NC Drill Setup

Old Content - visit altium.com/documentation
Modified by Admin on Sep 13, 2017

Parent page: WorkspaceManager Dialogs

The NC Drill Setup Dialog.

Summary

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

Access

NC Drill output can be generated in one of two ways:

  • Using an NC Drill output generator in an OutputJob Configuration file (*.OutJob). Output is generated when the configured output generator is run.
  • Directly from within the active PCB document using the File » Fabrication Outputs » NC Drill Files menu command. Output will be generated immediately upon clicking OK in the NC Drill Setup dialog.

Note : The settings defined in the NC Drill Setup dialog when generating output directly from the PCB are distinct and separate to those defined for the same output type in an Output Job Configuration file. In the case of the former, the settings are stored in the project file, whereas for the latter they are stored in the Output Job Configuration file.

Options/Controls

NC Drill Format 

The NC Drill Format region of the dialog allows you to specify the units and format to be used in the NC Drill output files. The units can be either inches or millimeters.

  • Units
    • Inches - Check this option to use inches as unit
    • Millimeters - Check this option to use millimeters as unit
  • Format
    • 2:3 - The 2:3 format has a resolution of 1 mil  (1/1000 inch).
    • 2:4 - The 2:4 format has a resolution of 0.1 mil 
    • 2:5 - The 2:5 format has a resolution of 0.01 mil 

If you are using one of the higher resolution, you should check that the PCB manufacture 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 Zeros

The Leading/Trailing Zeroes region allows you to determine whether leading or trailing zeros should be suppressed or not. Zero suppression is a technique that reduces the size of the generated data files by removing all zeroes from the start (leading) or end (trailing) of numbers.
For example, consider the generation of NC Drill files with format 2:5 . Using this format can yield the following data values: 00.00001 10.00000

  • Keep leading and trailing zeroes - If this option is enabled, these values will keep as: 00.00001 10.00000
  • Suppress leading zeroes - If this option is enabled, these values will appear in the file as: 1 10.00000
  • Suppress trailing zeroes - If this option is enabled, these values will appear in the file as: 00.00001 1

Coordinate Position 

  • Reference to absolute origin - Take absolute origin as reference point
  • Reference to relative origin - Take relative origin as reference point

Other

In the Other region of the dialog are special options and options for generating special drill files.

  • Optimize change location commands - Check this option to optimize change location commands.
  • Generate separate NC Drill files for plated & non-plated holes - Enable this option to create separate drill files for plated and unplated holes.
  • Use drilled slot command(G85) - Enable this option to use multiple drilled holes to create slots.
  • Generate Board Edge Rout Path- Enable this option to create a separate NC Rout file to define the board shape, including board cutouts.
    • Rout Tool Dia - allows you to specify the tool size used to rout the board outline.
  • Generate EIA Binary Drill File(.DRL) - Check this option to generate .DRL file. DRL is Binary format drill file. For a multi-layer PCB that incorporates blind and/or buried vias, a separate drill file for each layer pair is created, with a unique file extension

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

Generated NC Drill Files

Filename Description
FileName.DRL Binary format drill file. For a multi-layer PCB that incorporates blind and/or buried vias, a separate drill file for each layer pair is created, with a unique file extension
FileName.DRR Drill report - detailing the tool assignments, hole sizes, hole count and tool travel
FileName.TXT ASCII format drill file. Again, for a multi-layer PCB that incorporates blind and/or buried vias, a separate drill file for each layer pair is created, with a unique file extension
FileName-Plated.TXT ASCII format drill file. Specifically for plated holes in a PCB design. A separate file will be created for each hole type - slotted, square or round.
FileName-NonPlated.TXT ASCII format drill file. Specifically for non-plated holes in a PCB design. A separate file will be created for each hole type - slotted, square or round.
FileName-BoardEdgeRout.TXT ASCII format rout file. Specifically for board outline, including board cutouts.
FileName.LDP ASCII format drill pair report. Used by the CAM Editor to detect blind and buried vias.

Once generated, the output will be added to the project and appear in the Projects panel under the Generated folder, in an appropriately-named sub-folder. If you have used a separate folder for each output type, then corresponding (separate) Generated folders will be added to the Projects panel (e.g. Generated (NC Drill Output)).

Location of Generated Files

The output path for generated files depends on how the output was generated:

  • From an OutputJob file - the generated files are stored in a folder within the project folder, the naming and folder structure is defined in the Output Container that the NC Drill File output is targeting.
  • Directly from the PCB -the output path is specified in the Options tab of the Options for Project dialog. By default, the output path is set to a sub-folder under the folder that contains the Project file and has the name: Project Outputs for ProjectName. The output path can be changed as required. If the option to use a separate folder for each output type has been enabled in the Options tab, then the NC Drill files will be written to a further sub-folder, named: NC Drill Output.

Automatically Opening the Generated Output

When generating NC Drill output, you can specify that the output be opened automatically in a new CAM document. The way in which this is accomplished depends on how you are generating the output:

  • From an OutputJob file - enable the NC Drill Output auto-load option in the Output Job Options dialog (Tools » Output Job Options from the OutputJob Editor).
  • Directly from the PCB - ensure that the Open outputs after compile option is enabled on the Options tab of the Options For Project dialog (Project » Project Options).

To add a Drill Table to the Gerber File you place a Drill Table object on the Drill Drawing Layer (Altium Designer 14.3 and newer). For older versions, place the .Legend special string on the Drill Drawing Layer.

 

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