NC Drill Output Options
The NC Drill Setup Dialog
The NC Drill Setup dialog provides you with tools to completely configure your NC Drill file output options.
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.
The format specifies the precision of the coordinate data, which must be selected to suit the placement precision of the objects in the PCB workspace. For example, the 2:3 format has a resolution of 1mil (1/1000 inch). If your design has objects placed on a sub-1mil grid then this format will not be adequate. Conversely, the higher precision formats may be more difficult and expensive to photoplot and manufacture.
Zero Suppression
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
If the option to Suppress leading zeroes is enabled, these values will appear in the file as:
1
10.00000
If the option to Suppress trailing zeroes is enabled, these values will appear in the file as:
00.00001
1.
Other Options
In the Other region of the dialog are special options and options for generating special drill files. Enabling the Generate separate NC Drill files for plated & non-plated holes option creates separate drill files for plated and unplated holes. Enabling the Use drilled slot command (G85) option uses multiple drilled holes to create slots. Enabling the Generate Board Edge Rout Paths option creates a separate NC Rout file to define the board shape, including board cutouts. The Rout Tool Dia field allows you to specify the tool size used to rout the board outline.
Generated NC Drill Files
The following table lists each of the NC Drill files that can possibly be generated as output from a PCB document.
| 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 |
| 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 |
| 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 |
| 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. |
Notes
Use the dialog's 'What's This Help' feature to obtain detailed information about each of the options available. Click the ' ? ' button at the top right of the dialog and then click over a field or option to pop-up information specific to that field or option.
NC Drill output can be generated in one of two ways:
- using an appropriately configured output generator defined in an Output Job Configuration file (*.OutJob). Output will be generated upon running the configured output generator
- 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.
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 Output Job Configuration 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 ).
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.
The output path for generated files is set 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.
When 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)).