Drill Table questions

Hi all,

new to kicad. and this forum. I have searched but not found answers to my questions. I have seen there are a few threads talking about drill tables but nothing I found talked about how to add one.

I actually do PCB design and IC layout for a living. I have been using altium for the last 3 years for PCB design. so… one thing I try hard to be really picky about is documentation. I see no way to add a drill table to the FAB drawing (except manually). Do kicad users just not add a drill table? or am I missing some piece of information?

thanks in advance.

1 Like

here is an example.

Drill table

1 Like

Isn’t this what the drill file is for? (part of the gerber export.)
Or do you want to add this for manual drilling of your boards? (The only usecase that comes to mind right now.)

1 Like

I guess it depends on how you think about it? I think… the drill table is a reflection of the drl file.

I have designed 100s of PCB’s with lots of different tools, and all of them had a drill table or sometimes called a drill schedule on the FAB drawing. if you google PCB FAB drawings or PCB drill table you will see its a pretty common practice.

i dont know if its “old school” now.

i am guessing by your answer there is no way to add a drill table (except manually)

thanks in advance

1 Like

In Pcbnew when you plot your Gerber files, at the bottom of the plot dialog there is a button “Generate Drill File” which brings up another dialog. On the right side of the Drill File Generation dialog there are three buttons, “Drill File”, “Map File”, and “Report File”. You can select the map file format.


thanks, I will give that a try when I get home tonight.

There is. When plotting, click the “Generate Drill File” button (between “Plot” and “Close”) to get the drill file generation window. Select your desired output format and click “Map File”.

I quickly did this on one of my (very simple) designs, exporting to Gerber (merging PTH and NPTH) and got the file “FeatherSwitch - v1.0.0-drl_map.gbr”. This is what the resulting Gerber looks like in KiCad’s gerber viewer:

If you need text, there is also a “Report File” button on the drill files generation window that will give you an ASCII report file. Here is the one from this board:
FeatherSwitch - v1.0.0-drl.rpt (802 Bytes)

I hope this is what you are looking for.
(Lol… I see 1.21Gigawatts answered this while I was writing the above.)


thanks guys. that really helps.

do you think this is kind of an out dated practice? i have always done but that doesn’t mean its still needed?


Probably is, but I guess it really depends on the requirements of the board house that you use… I had to break the habit of including a drawing title block and revision table on my fab plots because it confused the automated tools at the hobbiest-level board houses that I’ve been using recently. :smiley:

now… thats just … so uncivilized…

which board house btw?

I include a drill chart, layer stacking cross section (similar to Allegro), notes and an impedance table (where required) on most of my fab prints. Obviously not required for a board using standard stackup.
The drill drill gets copied and pasted straight out of the .rpt file that @SembazuruCDE refers to above.
Impedance tables and notes are just text boxes.
Layer stackups are imported DXFs.

.RPT file info:

To be honest, I forget which one, but it might have been BAC. Automated systems don’t like the title block, page frame, and revision table on all the Gerber layers. Granted, last time before that when I was sending out Gerbers, my company was paying $200 NRE for each artwork layer… I now usually use OSHPark, and they take KiCad board files directly.