ATTN: RF PCB-LAYOUT DESIGN ENGINEERS, I need some help!

Right.

Or use just one solid ground plane.

John

Nope. The BAVs seem to be working fine (this is the +-18 volt floating power supply, 16 on a board, now running a "soft" square wave at 45 KHz.) No sign of reverse-recovery snaps. One minor screwup is that even a little ripple at 45KHz shoots right through the output opamps (psrr sucks at 45K!) so next rev we'll use an r-c-r-c power supply filter to zap the ripple harder. But the board (16 isolated analog voltage/thermocouple-simulation outputs, 4 ref junction RTDs, uP, 2 big FPGAs, 12K lines of code) works first-try as designed... just a few value tweaks, not a single kluge!

It's our first project with the new guy I designed it with, and I met him on this very ng! I knew there was a reason to waste so much time here.

John

Hello Chris,

That may be your problem right there. In my experience splitting grounds has never really worked. Definitely not in circuits that must operate above the audio band and it seems you are quite a few orders of magnitude above.

Try to tie them together. But not with any wires, it needs to be multiple connections with next to nothing in inductance. IOW copper tape and stuff like that. Watch you fingers to avoid those nasty copper tape cuts.

Regards, Joerg

Hello John,

Yes, that's what I meant. Considering the time it takes to have another stuffed PCB in hand it is often worth to try to connect split planes in as many locations as possible, to somewhat mimic a solid plane. It'll look ugly but you can go on debugging. In parallel I'd order a board with a solid plane.

Did you swap out those BAV99 for BAT54?

Regards, Joerg

Hello John,

Cool. What I found on isolated power supplies was that the ESR of the filter caps after the diodes begins to matter. For the very same reason, PSRR. At 60Hz the PSRR would take care of things but not at tens of kHz.

On pulse echo systems I have it easier than you did. I can synchronize the soft square wave to the pulse repetition rate and none of the ripple shows up. But the transformers have to be pretty wideband for that, usually 10:1.

That is great. I bet that 80% or more of all engineers do not even know that usenet exists.

Regards, Joerg

I do, in fact, have the ground planes tied together at one point via a strip of copper. I'm not sure that using one ground plane will help as I'm afraid that any of the higher-frequency RF components (3GHz to 4GHz ) may couple into the ground plane and radiate throughout my PCB causing the output of my LO source to be rife with spurs. I'm wondering if my problem lies in the overlapping of the analog and digital grounds; there may be some parasitic capacitance playing in here...it is, afterall, a 4-layer board.

Rene-- Yes, you are right...I would do a lot better if I isolated the RF components. The problem is, however, I do not have that luxury for this system. Everything pretty much has to be on one PCB. In fact, I've noticed that some of the copper traces on my board are radiating. Most of this radiation is from signals in the 6GHz range and above...turns out that the mixers I am using produce very strong 2nd and 3rd order harmonic terms and these high-frequency harmonics are radiating on my short copper traces. Does anyone out there have some experience doing PCB layouts for telecom industry? CDMA/GSM standards...etc.? I fee like PCB layout gurus would run into the same problem as I am having when making these devices seeing as how components inside cellular phones these days are jam-packed.

Thanks again for the posts. Any help is greatly appreciated.

Hello Chris,

That ain't enough. Try it in more than one place, lots more.

It could be. Two planes connected in one place may form a pretty good dipole antenna which can pick up and radiate. And you don't want antennas in your board. That is one reason why a common plane is usually better.

Regards, Joerg

I'd put the RF stuff in a box and have the controlling wires though the wall with T filters. You can also put the lot into a box and separate the sections with internal walls.

Rene

--
Ing.Buero R.Tschaggelar - http://www.ibrtses.com
& commercial newsgroups - http://www.talkto.net

Hello Chris,

You have to strictly adhere to trace impedance rules or your traces will sing. The minute your trace impedance varies or a trace isn't terminated with its characteristic impedance at least at one end it starts to radiate. Refer to an older ECL data book with trace impedance calcs or use an electronic cheat sheet like this one:

Also, avoid sharp 90 degree bends because that will disturb impedance. At 6GHz this kind of stuff really matters.

If you do layouts out of house you need a very exprienced RF layouter or you have to coach pretty much through the whole session. I am lucky that I have a good layouter 1/2 hour's drive from here. Don't know about 6GHz stuff but he did all my RF boards intuitively right with very little input from me.

Regards, Joerg

Having just separate ground planes is not sufficient. A PCB can act as a waveguide at high frequencies, so you have to block the path *inside* the PCB. Open a cell phone and you'll see how it is done: a ground trace around a circuit on one side and closely spaced vias from this ground trace to the ground plane on the other side. This creates a faraday cage inside the PCB.

Meindert

Wow, thanks for all of the great advice you guys have offered me. I have two questions, still.

1) I figured that even if my PCB traces were not 50ohm traces that I would avoid transmission line effects if I kept the traces very short (relative to the wavelength, of course). 50ohm lines on FR4 are something like 62mils wide...too wide for me to work with. I suppose what is happening is that my PCB traces, although short, look like quarter-wave antennas to the high-frequency harmonics (6GHz and above) that "live" on my board. Is there ANY way around this? How do I get rid of these nasty harmonics? Attaining 50dB of isolation on a PCB seems ridiculous to me unless I start enclosing the critical parts in Faraday cages and use hard-pipe to connect filter components. Do i have ANY other options at all? 2) Meindert - Thanks for the cell phone advice. I will pop one open as soon as I can. I guess I'm wondering: Do the cell phone guys isolate the VCO from the PLL or is it all done on one circuit board? The idea of creating a Faraday cage on the PCB is very interesting to me...

It seems to me that RF circuit design is a bit of a black-magic art form. I'm very green when it comes to doing RF circuit layouts so this is probably why I'm running into so many issues. Again, thanks for all of the handy advice, I will surely put it to good use.

-Chris

Hello Chris,

Short of reducing the FR4 thickness between trace and ground plane it's going to be difficult. You could try a little loop at the device that you suspect generates harmonics, kind of a poor man's low pass.

It is black magic. That's why you really need this book: Johnson, Graham "High Speed Digital Design - A Handbook of Black Magic". Seriously, that's its title. Pretty much a must on the desk of anyone doing circuits like you are designing.

Regards, Joerg