0
\$\begingroup\$

I am currently redesigning a PCB utilizing the Xbee 868 Mhz module with external antenna connection on the pad ( https://www.digi.com/products/embedded-systems/digi-xbee/rf-modules/sub-1-ghz-modules/digi-xbee-sx-868 ). I have followed the rules from the datasheet and calculated the proper antenna trace width and distances for 50 ohm impedance. From Xbee SX 868 User guide:

enter image description here

In my application the question is, either it is OK to place the SMA antenna connector not in the exact corner of the PCB:

enter image description here

enter image description here

As you can see from the screenshots, the connector is on the edge of the PCB, but only horizontal. Vertical wise it is closer to the middle. The bigger issue is that in close proximity to the connector (counter side of the PCB to the antenna trace) there are traces and components placed. Even though there is going to be solid ground and shielding between the connector (GND polygon not poured on the screenshot) and the rest of the traces, I fear that the signal quality might get altered by the digital circuitry in the close proximity.

Are there any rules I can follow and a way I could check what is the desired minimum distance of other circuitry to the antenna trace?

EDIT: A screenshot of the top layer with GND polygon poured: enter image description here

\$\endgroup\$
  • 1
    \$\begingroup\$ Your assumptions are correct, the digital circuit will interfere, but I think a bigger problem will probably be the xbee intefering with the rest of your circuitry when it is transmitting. I wouldn't say that there are "rules to follow", you sure could calculate, or simulate, how much the effects of this would be, but you are usually better off just using good design practices; keeping stuff that can be sensitive to interferance from stuff that can give off a lot of interference, such as antennas and switching power supplies. In your case what you have done is probably OK, but if you want to \$\endgroup\$ – Vinzent Jan 10 at 20:15
  • 1
    \$\begingroup\$ be sure then you can improve the isolation between the RF portion and the digital portion by for instance adding a shielding cage around the digital part of the circuit, this is a very common practise. \$\endgroup\$ – Vinzent Jan 10 at 20:16
  • \$\begingroup\$ This Xbee module comes in integrated ufl connection version which I was using so far. It was my intention to get rid of the ufl connector and provide eztral SMA one. The reason was fot better durability of the connection. \$\endgroup\$ – Łukasz Przeniosło Jan 10 at 20:38
  • \$\begingroup\$ Durability depends on protection from stress or connection cycles? \$\endgroup\$ – Tony Stewart Sunnyskyguy EE75 Jan 10 at 20:42
1
\$\begingroup\$

Let's suppose that the effective relative electric permittivity is above 3 (I don't have the dimensions of your stripline so I'll do some estimation). Anyway with an Er of 3, you'll have a wavelength of roughly 8 in, this is much much longer than the stripline length, so transmission line effects will not be noticeable from the short stripline. In general making transmission lines short will reduce the effects from them, and is actually a way I use to simplify designs (in some cases).

You don't need to worry about noise from the Xbee SX 868 affecting the signal around the SMA as the SMA connector has ground bulit into the case and serves as a shield, the limited area that is exposed will provide minimal capacitance for coupling RF/noise.

In many respects, moving the SMA closer to the source is better, make sure you leave the ground plane below the trace even if it is shorter. And I also like to run the trace around all four posts of the SMA on the top layer for the sake of betterness (even if it is minimal, might make it slightly harder to solder though).

| improve this answer | |
\$\endgroup\$
  • \$\begingroup\$ Thank you for answer. I have updated my question- in my case I am having a GND pour all over the top layer, so the GND ring around the SMA connector would be lost. Should the top GND pour be ommited around the connector? \$\endgroup\$ – Łukasz Przeniosło Jan 10 at 21:14
  • \$\begingroup\$ Are you using a 2-layer design? Do you have a ground underneath the stripline? The ground on the top layer looks fine (I might back it off a bit until the top pour is about as far away as the stripline is wide). \$\endgroup\$ – Voltage Spike Jan 10 at 21:32
  • \$\begingroup\$ This is a 4 layer PCB. The first layer under the top one is the power plane, but the arean under the connector and trace is cut off and ground net is placed there. Then comes the ground plane. The bottom layer also has only ground underneath. \$\endgroup\$ – Łukasz Przeniosło Jan 10 at 22:09

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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