RF PCB questions

[init]

Hey guys. I'm looking at learning some RF PCB practices and have a few questions.

I understand that there isn't necessarily a 'best' way to stack a multi-layered board but one of the common recommendations I see is to have the signal layer sandwiched between two power planes/ground planes. The understand the theory behind why this is good practice however I'm a bit caught up on the particulars of how you get from a component (which has to be on the top layer) to the signal layer. If you have a signal running from one component to another right next to each other, I imagine there's no point in routing the signal down a layer, then up again a few mm away. How far generally, should a signal line go before you bother via routing it to the signal layer? When you do so, should you leave a min/max gap between the top power plane fill and the trace running from component -> via?

Personally, I am assuming RF of 100MHz for my purposes, but I'm happy to hear how these things differ for larger frequencies.

[T3sl4co1l]

It never made much sense to me, as the components/pins expose RF anyway.  Yes, you get savings over long traces, but there may be better ways of managing those, anyway (how much RF do you really need to spread around..?).

And if you need high isolation between sections (or reduction of emissions), you probably need shields anyway.  The set of cases where you do need internal traces, but do not need external shields, is probably small enough not to bother with.

On the other hand, you have strong advantages for outside routing.  Like if you need to cut traces and probe test points.

But I haven't made any highly sensitive RF boards, and I would defer to those who have.

Tim

[Earendil]

This might be of some interest:
http://hackaday.com/2016/03/23/michael-ossmann-makes-you-an-rf-design-hero/

He recommends power planes on the inside.

His boards are open source so you could get some ideas from his design:
https://github.com/mossmann/hackrf/tree/master/doc/hardware/hackrf-one-gerbers

I've also seen quite a few RF IC evaluation boards where they route signals on the top layer using a microstrip or coplanar waveguide.
Analog - for example - provides Gerber files for their evaluation boards so you can also get some ideas from there.

Vias add inductance/capacitance so at very high frequencies you probably don't want your signal to go through them very often.  At 100 Mhz this is unlikely to be a serious consideration though.

Regarding the distance. Though not directly relevant to your question but the usual rule of thumb is that you can route the signal 1/10th of the wavelength before you need to care about transmission line effects. For 100 Mhz that's about 15cm in FR4 I believe. Considering the 3rd harmonic that's about 5cm total. So unless you also have other considerations (like isolation as T3sl4co1l mentioned) you're probably safe to connect components under this distance directly.

Full disclosure: I haven't actually done this in practice. I love reading about topic though.

[Howardlong]

Well, I guess I do a bit of this stuff ;-)

There is no need for multilayer (beyond two layer) unless you need to: the caveat here is that to get small dimensions demanded these days at high frequency in terms of consumer acceptance, EMC and tiny modern RF parts you are often pushed that way.

The small parts mean it's often logistically hard to do 50 ohm without relatively long tapered tracks to the pins. Moving to either a thinner (and less rigid) substrate, or for production multilayer, is therefore often more practical.

But yes, I agree, keep the RF on the surface, and know (and confirm) your board house's stack up in terms of dimensions and material of you go multilayer.

Having said that, you can do an awful lot of prototyping yourself especially using 0.8 or 0.4mm boards. I also do plenty of unit testing on standard 1.6mm double sided board, etching only one side and using the back side as a solid groundplane.

Rule of thumb for 50 ohm on FR4 for microstrip is track width = board thickness * 2.

Most of my production stuff ends up at six layer as I am usually very space constrained, and six layer gives me a lot more flexibilty than four.

On six layer with RF on both sides I use ground planes on layers 2 and 5 and use layers 3 and 4 for non-RF routing. Ground floods on all layers and heavy ground stitching where there aren't any parts or tracks. Keep via'd RF to a minimum, if at all. Note stitched ground floods on RF signal layers makes your microstrip into coplanar waveguide, which makes the track width and flood gap calcs a little (but often practically not a whole lot) different.

As with many things, much of the RF black art voodoo is really down to understanding from experience and realising what's important and what's not so much. In that regard, I'd start off with double sided with solid ground plane on the bottom and microstrip on the top.

