Absolute KiCAD beginner here - I’m trying to create a 4-layer PCB board with 4 nested copper loops in the internal layers, with through-hole vias conneting to the external layers. I’ve watched some tutorials but I’m still a bit confused as to how to get started, how do you create a 4-layer schematic? And it looks like I’m not able to add a purely-copper component, how would I do this? Thanks in advance.
You don’t. Schematics are abstract representations of circuits. Layers belong in layouts where that circuit is realised.
As for the loops (some kind of coil?) others will be more qualified than I to advise. Probably some kind of copper zone for each loop.
1 Like
That is true. I was thinking that you might be able to create a footprint in an external layer to form some copper shape, but being able to do that for inner layers (or more than one layer) sounds dubious.
Are you trying to make either an inductor or an antenna?
At schematic I don’t add a component. I only draw a not straight wire to signal that here are some coils.
So at PCB everything is one net. I have a ferryte footprint with defined openings and a graphic lines that help me to route tracks as I want. The end effect (4 layers) looks like this:
You should be able to find each layer coil begin and end.
I decided to not play with using rounded traces as, except aesthetic impressions it gives me nothing.
So in the schematic, would I create a page for each layer?
I think you don’t get it. There are no layers in the schematic.
Schematic shows connections to be done and not how they will be done (at which layer(s)). If, at schematic you have R1 connected to R2 with shortest possible wire (really it can be 0 length if resistors symbols touch each other) then at PCB this connection can start at R1 pad (I assume SMD) top layer then using via can go into In1 layer then after some meanders it can go with via into In2 layer and then with next via onto bottom layer to finally go through via to top layer and to R2 pad.
This is a two-terminal device, right?
Current flows into one terminal, spirals around though 4 layers, and comes out the other terminal, yes?
If so, the schematic representation is just a two-Teminal inductor.
You need to draw your footprint of this inductor using all 4 layers. That might be a little daunting, but conceptually not too hard.
1 Like
Did you checked if it is possible in KiCad? Can you have vias and tracks at inner layers in footprint?
I’m simply not sure and don’t have V7.0.7 here to check it.
Perhaps this will help…
Example: Using a Transformer with Two Inputs and Three Outputs, and 4-Layer PCB.
I did NOT bother to represent an actual device, just made it for Demo…
Summary:
• Schematic Symbol
• You can draw any representation/style you want
• You can Assign NET’s to the Wires
• You can Link Footprint to the Symbol
• There are handfuls of Symbol graphic representations to choose from and/or Draw yourself in Symbol Editor and/or Schematic
• PCB - Footprint
• You can draw/create your own Transformer Silk/other
• You can Use a Kicad stock Transformer (plenty of them and, you can Download a 3D-Model such as the one shown)
As other’s indicated, your schematic can reference NET’s if you want. There are No layers assigned in Schematics, only NET’s
On the PCB, you can load the Net from Schematic or, Not… You can assign NET’s in the PCB
Example Screenshots show Demo’s of:
• Schematic Symbol with NET’s
• PCB with Footprint (associated to Schematic Symbol - Ref, not visible (I don’t like clutter)
• PCB has Vias, 3D-STEP associated with Footprint, Wires for fun but not actually hooked up.
The 3D-STEP was downloaded from Digikey - just grabbed a CTR-TAP one. Didn’t care about actual/correct layout, connections…etc. Not important for purpose of this post…
Result: Shows Inner Connections to Vias, Tracks on Top, Btm and Two Inner Layers
To enable good visibility in 3D-Viewer, I set colors/opacity as I prefer…
@hannahannah I’ve done something like this before for NFC antennas. There are two ways to do it:
- Make it a footprint. This is a bit of a pain at the moment because it’s hard to place traces on inner layers - you have to explicitly set the layer of some graphic elements and the footprint editor does not provide a convenient way to do that. I’d recommend against it for this reason as it might require editing the footprint in an external tool.
- Don’t make a footprint. Instead, draw your traces directly on the board. On the schematic, you have a short circuit (direct connection) where the coils are. This is important. You don’t need anything else on the schematic. In the board layout, go to File->Board Setup->Physical Stackup and select 4 layers. Put in and connect all the other stuff on the board except the coil, lay it out so you have space for your coils left on the board. Then, go to Route->Interactive Router Settings and disable “remove redundant tracks”. Point your mouse pointer to one of the pads that the coil is connected to, and press X. The trace will start from whichever layer the pad is on. Take it off the pad, press V, click to place the via and then press - (the minus key) until you are on the layer you want your first coil layer to be. Draw your first coil layer with the mouse, then press V again to place a via. Click to place the via, and then press - again to get to the layer you want the second layer of coil. Continue this way until you get to your final layer. Once you have everything in, you can adjust exact trace positions by switching to a layer (with the +/- keys) and then pointing to a trace and pressing D to drag it (click to fix). When everything is exactly as you want it, select all the traces, right-click, and select Locking->Lock. Now these traces cannot be modified unless you unlock them. You can then continue connecting things.
I drew a simple example using this technique to demonstrate it.
If you want rounded traces, select the tracks (but not the vias) using the selection filter, right click, and select “fillet traces”. Note that you have to do this before locking the traces (or unlock them first).
1 Like
Don’t forge, there are a couple of plugins/scripts around to help you draw the coils/loops. Some of them probably out of date, but a good starting point nonetheless.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.