`) file for communicating mechanical dimensions
to a mechanical CAD package. The exporter exports the board outline and cutouts,
all pad and mounting through holes including slotted holes, and component
outlines; this is the most basic set of mechanical data required for interaction
with mechanical designers. All other entities described in the IDFv3
specification are currently not exported.

NOTE: You must attach IDF component models to your design's footprints before
they will be included in the exported model. For more information on attaching
models to footprints, see the <<creating-and-editing-footprints,footprint
documentation>>. Some IDF-specific guidance is included in the
<<idf-component-outlines,Advanced Topics documentation>>.

NOTE: For more information on creating IDF component models, including descriptions
of the IDF utility tools included with KiCad, see the
<<idf-component-outlines,Advanced Topics documentation>>.

Once models have been specified for all desired components, the model of the
board can be exported. In the PCB Editor, select **File** -> **Export** ->
**IDFv3...**.

image::images/idf_export.png[scaledwidth="70%",alt="IDF output settings"]

* **Grid reference point:** Choose where the exported model's reference point
  should be. If the **Adjust automatically** option is selected, KiCad will set
  the reference point to the centroid of the PCB. Otherwise, the reference point
  is set relative to the display origin.

* **Output units:** Choose whether the exported model's units are millimeters or
  mils.

* **Ignore 'Do not populate' components:** If enabled, IDF files for footprints with the 'Do not populate'
  attribute set will not be included.

* **Ignore 'Unspecified' components:** If enabled, IDF files for footprints with the 'Unspecified' footprint
  type will not be included.

The outputs can be viewed directly in a mechanical CAD application or converted
to VRML using the <<idf2vrml,`idf2vrml` tool>>.

[[_3d-export]]
==== 3D model exporter (STEP / GLB / BREP / XAO / PLY / STL)

The 3D model exporter creates a 3D model file from the PCB and any STEP files specified in
footprints. A number of formats are supported:

* STEP
* GLB (binary glTF)
* BREP (OCCT-native boundary representation)
* XAO (SALOME/Gmsh)
* PLY
* STL

Different formats may be appropriate for different usecases. For example, STEP models are suitable for use
in mechanical CAD applications, while XAO models are useful for physical simulations.

NOTE: KiCad's footprint library includes both STEP and VRML (`.wrl`) versions of each model.
      However, footprints in KiCad's library only reference the VRML versions of the models.
      VRML models are not included in STEP exports, but the STEP exporter will instead include
      the corresponding STEP version of the model if the **subsitute similarly named models**
      option is enabled.

NOTE: KiCad can also export 3D models in <<vrml-exporter,VRML>> and <<idf-exporter,IDF>> formats,
      but these formats use separate exporters.

To use the 3D model exporter, click **File** -> **Export** -> **STEP / GLB / BREP / XAO / PLY / STL...**.

image::images/step_exporter.png[]

* **Format:** Selects the output format.

===== Board options

* **Export board body:** If enabled, the board body (non-copper) will be modeled in the exported model.

* **Cut vias in board body:** If enabled, via holes will be cut in the board body even if conductor layers
  are not modeled.

* **Export silkscreen:** If enabled, silkscreen will be modeled in the exported model.
  Silkscreen is modeled as a set of flat faces; it is not three-dimensional.

* **Export solder mask:** If enabled, solder mask will be modeled in the exported model.
  Solder mask is modeled as a set of flat faces; it is not three-dimensional.

* **Export components:** If enabled, 3D models for components will be included in the exported model (but see
  **Substitute similarly named models**, below). If **All components** is selected, models for all components in
  the PCB will be included. If **Only selected** is chosen, only models for the footprints currently selected in
  the board will be included. If **Components matching filter** is selected, only models for footprints with
  references matching the filter will be included. The filter supports wildcards and commas, so `C1,R*` will
  include `C1` and all resistors.

===== Conductor options

* **Export tracks and vias:** If enabled, tracks and vias on outer layers will
  be modeled in the exported model.

* **Export pads:** If enabled, pads will be modeled in the exported model.

* **Export zones:** If enabled, zones on outer layers will be modeled in the exported
  model.

* **Export inner conductor layers:** If enabled, inner conductor layers will be modeled in
  the exported model.

* **Fuse shapes (time consuming):** If enabled, intersecting geometry will be fused into
  a single shape. This may make the exported file easier to work with in some tools, but it
  also significantly increases the export time.

* **Fill all vias:** If enabled, via holes will not be cut in conductor layers.

* **Net filter (supports wildcards):** If filled, only conductors corresponding to nets that
  match the filter will be modeled. The filter supports wildcards, so `/tx_*`
  will model `/tx_p` and `/tx_n` conductors.

===== Coordinates

* **Coordinates:** Selects the origin for the generated model. If **user defined origin**
  is selected, you can manually specify the origin point.

===== Other options

* **Ignore 'Do not populate' components:** If enabled, components with the DNP attribute set
  will not be included in the exported model.

* **Ignore 'Unspecified' components:** If enabled, components with the Unspecified footprint
  type will not be included in the exported model.

* **Substitute similarly named models:** VRML models cannot be used in STEP, BREP, or XAO exports, but
  if this option is enabled the exporter will look for an identically named STEP model to include
  in the export instead of a footprint's specified VRML model. Note that footprints in KiCad's
  footprint library specify VRML models, but suitably named STEP models are also included for each
  VRML model. Therefore this option must be enabled in order to export 3D models for footprints
  from KiCad's library using this dialog.

* **Overwrite old file:** If enabled, the exported model will overwrite an existing file
  with the same name.

* **Don't write P-curves to STEP file** If enabled, parametric curves will be disabled in the exported
  STEP model. This reduces the file size, but may reduce compatibility with some software.

* **Board outline chaining tolerance:** Controls the minimum distance between two points for
  the points to be considered coincident. If the board outline in the exported model is
  not contiguous, try increasing this tolerance.

==== Footprint association (CMP) exporter

CMP files are used to sync footprint assignments and some other footprint fields between the PCB
and the schematic. You can import CMP files into the schematic using the schematic editor's
**File** -> **Import** -> **Footprint Assignments** menu item. This provides a very limited form of
xref:../eeschema/eeschema.adoc#backannotation[back annotation]. It is recommended to use the
Update Schematic from PCB tool instead.

This exporter has no configurable options.

==== Hyperlynx exporter

The Hyperlynx exporter creates a file suitable for importing into Mentor Graphics (Siemens) HyperLynx
simulation and analysis software. This exporter has no configurable options.
