NC Drill Setup

Parent page: WorkspaceManager Dialogs

The NC Drill Setup dialog


The NC Drill Setup dialog is used to configure NC Drill file output options.


This dialog can be accessed in the following ways:

  • At the PCB document level, click Outputs | Fabrication » .
  • Click Project | Project Actions |  to access the Generate output files dialog. Click Configure to the right of  NC Drill Files. 
  • At the PCB or schematic document level, click Home | Project |  » Generate outputs to access the Generate output files dialog. Click Configure to the right of NC Drill Files. 
​​When the NC Drill Setup dialog is accessed using the Outputs ribbon command, the NC Drill files are generated immediately. When using the Generate output files dialog to access the dialog, you are only configuring the settings for the NC Drill files.



  • NC Drill Format - specify the units and format to be used in the NC Drill output files.
  • Units
    • Inches - enable this option to use imperial units where all work is done in mils (1/1000 inch).
    • Millimeters - enable this option to use metric units where all work is done in millimeters.
  • Format
    • 2:3 - provides a resolution of 1 mil  (1/1000 inch).
    • 2:4 - provides a resolution of 0.1 mil. 
    • 2:5 - provides a resolution of 0.01 mil. 

If you are using one of the higher resolutions, check that the PCB manufacturer supports that format. The 2:4 and 2:5 formats only need to be chosen if there are holes on a grid finer than 1 mil.

  • Leading/Trailing Zeroes
    • Keep leading and trailing zeroes - if this option is enabled, all leading and trailing zeroes will appear in the generated NC Drill file.
    • Suppress leading zeroes - if this option is enabled, no leading zeroes will appear in the generated NC Drill file.
    • Suppress trailing zeroes - if this option is enabled, no trailing zeroes will appear in the generated NC Drill file.
  • Coordinate Positions 
    • Reference to absolute origin - use the absolute origin as the reference point.
    • Reference to relative origin - use the relative origin as the reference point.
  • Other
    • Optimize change location commands - check this option to optimize change location commands.
    • Generate separate NC Drill files for plated & non-plated holes - check this option to create separate drill files for plated and unplated holes.
    • Use drilled slot command (G85) - check this option to use multiple drilled holes to create slots.
    • Generate Board Edge Rout Paths - check this option to create a separate NC Route file to define the board shape, including board cutouts.
      • Rout Tool Dia - specify the tool size used to route the board outline. This option is available only when Generate Board Edge Rout Paths is enabled.
    • Generate EIA Binary Drill File (.DRL) - use this option to generate a .DRL file. DRL is a binary format drill file. 

The NC Drill files should be created with the same format as the Gerber files. For example, if the Gerber files have been configured to use the 2:4 format, the corresponding NC Drill files should use the same format.

If Gerber files have been generated with the coordinate position on the film set to use either the absolute or relative origin, the NC Drill files should ideally be generated using the same origin reference.

Location of Generated Files

The generated NC Drill files are stored in a folder that is specified in the Options tab of the Options for Project dialog. 


You are reporting an issue with the following selected text and/or image within the active document: