PCB striplines & via fences

[nali]

Hi

I need to mount a LTE modem device on my PCB and I'm now at the stage where I need to run the PCB trace out to a SMA antenna connector, so I’m reading up on PCB transmission lines. I’ve looked at various online resources, downloaded Saturn toolkit and of course have the Tech Spec of the actual device.

The Tech Spec suggests a Stripline for the antenna traces and gives an example (below). This is for I think a 6 layer board but I want to use a 4-layer board mainly for cost reasons so I’d need to make it an offset stripline… which in itself shouldn’t be a problem.

My question is regarding the via fence, as none of the calculators I’ve found feature this – just a stripline and reference plane(s).  Can anyone shed some light on whether they make much difference (to EM interference with other parts of the PCB), whether or rather how they affect the impedance of the line, are there any calculators out there that cater for this type of line?

I’m probably way overthinking things as a) the line will only be 30mm or so and b) antennas often don’t present a perfect load depending on installation, but this is as much for my education as it is getting the PCB done.

Thanks!

[Rerouter]

Keep the vias about double your ground gap and the impedance change should be minimal, short of 5G signals a standard via fence spacing will be far too tight to cause any resonant issues.

As its more ground material it does lower the impedance of the signal, but due to the spacing, its minimal in most cases.

[nali]

Cheers... I'm not sure what you're referring to by "ground gap" though, do you mean G or H1/H2 in the image I originally posted?

My H1/H2 will be quite different for a 4-layer board as H1 will be the core and H2 will be the prepeg, so it'll be an offset stripline. The value "G" is the one I'm trying to get my head around. Mind you, I did find a note in a Rogers presentation suggesting that gap to the vias should be about 3x the width of the centre trace so maybe that can be a starting point.

(it's on p32 of this document)

[ejeffrey]

It is pretty insensitive to the spacing.  I usually make them approximately H1+H2 away.  You can actually push them out farther in most cases -- in most cases the issue is how close can you get them to improve density.  The vias can't carry any longitudinal current so they don't meaningfully affect the inductance.  They have some slight capacitance, but it is tiny.

They aren't in the calculators because they aren't supposed to participate in the transmission line.  Their only purpose is to short out waveguide modes of the substrate. 

[nali]

OK thanks, that makes sense. I can get on with my board now... actually I've got tons of room on this board so I can do pretty much whatever I want layout-wise.

Every day's a school day! 

[SpencerTC]

I see that I am a bit late, but I thought I would introduce you to a paper I read, which when I experimented with seems to be very accurate, regarding the spacing between vias and vias and the spacing between the stripline and vias.

The paper can be found at https://mpd.southwestmicrowave.com/wp-content/uploads/2018/07/Optimizing-Test-Boards-for-50-GHz-End-Launch-Connectors.pdf and you might just want to skip to page 12.

It likely isn't near as much of an issue at the frequency you are working with, but the principles remain the same, at least down to 8GHz where I was experimenting.

Good luck with your design.

Best regards,
Trent Spencer - KM4YTU

[nali]

Thanks for the link, I'll have a read of that when I get a bit of time. Although I'm not a total newbie when it comes to RF I've never really paid too much attention to transmission lines and the like, so I do intend to read up on it a bit more.