comb-over

8. From a coupler netlist to a KiCad board

This example takes the 10 dB coupler of Example 2, which is defined only by its even/odd impedances, and turns it into a KiCad 9 project with edge-launch SMA connectors. Nothing is typed into the netlist: every step uses the layout panel.

Netlist: examples/coupler-10dB-microstrip.cir

1. The offer

The netlist has no .layout line. Its topology, one coupled pair with a port at each of its four ends, fits the coupler template, so the panel offers a layout:

Layout offer
Layout offer

Choose a substrate and press Make PCB layout. The panel then:

  1. Writes .substrate jlc-ro4350b-1.524 after the header.
  2. Converts the section to microstrip. The even/odd impedances come from the section's Maxwell matrices, Z0e = √((L11 + L12)/(C11 + C12)) and Z0o = √((L11 − L12)/(C11 − C12)), and the coupled-microstrip synthesis then finds W and S for them on the substrate. Here Z0e 69.40 / Z0o 36.00 Ω becomes W 2.7226 mm, S 0.267 mm. The Zeo line is removed; len 90deg and the port wiring stay.
  3. Adds .layout coupler K.

Your previous netlist is kept: the notice above the status line has Restore it.

2. The panel

Layout panel
Layout panel

control writes
Substrate .substrate ID. It also re-synthesises W and S so the sections keep their impedances on the new substrate.
Template .layout TYPE SECTIONS…, from the templates the topology fits
Connector, Launch connector= and launch= (§8.4 of the manual); the defaults are omitted
Pitch, Feed, Margin pitch=, feed=, margin= in mm; blank uses the connector-derived default, shown greyed
Physical view nothing in the netlist; adds the as-built response to the plots

KiCad project downloads the board (manual §8.3). KiCad library downloads the part alone (§8.2).

3. Physical view: what will actually be built

With Physical view on, every plotted trace gets a dashed twin, computed from the as-built netlist. That netlist covers:

At 5 GHz on the two RO4350B thicknesses:

1.524 mm: bare section 1.524 mm: as built 0.508 mm: bare section 0.508 mm: as built
W / S 2.7226 / 0.267 mm 0.8831 / 0.1025 mm
S11 −31.78 dB −23.72 dB −32.91 dB −34.10 dB
S31 (coupling) −10.07 dB −10.34 dB −10.07 dB −10.25 dB
S41 −22.19 dB −25.60 dB −23.31 dB −24.98 dB
board 31.0 × 24.0 mm, 0 stitching vias 33.1 × 24.0 mm, 20 stitching vias

Physical view, 1.524 mm
Physical view, 1.524 mm

On 1.524 mm the as-built match is 8 dB worse than the bare section's. The reason is the size of the copper relative to the wavelength. The coupled lines are 2.7 mm wide and the 50 Ω feeds 3.3 mm, so the escapes, tapers and connector pads add a few millimetres of mismatched line at each port, roughly 15–20° at 5 GHz.

The same coupler on 0.508 mm keeps its match as built:

Physical view, 0.508 mm
Physical view, 0.508 mm

4. The trade-off

The thinner board is the better coupler at 5 GHz. But the Amphenol 132289 SMA is made for 0.062" (1.57 mm) boards, and the panel says so:

⚠ 132289 is made for 1.57 mm (0.062" board) boards; this board is 0.578 mm. The ground legs will not clamp the board…

There are three ways out:

  1. Stay on 1.524 mm. The connector fits; accept or optimise the match (next section).
  2. Use 0.508 mm with a connector made for that thickness. Only one connector is built in so far; others are added as entries in js/connectors.js.
  3. Lower the frequency. The escapes shrink in electrical length.

The thickness check sits on the layout card, not in the DRC list, because it is a mechanical fit, not a copper rule.

5. Optimising what is built

The physical view is for looking. To optimise the board itself, press As-built netlist. It opens the netlist of the layout, with every line section as a T element, so you can:

The launch placeholders sma_l and sma_c are already tunable, for fitting to a measured board.

Try