Looking for 'high-ish' frequency PCB review. - Page 1
Forum section: electronics / projects

author: TERRA Operative
author_rank: Super Contributor
timestamp: March 03, 2021, 03:45:09 pm
content: Hi all.I am currently designing my own version of theTektronix 067-0625-00 Peak-to-Peak detectorand am looking for any advice corrections or pointers for my PCB design.I'm having a bit of fun with this, pushing the layout far further than the original design was designed to go, just because I can and for a bit of layout practice (I haven't done much 'high' frequency stuff)I decided to have a go at a coplanar waveguide with ground, designed for 50ohm impedance on FR4, which should be good to just alittlemore than the 500MHz specified in the original part (component interruptions etc not withstanding).Can anyone who knows more about this stuff take a look at the designs below and let me know if anything looks incorrect or able to be improved?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: March 03, 2021, 05:12:03 pm
content: Nahh don't split the path. You're making stubs. Just put the diodes and terminator in the same place, one straight route. The diodes have much higher impedances (for most of a cycle, anyway), their capacitance is dominant.Don't bother with feedthru capacitors, just use pairs of small chip capacitors flanking the diode. Keep distance from signal to diode to capacitor as short as possible. You can safely place them close enough that their pads are nearly touching, leaving a minimum width soldermask sliver between them (~0.1mm).If you're feeling really pedantic, use two pairs of flanking capacitors, with a ferrite bead (~100 ohm at 100MHz?) between them. Stitch the ground plane modestly in the area, isolating RF signal from the DC side.This can all be one board, no need for two.Nice part about 2-layer 50 ohm trace, the width is so big you can basically put all three pads across the trace and still have soldermask between them. Without widening the trace at all...At worst, I suppose a tee coil peaking configuration could be used, but that wouldn't be needed until like ~GHz. Also would be hard to do on a PCB; and most of all, wouldn't be easy to realize a stable frequency response due to the C(V) dependence of junction capacitance. So it wouldn't be able to provide the ~double bandwidth that is possible from that configuration in a linear circuit, the worst-case improvement would be more modest. Anyway, there are <1pF RF diodes available to cover that range, without questionable hacks..Tim

author: TERRA Operative
author_rank: Super Contributor
timestamp: March 04, 2021, 02:39:47 am
content: Thanks for the pointers!I've made a new revision, I shrunk it down to one PCB and reworked the layout, also switched to end-launch BNC's for output as well as input.Hopefully I got things close to your suggestions.....I'm not sure about C1/C2 and C5/C6 that I used to replace the feed-through caps, should they be staggered down the trace to allow the trace to maintain the proper width?I hope I'm on the right track...

author: WideBandwidth
author_rank: Contributor
timestamp: March 04, 2021, 02:48:08 am
content: In your second design, it looks like you got rid of the via fence you had going along the coplanar waveguide ground planes. That's definitely not going to help matters. That's probably not going to be nice to the transmission line impedance at very high frequencies, and C6/C1 are going to have a really long path to to bottom ground plane. But since you got the end-launch BNC, not sure how big a difference this would make.

author: TERRA Operative
author_rank: Super Contributor
timestamp: March 04, 2021, 03:17:44 am
content: Ah derp. I forgot the vias!Here we go, enough vias for everyone!

author: TERRA Operative
author_rank: Super Contributor
timestamp: March 04, 2021, 03:23:08 pm
content: Had another poke at it tonight.I made the traces more symmetrical between the - and + sides, pulled the solder mask off the main trace (will be gold plated) and pulled the ground plane out from under the components on the main trace.Made a few other little tweaks here and there too (And fixed the STEP file for the battery holders, but that's purely cosmetic, because I'm a pedant).I just have to figure out if C1/C2 and C5/C6 are ok as they are or if they should be staggered to maintain uniform trace width (I assume the latter option is better?)

author: WideBandwidth
author_rank: Contributor
timestamp: March 04, 2021, 03:38:44 pm
content: At the frequencies you're working at, you're not going to see a difference. Even at 1GHz, wavelength in free space is 30cm, in FR4 it's somewhere around half of that. Meanwhile an 0603 capacitor (for example, I don't know what size you're using) is ~0.7mm in width. So you're worrying about a little strip of transmission line that's less than a tenth of a wavelength long. Depending on the size of those caps, I'd be more worried about their self-resonant frequency.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: March 04, 2021, 04:03:45 pm
content: Where did the diode resistors come from?With BAT54s, you're not going to be doing anything flat above 200MHz anyway. The RF signal path is one trace, short and low Q. The DC path is... a DC... path... it doesn't care.Also, those look very far from IPC compliant SOD-123 footprints??Tim

author: TERRA Operative
author_rank: Super Contributor
timestamp: March 04, 2021, 04:19:20 pm
content: The diode resistors are R2 and R3 are in the original schematic in the OP, they are 100ohm carbon comp in the original design, in series with the schottky diodes.R1 and R12 are the termination resistors, I stuck two 100ohm resistors to ground, but probably should only use one 50ohm there I guess.These parts housed in a cavity in the 'RF Head' section of the original design (Hence my original two PCB design).For the schottky diodes, Tek specifies 15V diodes (They are through hole 'ND4973' diodes wired point to point in the original design), do you have a suggestion for a higher frequency capable SMD part?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: March 04, 2021, 05:40:16 pm
content: Examples here:https://www.digikey.com/short/dv7h0pz3Tim

author: TERRA Operative
author_rank: Super Contributor
timestamp: March 06, 2021, 06:01:59 am
content: Ok, diodes replaced with 1N5711 Shottky's and tweaked stuff here and there a bit more.I guess next is to figure out if C1/C2 and C5/C6 (4700pF 0603) are going to have self-resonant problems. Oh, and R1/R12 termination resistors have to be poked yet too. Will do that later.I keep diving deeper and deeper...Anyone have any pointers on these caps?

author: TERRA Operative
author_rank: Super Contributor
timestamp: March 07, 2021, 09:01:07 am
content: Ok, more tweaking.I reworked the termination resistor at the input BNC, and staggered the caps as mentioned previously.Still not 100% sure about the capacitor self-resonant frequency thing, but at this stage I might just suck it and see.I think the MLCC caps I used should have less overall inductance than the feed through caps and their leads in the original design.