RF PCB Design Help - Page 1
Forum section: electronics / rf-microwave

author: DrMag
author_rank: Regular Contributor
timestamp: April 27, 2017, 05:51:05 pm
content: Alright, you RF gurus out there--can you critique what I'm trying to accomplish here? I know very little of the dark art of RF pcb design, but what little I know tells me I need to be careful about layout and trace sizes/lengths. I am trying to build an oscillator that can be used to transmit (low power) on the 2m band. I'm planning on using an Si5351 with a butterworth band pass filter. The filter design I chose is centered at 146 MHz with a bandwidth of 80 MHz (mostly to get capacitor/inductor sizes large enough that traces won't make a huge impact). The board design prototype here puts the filter on CLK0, and for reference just a straight signal from CLK1. I have a ground plane on the bottom side (except for a power trace to Vcc), and the traces to the SMA connectors are sized at just short of 3 mm wide, which I believe on a 63 mil FR4 board should give me the desired 50 Ohm impedance. All other traces on the top side are 0.2 mm to accommodate the pin size/spacing on the Si5351. I may be able to up those traces to 0.3 mm if I relax the spacing constraints on the design rules.Are there any major no-nos I'm doing here? Would I be better off trying to separate the inductors, or at least rotate L2 by 90 degrees?

author: rheb1026
author_rank: Regular Contributor
timestamp: April 27, 2017, 07:29:25 pm
content: Not an expert, but I noticed two things:- You have no pullup resistors on the I2C lines. Although you may have these off this board somewhere- You may want to use CLK0 and CLK2 just to keep the two as far apart as you can, instead of 0 and 1. I seem to recall reading somewhere about crosstalk between the channels on the Si5351, but I personally have no experience as I've only used one channel with these ICs

author: loxodes
author_rank: Contributor
timestamp: April 27, 2017, 07:47:57 pm
content: The board will probably work as is, trace widths and lengths aren't super critical for small boards at VHF.Yeah, orienting the inductors perpendicularly may improve the filter a little.Are any external capacitors required for the crystal?And a bit of bikeshedding:- maybe label OUT1/OUT2 and the connector pinout on the silkscreen- add a bit of bulk capacitance to the board (at least a few uF?)- consider moving the orientation marker for U1 so that it will still be visible with the component soldered down- the ground connections on C4, C5, and U1 have unnecessarily high parasitic inductance - consider moving the ground vias closer to C4 and C5 and add in a dedicated via for U1- the trace width through the filter looks unnecessarily narrow, maybe bump it up to .5mm or even the width of the pads

author: DrMag
author_rank: Regular Contributor
timestamp: April 27, 2017, 08:52:30 pm
content: Useful comments, thank you!I did realize after posting that I had not put in pull-ups (not critical, as you note it can be done off-board, of course), and I've added those already. The crystal won't need external caps, as I'm planning on using an 8pF load crystal, and that can be provided by the chip itself.loxodes, what to you mean by a bulk capacitance to the board? Where would you place that?

author: loxodes
author_rank: Contributor
timestamp: April 27, 2017, 09:24:49 pm
content: Quote from: DrMag on April 27, 2017, 08:52:30 pmIf there are long or thin power leads connecting to the board, a sudden burst of activity (like programming the synth chip over I2C or connecting up a load) could spike the current consumption and increase the voltage drop across the wires running into the board. In the worst case scenario, this could brown out the chip and reset things.A large-ish capacitor placed near the power input helps keep the voltage steady during bursts of activity. How large? I usually look at the values used on reference designs or example schematics in the datasheet.

author: DrMag
author_rank: Regular Contributor
timestamp: April 27, 2017, 10:15:31 pm
content: That makes sense. Thank you! I definitely feel better about this design, and unless someone shows up with a show-stopper, I'll probably have it made up and try it out. Here's the revised version of the board:

author: mc172
author_rank: Frequent Contributor
timestamp: April 27, 2017, 11:15:32 pm
content: I would lay the filter out as per the image I've attached. This avoids the downstream nodes being in close proximity to the upstream notes (i.e., the output of C1 is close to the input of L1 in your second layout). Keep the tracks between the filter elements fairly thick, otherwise your series inductance will start to add up and detune your filter.You can pretty much do what you want with the output traces as the wavelengths involved are so long relative to the track lengths that it almost doesn't matter.The big green mess is what you could do with the top layer grounds - join the two SMAs with a top layer ground pour with a few vias. Don't worry about thermal reliefs - the SMA connectors will require more power than the ground plane will during soldering.PS - yes, I did this in Paint.Edit - moved the last capacitor down and right a bit. I've left the original attached for comparison.