2 components sharing a "turret" (or a pad ?)


I use Kicad (5.1.9-0-10_14) to build guitar effect pedals. I’m not a Kicad expert, but I know how to get nice working PCBs.

I also build valve/tube amplifiers and I’m using Turret Boards.

I have the idea to design the schematics with Kicad and then generate some kind of turret board (the turrets would be connected by cu traces like on a PCB and components footprints would be visible on the board)

One of the major differences between a PCB and a turret board is that with a turret board, several components can be connected to one “shared” turret.

I could create a “turret” object in Kicad that would be a kind of pad and two components would be connected to this single pad.

But when I try to connect 2 components (a very simple example with only 2 components : R1 and C1 to a single pad (or position 2 pads in the same place), I get DRC errors (this seems normal to me from a pcb point of view) : Drilled holes too close together and Courtyards overlap

So my question is : is it possible to share a pad between 2 components, or do you see a way to have 2 (or more) components connected to a single “turret”?

Thank you very much!

It’s not going to be a “regular” PCB, and there is no need to be exact here.

I would just use resistors where the pads are relatively close together, and then “extend” then as necessary with PCB tracks to make the connections.

To keep track of the “connection points” you can draw an array of circles on for example the Dwgs.User layer

I would also set the grid to something compatible with the pitch of the holes in your board.

Just to be clear, you want to stay with “Turrets”? You do not want to put the wired directly into holes in the board? There is almost no reason to have any copper on the board. ??

If this is the road you are going down; I would not use a schematic but just make the red board with holes every 0.2 inch just like the picture.

I think it would be nice to have a silk screen layer with “pictures” of resistors and capacitors printed on the board. Rectangle labeled C4, including a line where the leads go.

KICAD was built to make boards with copper on the board and to get away from this type of constructions. lol A million years ago, when we were getting away from this type of PCB, one of the steps was to have a hole in the PCB for each leg of the component but to make the hole large and insert a rivet into the hole. This allowed people that don’t know how to solder to a PCB to solder to the rivet. Maybe rivet is the wrong word. Piece of soft metal tube that goes in the hole and expands out.

Please tell us more. Can you hand draw a picture of what you want?

KiCad isn’t particularly suited to this sort of design. Whilst you could put single point pads in your schematic where the junctions are, this means that the schematic is no longer an abstraction but rather a layout placement diagram.
I think that Lochmaster might be better suited to this sort of design methodology. There is a review here http://www.bestsoldering.com/lochmaster-4-0/
I believe that it supports a point to point mode although I have never tried it. There is an open source vero board layout program called veroroute which might also be an option - although I have no experience with this either.

Why try and force the limitations of the turret board onto a pcb? Just put the holes in line and put a heavy trace down. Assembly is easier. Mistakes are easier to correct. Repairs and modification are easier.

1 Like

One other option is to make a new component which includes the one turret and all other pads/holes for components which will connect to the turret. That will render the BOM invalid but perhaps it will work better for you.

I do such crazy things with SMT. I have one 3 pad footprint which accommodates one of two 0603 chip resistor locations, and a 4 pad footprint which accommodates two 0603 chips in X direction or two in Y direction.

BTW if you are going to make a pcb, you really ought to dive into SMT. I have been engineering since 1975 and was initially intimidated by SMT. But if you avoid the fine pitch parts, it is not difficult and it has many advantages. The main disadvantage of SMT components is for hand wiring…but you are making a pcb.



There are different styles of Turret Pins (shapes with/without Pins, with Holes, with Wire-Wrap…etc).

