Bare-Metal Micro

Note: This guide is written based on KiCad version 5.1.9.

At a glance…

The following is a screenshot of KiCad Plot dialog showing the correct settings.

The following is a screenshot of KiCad Generate Drill Files dialog showing the correct settings.

Step-by-step

1. Open your design in Pcbnew.
2. Select Place -> Drill and Place Offset to place the auxillary axis origin at the bottom left corner of the board.
3. Select File -> Plot… to open the Plot dialog.
4. Choose Gerber as the Plot format.
5. Set the output directory to something meaningful, such as, gerber/
6. Make sure the following layers are included:
   • F.Cu, Front copper layer
   • B.Cu, Back copper layer
   • F.SilkS, Front silkscreen
   • B.SilkS, Back silkscreen
   • F.Mask, Front solder mask
   • B.Mask, Back solder mask
   • Edge.Cuts, Board outline
7. Under General Options, only the following options should be selected:
   • Plot footprint values
   • Plot footprint references
   • Exclude PCB edge layer from other layers
   • Exclude pads from silkscreen
   • Use auxilary axis as origin
   • Check zone fills before plotting
8. Set Default line width to 0.1 mm.
9. Under Gerber Options, only the following options should be selected:
   • Use extended X2 format
10. Choose 4.6, unit mm for the Coordinate format.
11. It’s probably a good idea to click Run DRC… one last time before generating the files.
12. Click Plot to generate the Gerber files.
13. Output Messages should indicate that a plot file was created for each of the layers.
14. Click Generate Drill Files… to open the Generate Drill Files dialog.
15. Make sure the Ouput folder is the same as the Gerber output directory.
16. Select Excellon as the Drill File Format.
17. None of the checkboxes should be checked under Drill File Format.
18. Select Use route command under Oval Holes Drill Mode.
19. Select Auxilary axis under Drill Origin.
20. Select Inches under Drill Units.
21. Select Decimal format under Zeros format.
22. Click Generate Drill File to generate the drill files.
23. Messages should indicate that two drill files were created. One for plated through holes and one for non-plated through holes.
24. Click Close to close the Generate Drill Files dialog.
25. Click Close to close the Plot dialog.
26. Select File -> Save to save the plot settings.
27. A zip file can now be created with all the files that were generated in the output directory.