Electronics > RF, Microwave, Ham Radio

RF PCB questions

(1/2) > >>

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.

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.


This might be of some interest:

He recommends power planes on the inside.

His boards are open source so you could get some ideas from his design:

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.

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.

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.


[0] Message Index

[#] Next page

There was an error while thanking
Go to full version