I'm currently rough drafting a RF/microwave pcb which I hope will be fairly wideband, from Mhz to possibly 6-7GHz. (not sure if it's possible). Anyway, when laying out the various components I find that many of the devices have different pad sizes, so there's no way to adjust the board or CPW to match all the different pad sizes. The distances between these pads will be small except for a short run of about 7mm to an RF switch. My question is, should I bother tapering the connections to the varying pad sizes to avoid abrupt changes, or does it not matter for short sections like this (~1mm between pads)?

The board will be a 4-layer with Er of 4.6. For 50 ohm impedance, the grounded CPW track width was calculated to be 0.35mm. This is smaller than all the components except for the RF switch which has 0.3mm pads. The SMA connector, 402 and 603 all have different but larger pads. There is another board option that is thinner, but the track width came out to 0.2mm which seems like it would make things worse. Anyway, I started adding tapers in the top path, but wanted to get some opinions here before moving on to the rest of the board.

Here is the layout I started: (no via fence yet, and pardon the 3D, it was the only way I could export)

rf board layout

There are two SMA connectors on the left, each going to a TVS diode and 2nd-order high pass filter, and on to the RF switch in the center.

Additional info: The TVS will have a capacitance of < .07pF and the L1/2 inductors are about 5uH, which is why I cannot use a smaller SMD.

Update: For others who might run into the same issue, here is the updated layout using the advice here:

updated rf layout

  • \$\begingroup\$ What precision do you need (flatness / some dB of return loss / SWR how close to 1.0 / etc.)? \$\endgroup\$ Dec 27, 2022 at 17:14
  • \$\begingroup\$ I don't really know what is feasible, but I'm thinking around 1-2dB off from flat \$\endgroup\$
    – fivejeez
    Dec 28, 2022 at 5:56

1 Answer 1


That's not the place to taper a track. A taper may be used usefully when connecting two lines of the same impedance but different geometry, for instance when changing from CPW to microstrip to use a wider track. In this case, matching in a wider pad (for instance L2's), you will get better results by keeping the track the correct width for as long as possible. It would be even better to narrow the connecting track further, to make it look a bit inductive, to form a low pass filter with the capacitive pad, thus improving its match. The matching problem comes not from the change in track width1, but from the track being the wrong width. A naive way to think about reducing the track width further is that 'on average', the track is closer to the design width.

However, you probably don't need to worry about the pad. The component itself will have imperfections, a bit of extra C across it, which could make the pad strays pale into insignificance. Get a good model of the component, and see what its strays are. The TVS will probably dominate them all.

The pads for L2 look to be excessive anyway. The purpose of a PCB pad being larger than the component pad is to provide fillets for solder so that you can visually inspect the joint quality, and to provide some tolerance for placement during board assembly. There's no reason that L2's pads require such a long heel (under the package) or toe (opposite the heel), when you could increase the size of the side fillets along the track.

I reckon you could get C4/5/6 closer to the package.

1 - yes, if you have two transmission lines of the same impedance and geometry but different sizes, there is a capacitive discontinuity if you simply connect them directly. Hence the 'Kraus Step' of moving the steps apart, aka adding a bit of high impedance inductive line between them to turn the C's into low pass filters. Or connecting them with a taper. However, those effects are far smaller than the strays of the inductor and TVS that you may have to deal with first.

  • \$\begingroup\$ You could also potentially couple the narrowed sections together, making a sort of tapped inductor with the (pad/component) capacitor in the middle -- an all-pass structure that maintains a peaked frequency response. But needless to say, this is in the domain where you'll want a transmission line / PCB simulator to optimize everything. Which may also show the pads just aren't an issue, or that the components dominate. \$\endgroup\$ Dec 28, 2022 at 15:03
  • \$\begingroup\$ Thanks, definitely point taken about impedance matching, however I cringed a bit seeing the hard corners created by the different sizes while routing the tracks. My concern is at the higher GHz these corners (rounded or not) are places where reflections can occur and affect SWR. Is this unfounded? \$\endgroup\$
    – fivejeez
    Dec 28, 2022 at 15:10
  • \$\begingroup\$ @fivejeez Yes, it is unfounded. If you have access to a simulator that can model such discontinuities, it's worth recalibrating your intuition. \$\endgroup\$
    – Neil_UK
    Dec 28, 2022 at 16:54
  • \$\begingroup\$ well that makes things simpler then, great! Are there any reasonably priced software that model this? This would be my first RF board. Right now I just use KiCAD for layout because it is free. \$\endgroup\$
    – fivejeez
    Dec 28, 2022 at 20:39
  • \$\begingroup\$ You may be able to get by with a 2-D field solver. \$\endgroup\$
    – SteveSh
    Dec 28, 2022 at 21:19

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.