I’m sure you can locate your desired one on-line but, attached is a quickly made one and Footprint (Pin with Through-Hole, Pads on Top and Btm). You can set the pads (in Footprint) as desired and the FreeCad file and Step file are attached…

Pin depth=1.6mm, O.D/Pads.≈3mm, Height=6mm (my Kicad PCB setup is for 1.65mm, so you’ll see a Gap on bottom side…)

Turet_6mm.kicad_mod (610 Bytes)

Turret_6mm.step (12.5 KB)

Turret_Pin6mm.FCStd (27.5 KB)

Screen Shot 2021-11-27 at 9.35.08 AM

Screen Shot 2021-11-27 at 9.34.53 AM

You could turn off the DRC errors? As you are overlapping deliberately. And perhaps make a turret component with turret hole surrounded by SMD pads for fake connections? I’m on my phone, so haven’t tried thuis…

It appears there is no copper on the board. So just don’t send the copper gerber files. You and make any type of fake component you want as long as you don’t use the copper layers.
Here is a picture of a PCB like he is using.
I made my ham radio like this. Really no need for a CAD program.

Perhaps something like this … ? But EEschema does not allow parts at free angles. The four pins on my cross point turret have the same pin number so will allow track wiring in Pcbnew to a single pad component such as a mounting hole. Then on Pcbnew, you could use the bottom layer for copper tracks that you want and the top layer for air wires, then not send the top layer Gerber to the pcb manufacturer?

Trying to use the schematic for this seems illogical to me.
The schematic is meant as an abstract representation of how a circuit works.

The PCB is for mechanical placement of parts and connections.
There is no “real PCB” here, but you can still treat it as such.

The “Turrets” can either be represented by real single point parts (Maybe create a schematic symbol that sort of looks like a junction dot) or simply use via’s to represent the turrets. In this way Pcbnew can be used to verify there is enough room for the real parts and as documentation between the schematic and “pcb”.

First of all, thank you for all these answers, wow !

I’m going to analyse this and think about it; I’m well aware that Kicad is not necessarily the best suited for what I want to do with the turret boards

To answer some questions: yes, I like turrets for the ease of changing a component (prototyping, maintenance etc) without having to remove the whole PCB ; yes, I need copper tracks because there are wires between some turrets :


I usually draw my layouts with MS Visio (and therefore, there is no automatic DRC type verification), so I could “draw” with pcbnew the tracks and make my own footprints (and turn DRC off :wink: ) ; or cheat with very small pads which will be covered by the base of a turret (OK, this is weird :wink: )

In any case, thank you very much and I still have to think about whether I should abandon my idea or come up with an acceptable compromise, I’ll let you know

I added some red dots and red lines on the board.
Normally a resistor or capacitor has two holes for the leads and traces to connect them together.
I am suggesting making the board like normal and adding the turrets. (turrets in the schematic & PCB)
The PCB will have the option to solder to the turrets or put the leads in the board and be connected by copper. You can still use only turrets. The software will check the data and see if R1, C3, and Turret-7 are connected like in the schematic.
The silkscreen will say “R1” or “10k” or “R1/10k” any way you want. It will make assembly easy.

Assign a round filled zone to each turret. The blue round markings circling the turrets are filled zones. Filled zones can be drawn round by defining a fillet half the size of the filled zone. Add a drill hole in the center of each zone. Size the smd pads for each axial component footprint to match the diameter of the leads or smaller. Uncheck, F.Paste. Move the pads of the axial components into their assigned zone close to the edge. Draw a keep out area over the entire board to omit the copper pours and/or omit the copper from the gerbers. In the example shown the copper rectangle is a filled zone. The pads for each chip component to be soldered to the zone are made short so they neither overlap nor extend beyond the width of the zone. The copper extending the entire width of the zone is exposed by drawing a graphic polygon on the F.Mask layer. A graphic polygon is also drawn on the F.Paste layer. The clearance between each chip is at minimum.

Thank you very much for all these tips !

For the moment, this is what I do:

  • The components are SMDs which I have increased the size, pad on F.Cu
  • I have created a symbol and a footprint for turret
  • The turrets are inserted into the schematic (as connectors)
  • The F.CrtYd layer is minimised around components and turrets (new footprints)
  • To visualise the space left for the turrets stacking tool, I drew a circle under Dwgs.User (and not F.CrtYd)
  • I will exclude the f.cu layer from the Gerber files

So : no longer DRC error, check copper traces ok !

I still have to test whether this is applicable with a “real” schematic or too much pain in the … :wink:

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.