Backdrilling kiCAD 8 or 9

Layout
1

Hi,

I am working on a PCB design that needs backdrilling on certain vias on RF signals. I designed the first rev of the layout using KiCad 8.0. I was excited to learn about the Padstacks feature in KiCAD 9.0. However, I am unable to figure out how to use the existing capability to specify a back drill spec.

I can create a user layer and call out back drill locations on that layer. However, I am don’t know how to convert that information into a .drl file that has the complete specification of the drills including back drilling.

Is there a known method that can be used for this, in either, KiCAD 8 or 9?

Thanks,
Prasoon

2

I think you may try with this workaround:

  • Create footprint with a circular pad for the backdrills just in User.Eco2 (for example) or any custom layer.
  • Add footprint on selected backdrills
  • Plot custom layer using default gerber configuration
  • Open this layer using Kicad Gerber Viewer and Export to PCB Editor without Automatic Layer Assingment.
  • Export selected layer as Hole Data.
  • Open generated PCB file with Kicad and plot drl files as usual.
3

Hi,

Thanks for the suggestion. I have gone through the workflow, but, I think I have only mixed success.

I created a circular pad in the footprint editor on the User.Eco2 layer and B.Cu layer. This pad was specified as a NPTH, mechanical pad with a pad diameter of the required back drill. I kept the padstack as normal. The attributes (refdes, value, description) were assigned to the B.fab layer.

In the PCB editor I instantiated the footprint over one of the through hole vias. I then exported the User.Eco2 layer as a Gerber layer. In the Gerber viewer I exported this layer as “Hole Data”. I open this “kicad_pcb” file in the PCB Editor and generate a drill report. I now see a lot of drills and not just the one that I was expecting. I also see that the exported “kicad_pcb” shows a different orientation.

Am I carrying out correct steps in correct order?

Thanks,
Prasoon

4

I attach a (plenty of vias) v8.0.3 Kicad project as example. Basically these are the steps you can take into account:

test.zip (74.5 KB)

Layout Example and Generate Drill Files report

image
image780×735 39.7 KB

image
image658×606 41.7 KB

0.5mm backdrill-pad footprint

image
image1011×642 48.3 KB

3 backdrilling-pad placed over THT vias

image
image1269×666 35.7 KB

3 Backdrilling-pad opened with Kicad Gerber Viewer and export them as Hole Data. Note that a new backdrilling.kicad_pcb Kicad PCB will be created.

image
image1280×433 43.8 KB

image

Here’s the last step:
Drill Files report of backdrilling Kicad PCB file

image
image641×606 39.6 KB

1 Like
5

Thanks. Let me try this and I will let you know.

As another workaround, I followed your recommendation of using a pad footprint as a backdrill indicator. But, i specifed the pad type to be a NPTH. With this, the drill report contains PTH and NPTH at the correct locations. Now I just need the fab house to confirm if this specification is adequate and if they can control the back drill depth based off the fab sheet spec for NPTH. Holes with different depths could be specified at different user layers.

Thanks,
Prasoon