NRF52840 sma routing

RE: NRF52840 sma routing

AmbystomaLabs — Fri, 07 Sep 2018 16:37:26 GMT

I don't want to get too involved here since you have a big thread going on with ketilijo but...

1. You should model your surface mount connector and not just assume that if you get the CPW on the board correct everything works out. The feed pin on that SMA is massive and the resulting capacitive coupling to the board is severe. Normally, SMA's have almost no ground near the feed pin as a result. So, you need to model it in an EM simulator and/or follow the manufacturers layout guidelines.

2. When switching to thru hole the resulting capacitance from the feed pin to the surrounding layers is even more severe. As you have shown it above, switching that to thru hole would likely be close to a short at 2.4GHz. Again, model the solution and don't guess or you won't be happy with the results.

3. Unless you have need of the right angle to board solution that thru hole provides you will get a more reliable RF solution with all the same mechanical qualities of thru hole by using an end launch sma connection instead. Then the CPW just goes straight onto the feed pin since it is all characterized. Normally end launch with a tab center pin is preferable to those with the round center pin for RF purposes. But at 2.4GHz a round center pin isn't too bad.

RE: NRF52840 sma routing

ketiljo — Wed, 29 Aug 2018 07:18:35 GMT

You can adjust the impedance with the width of the track as well. But 60 ohm is good enough. You can find calculators to help you find the loss due to the slight mismatch. With a 60 ohm transmission line (and antenna load impedance to make it easier), the loss is only 0.04 dB.

RE: NRF52840 sma routing

Sparky Tinker — Wed, 29 Aug 2018 02:56:27 GMT

Thankyou for looking at this.

I looked at the Co-planar waveguide calculations and they came up with about 60ohm.

Calculator_1

Calculator_2

Relative Dielectric Constant = 4.2

Track Width = 30mil = 0.762mm (as per reference design)

Track Spacing = 10mil = 0.254mm (as per design rules)

Board Height = 64mil = 1.6mm

copper height = 1.4mil = 0.035mm

One way I managed to get close to 50 ohms was to use 0.5mm between guide and ground plane, so this would mean using a 0.8mm board and ground plane on the 3rd layer.

looking at the space left in the SMA connector there isn't much room to change track thickness and gaps.

Am I simply over analysing this or will 10 ohms cause a disturbance in the signal,

I am using rssi for distance calculation and am trying to get the most uniform and stable signal across multiple copies of this device.

RE: NRF52840 sma routing

ketiljo — Mon, 27 Aug 2018 13:49:32 GMT

1. You need to have the bottom layer as solid ground plane. Technically, you don't need the cut out on the inner layers either, but it doesn't harm. The transmission line must be calculated depending on the PCB stack up. The dimensions of the transmission like hence depends if you have a cut out in the inner layers or not.

You want to use a "co-planar waveguide" as the transmission line. You can find online calculators.

2. Not unless it's very long.

3. The output isn't 50 ohm so some external impedance transformation is needed. The components also do low pass filtering of the harmonics.

4. If you follow the reference design exactly, there should be no need to tune anything.

Using a through hole or surface mount connector matters little.

RE: NRF52840 sma routing

Sparky Tinker — Sun, 26 Aug 2018 08:10:17 GMT

Addendum:

I made the sma connector surface mount, is there any considerations when making it a through hole component.