Altium

November 11, 2018
2 minute read.

Gerber Export Guide

This article describes the preferred method for generating Gerber and Drill files to print circuits on the Voltera V-One. Before proceeding, it is recommended to read the Circuit Design Guidelines.

Note: Screenshots are of Altium Designer 13.2 running on Windows 8.1. The exact names of the settings presented may differ based on the Altium Designer version, operating system, and circuit design in question.

Exporting Gerber Files

From the .PcbDoc file, navigate to File > Fabrication Outputs > Gerber Files.

General Tab

Select either Millimeters, 3:5 (preferred) OR Inches, 2:5

Layers Tab

Under Layers to Plot check Plot the Top Layer, Top Paste, Bottom Layer and Bottom Paste. This will generate GTL, GTP, GBL and GBP files. You will not need all of these files for every circuit, but exporting them all simplifies this process. Ensure that Mirror is not checked for any of the selected layers.

Drill Drawings Tab

No options should be checked. Drilling information will be exported later.

Apertures Tab

Check Embedded apertures (RS274X)

Advanced Tab

Use the default values for Film Size.

Under Aperture Matching Tolerances, set Plus and Minus to 0.005mil.

Under Batch Mode, select Separate file per layer.

Under Leading/Trailing Zeroes, select Suppress leading zeros.

Under Position on Film, select Reference to relative origin.

Under Plotter Type, select Unsorted (raster).

Under Other:

  • Uncheck G54 on aperture change

  • Uncheck Use software arcs

  • Check Optimize change location commands

  • Check Generate DRC Rules export file (.RUL)

Completing the Export

To export the Gerber files, click OK. The exported files can be found in the the same location as your .PcbDoc file under the Project Outputs for <YourProjectName> folder. CAMtastic will also be launched and can be used to inspect the exported Gerbers, close it when you are ready to proceed. We do not recommend using CAMtastic to (re)export files.

Exporting NC Drill Files

From the .PcbDoc file (not CAMtastic), navigate to File > Fabrication Outputs > NC Drill Files.

Use the same settings as Gerber Export for:

  • Units
  • Format
  • Leading/Trailing Zeros
  • Coordinate Positions

Under Other:

  • Uncheck Use drilled slot command (G85)
  • Uncheck Generate Board Edge Rout Paths
  • Check Optimize change location commands
  • Check Generate separate NC Drill files for plated & non-plated holes
  • Check Generate EIA Binary Drill File (.DRL)

When ready, click OK to export the drill files. As before, CAMtastic may be launched and can be used to inspect the exported Gerbers, close it when you are ready to proceed. We do not recommend using CAMtastic to (re)export files.

Can't find something?

Let us know. We can help.