Hi all,
I’m designing an 8-layer board in KiCad 8, and I need to place a pad an inner copper layer** — for example, on In1.Cu or In2.Cu.
I’m not looking to use a via
I’ve tried editing pad properties, but KiCad doesn’t seem to allow assigning SMD to inner inner layers only to F.Cu or B.Cu
Any help is appreciated
Thanks for your reply! I wasn’t trying to add a blind via, but rather to change the copper layer pad to an inner layer, like shown in the image.
Also, if you happen to know how to change it, I’d greatly appreciate your guidance
SMD pads assigned to the inner layer? How do you solder components?
As far as I know, KiCad has not official support for SMT pads on inner layers (but there are valid reasons for having these). Some people have hacked around this by changing the layers of those pads with a text editor, and this seemed to work. apparently KiCad has no GUI to generate this sort of pads, but when the pads are placed on an inner layer by other methods, they tend to stay there without problems.
Also note that the default settings in KiCad is for a 2 layer PCB. As a result, KiCad’s libraries can not assume inner layers are present, or of what those layer names would be.
in that image, all the pads are on the top layer (like it should be to be able to solder the part down). I think you might be getting confused by the colors.
in that image the colors are not other layers, they are (probably) assigned to groups of nets or by function (digital, analog, comms, etc).
fan out from BGA
I added a through-hole via close to the SMD pad of the IC that I needed to route
To create the fan-out in KiCad, I placed a blind via directly on the BGA ball using the ‘via-in-pad’ technique. Then, I added a through-hole via near the SMD pad I wanted to connect. I’m not sure if this is the standard approach, but it seemed to work in my design. I’d appreciate hearing if others use a similar method or have any suggestions for improvement
You can also use hotkeys for via placement.
Place Blind/Buried vias is Alt + Shift + V
Switch to B.Cu is Page Dn.
Switch to Top Cu is Page Up.
Internal Layers need hotkey assignments.
You can end up with this sort of result:
As Paul noted, It is possible for an inner-layer SMD ‘part’ in Kicad, but it’s a bit of a hack presently. One reason is for inner-layer net ties. Attached is the contents of a inner-layer nettie footprint kicad_mod file. Note where you can hack the layer name of the ‘pads’.
It’s kludgy as it won’t be editable in the footprint editor but you can place it. It’s also kludgy to select it once placed.
I used (96) of these inner-layer ‘components’ to try to keep the remote transimpedance amps return reference the same REFGND area as the associated PGAs.
