1
\$\begingroup\$

I'm trying to design a 50Ω coplanar waveguide to connect the output of a LoRa module to a SMD metal antenna. The two images below show the top layer (red) and bottom layer (blue). Vias are green and both copper pours are connected to ground. C7, C9, C10 are tuning components - not all will be caps and not all will be fitted in the final design.

Top layer view of coplanar waveguide

Bottom layer view of coplanar waveguide

Board thickness is 1.6mm, dielectric is FR4 (which I know isn't ideal and doesn't specify exact performance - cost reduction is important to this design). Feed trace width is 1.5mm, gap between feed trace and copper pour is 0.3mm and copper thickness is 35um. Operational frequencies are nominally 868MHz and 915MHz.

Does this look like it has sensible dimensions for a 50Ω feed? I used a few different online calculators (each of which with varying degrees of variable control) and it seemed close - but I have no experience of any RF work so I wanted to run it past some more experienced eyes. Also any general comments on the RF section layout would be welcome.

EDIT: Following on from @ThePhoton's comments, I have shifted the antenna feed slightly - see updated top copper image below:

Updated top copper layer view

\$\endgroup\$
10
  • 1
    \$\begingroup\$ First calculator I tried gives 52 ohms for your geometry. But that break in the return path due to pad 4 of the antenna looks like a problem. \$\endgroup\$
    – The Photon
    Nov 1, 2017 at 17:27
  • 1
    \$\begingroup\$ Yes, ideally get at least ~1 mm of copper there. Maybe flip C7 around to make it easier to adjust the trace. \$\endgroup\$
    – The Photon
    Nov 1, 2017 at 17:32
  • 1
    \$\begingroup\$ Stupid question: can you turn the antenna around 180° ? \$\endgroup\$
    – bobflux
    Nov 1, 2017 at 17:46
  • 1
    \$\begingroup\$ What's this? A board for ANTs? \$\endgroup\$
    – pipe
    Nov 1, 2017 at 18:33
  • 2
    \$\begingroup\$ Keep in mind the effect called "overetch": without correction, manufactured dimensions for traces will be smaller, and gaps will be bigger. Also, the dielectric properties can vary. You need to specify "impedance controlled" to your PCB manufacturer, they might apply a correction factor to Gerbers, and be more careful with dielectric resin properties. \$\endgroup\$
    – Ale..chenski
    Nov 1, 2017 at 19:03

2 Answers 2

Reset to default
4
\$\begingroup\$

Your trace width and spacing calculate out as a 50 ohm trace on a couple of calculators I checked, so that should be okay.

But I see a couple of other issues you should look out for:

  • In the original design, the return path is broken due to the cut-out around pad 4 of the antenna.

  • As shown on the app note from the vendor, the matching network should be as close as possible to the feed point of the antenna. The antenna is designed with plenty of space to fit the components beneath it. How to convince your CAD tool to allow this without a DRC error I don't know.

  • As shown in the app note from the vendor, the ground beneath the antenna component should be solid. This means the trace should be moved to an inner layer or the back side of the board.

  • With the matching network placed under the antenna (according to vendor recommendations), you may have to remove the antenna to adjust the matching network during tuning. Given the heavy thermal mass of the antenna and the un-connected pads that it mounts to, the pads are likely to lift when you try to do that. Be prepared to discard several boards if you have to tune that matching network.

\$\endgroup\$
2
  • \$\begingroup\$ Thanks for these observations. Having contacted the vendor, having the matching network slightly outside the antenna does decrease performance, but not dramatically (they didn't give figures). They also claim that this effect is less pronounced for shorter feed lines. I'll double-check with them re: routing the trace on the opposite side of the board. Thanks! \$\endgroup\$
    – stefandz
    Nov 1, 2017 at 19:04
  • \$\begingroup\$ For those following along I got a chance to show this design to the vendor. They are happy with the trace on the top layer - they say that this should not cause any issues. \$\endgroup\$
    – stefandz
    Nov 2, 2017 at 15:29
1
\$\begingroup\$

Grounded CPW should have most of the fields be between the two conductors, but you might still find that your antenna will interfere if you put it on top of the CPW line. Remember that for the impedance of the CPW line, not just the board but the space above the CPW matter (Putting something on top will ruin the impedance). Is there any way you can route the signal on the other side of the antenna?

In addition, currently you have vias to ground your outer conductors of the CPW line, which is good. However, try to either add more or keep them symmetrical to the center conductor. Symmetry is key in the performance of the CPW line here. Also make sure there is a via very around the ends of the line. You already have vias at the ground of those capacitors, but also add one where the next CPW line starts, so you ensure you have a good ground at that starting point.

\$\endgroup\$
1
  • \$\begingroup\$ Thank you - I didn't realise that symmetry of vias was critical to performance. \$\endgroup\$
    – stefandz
    Nov 1, 2017 at 19:06

Your Answer

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

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