Somewhat counter intuitively, if you're space constrained then it can be easier: a 2mm uncontrolled RF path may well be inconsequential in practical terms at 2GHz: it can take that long to taper to a device's pin.

[nctnico]

About the question on how to change layers: you can create a matched impedance changeover from one layer to another by using ground layer vias (google that for exact details; there are appnotes out there). You can even do this for going from a ground referenced to a power supply reference plane by using vias + decoupling capacitors. The rule of thumb is that the return current of a controlled impedance trace flows directly underneath it. Electrical current always runs in circles.

[rfbroadband]

your questions are very broad and general, I will try to provide some answers as I have designed boards up to 20GHz.

as to why multi-layer RF PCBs? Contrary to many years ago more and more products require the integration some of the RF functionality to be combined with non-RF functions onto a single PCB due to cost pressure dictated by the market. Thus, simply using the most expensive, high end RF PCB material, do a 2 layer design, shield it with an AL shield is often simply too expensive. If your product supports that cost/margin, go for it...

The moment you need more than just RF on a PCB (uC, FPGA, or many analog functions) you need more than 2 layers. So the question becomes, when and how do you decide that 4 (or more) layer FR4 can't be used due to RF requirements?

One question to consider is the following: Do you do discrete RF design, meaning you have many individual circuits, components that create an RF system, thus you need to route RF signals from RF block to RF block, or do you have a very highly integrated RF transceiver IC that only has one high frequency RF input that needs to be connected to a filter and an antenna, because all other signals out of that RF chip are base-band signals? If the latter is the case you will be surprised for how long you can get away with FR4, because you only need one RF trace from the chip to the antenna and you keep that trace extremely short. We once did a 10GHz design on FR4 and got away with it (extreme cost pressure of the target market). We kept the one RF line extremely short, routed the signal into the RF chip and the remaining signals were base-band (low freq. signals) so that worked out ok. (The target market was low cost consumer electronics.)

If you do discrete RF design, but need more than 2 layers you can chose a sandwiched PCB stack up like the one shown below. You could use RF material (Rogers 4350 for example) for layer 1-2 and 3-4 and use FR4 like material in between (from 2 to 3). More layers would scale accordingly, thus for an 8 layer board you could use RF material for layers 1,2  and 7,8 and FR4 for everything in between.

In this case keep all RF traces on the top, use layer 2 as RF ground and do nothing else on that layer! Layer 3 could be power and some routing and layer 4 (bottom) could be used for digital routing and placing non RF components on the bottom side. With careful layout shielding techniques you can achieve very good isolation (> 120dB) between top and bottom layer. You can design boards where you run a uC with 20MHz xtal clock on the bottom side and with proper shielding within the PCB you will have a hard time even finding the clock from the bottom side on the top, unless you use very sensitive equipment. In addition you can still design a mechanical Al RF shield that is mounted to the top side of the RF section of the PCB to shield circuits located on the same side from each other.

Vias: Depending on the density of your board, you may run into issues if you want to avoid blind vias for cost reasons. If you route your digital and supply signals from the bottom side (lets say from layer 4 to 3) using a thru via, the end of that via will go all the way to the RF layer 1. The signal contained in that via ("only" to be routed from 4-3) will couple into the RF ground plane in layer 2 and (if applicable) layer 1. To avoid that you can use blind vias if you can justify the cost increase. If possible I would try to avoid routing RF signals thru several layers and keep them on the same layer.

Multiple high speed clock signals: If your design requires many GHz clock signals it is likely not possible to keep all the signals on the top side, in this case you will have to route the signals over several layers, you have to be very careful and make sure your  matching and shielding is sufficient. In this case the PCB stack will be different and more expensive.

Development time and schedule: You also need to consider whether your schedule (and cost constraints) permits spinning the board several times to get the required RF performance in the presence of digital signals. You may have to use special tools (EM simulators) which can't be justified all the time (cost of the tool and the experience needed to use such a tool).

There is no general answer because there are too many variables/requirements to consider.... but I hope  this answers some of your questions.