开云体育

Here's some pictures of the original HP board that I found online:







Jared

Straight signal line, 2 layer, (transistors.....), bottom ground plane stitched to top ground pour.

Yep, looks reasonable to me.

Harvey

On straightening the traces, I wonder if rotating the parts (and 45 degrees is legal) would help.? Don't think that power leads are as critical.? IIRC, the bends might cause impedance changes and therefore reflections, but someone who actually does this might want to comment.

From what I remember about waveguides (seeing them), the minimum bend radius is frequency related, too.

Harvey

Alrighty, I've tweaked the layout a bit. I rotated the amplifiers by 45 degrees to straighten the traces. Also sprinkled a couple more vias around the place here and there.

If this looks good, I'll place an order for some boards.






Jared

From what I see, this looks a lot more like the original layout. If the packages were different, I'd have gone with a 90 degree rotation on the amplifiers.? However, unless you do a staggered layout (stairstep), I can't see it done with these packages.? I can't tell you which would be better.

It looks good to me, from my limited experience.? Also resembles the original layout a lot.

Harvey

Ok, so the latest PCB's arrived. This design is using the same prescaler chip as the HP design, with the same prescaler bias network.
I think I'll have to order a couple more parts, pending a raid of the parts bin, but soon I'll have a much closer replica to test out and see how it works.

Fingers crossed that the prescaler chips I sourced from China are genuine parts.......



Jared

And, success!

With the same prescaler and bias network as used by HP, the option board works!
I bought the prescaler chips from Aliexpress, they came loose in a non ESD plastic bag, s I was a bit dubious if they would be working or even genuine. Closer inspection revealed that they may be salvaged parts. Good for not being fakes at least......
However, on installing one, it turned out to work fine, nice.



There is a selected resistor (R6 in the HP design) that is specified as 316K, I stuck a 500K trimpot there and tweaked it until the counts reliably froze with no input and got a value of 288K. If I continued winding the trimpot until the display showed random numbers with a 3GHz input at it's lowest acceptable input level, I got 190K, so it seems this resistor does need to be selected for optimum operation (Or my more accurate 5.0V vreg has shifted the required value compared to the 5.1V zener regulator in the original design). I think something around 267K (that seems to be a standard value) should be fine.

I then ran the tracking generator from my 3.2GHz Siglent VNA into the input along with an 8481A power sensor hooked to a E4418B power meter using a BNC Tee
A bit of a crappy setup, but it gives a rough idea of performance.

Here's the results:



I need to get an 8482A to reliably test the low frequencies below 100MHz, but the option board locks onto a signal waaayyy down to 15MHz, not too bad! I can get a lock up to 3.1GHz, so the frequency range is a bit better than specs. Happy with that.
I found that my design needs a bit more power in the 2.7 - 3.0GHz range, HP specify -21dBm whereas I need -18dBm. Maybe some tweaking to the layout maybe something like the diode positions as mentioned by Tom Lee, or a third stage of amplification?

Here's a chart showing SWR, maybe someone can suggest some improvements from this too?




Anyway, as it is, I'm pretty happy with it so far. :)

Let me know if there's anything obvious I can improve on the next (hopefully final) revision if needed.



Jared

Awesome.

I think the easiest next experiment would be to remove one of the doubled-up diodes in each of the two places, and check the frequency response at the upper end.

Ed

Alright, fine, here's the money shot. :)



Sooo many zeroes! :D



Jared

Alrighty, now Christmas is done, it's almost time to order the final revision of the PCB's.

I have one last thing to figure out (If it even matters at 3GHz?)
To keep impedances as close to 50 ohms and VSWR low as possible etc etc etc, I have seen that for a through-hole RF connector into a coplanar waveguide, the ground plane should be pulled back around the connector's center pin.

Does anyone know how to calculate the required clearance? I'm using a standard 2 layer 1.6mm FR-4 PCB with 1oz copper.

Here's a picture of the board so far, you can see I pulled the ground plane back by an arbitrary amount to the left of the PCB for now, I just need to get that right and the PCB will be done ready for production.




Thanks!
Jared

"Jared Cabot via groups.io" <jaredcabot@...>
writes:

Alrighty, now Christmas is done, it's almost time to order the final revision of the PCB's.

I have one last thing to figure out (If it even matters at 3GHz?)
To keep impedances as close to 50 ohms and VSWR low as possible etc etc etc, I have seen that for a through-hole RF connector into a coplanar waveguide, the ground plane should be pulled back around the connector's center pin.

Does anyone know how to calculate the required clearance? I'm using a standard 2 layer 1.6mm FR-4 PCB with 1oz copper.

Here's a picture of the board so far, you can see I pulled the ground plane back by an arbitrary amount to the left of the PCB for now, I just need to get that right and the PCB will be done ready for production.

The proper way to calculate this is with an electromagnetic field
solver. OpenEMS is free and open-source and more than suitable for this
task. Others exist too (e.g., meep), but OpenEMS is probably the best
first choice (easiest to learn).

Learning to perform EM simulations such as this is not a trivial task,
but is well worth the effort and frees you up so that you don't need to
rely on calculators for this sort of thing, which don't exist for many
geometries and configurations and suffer accuracy limitations outside
the conditions in which they were designed to provide a reasonable
approximation. And, once you learn the process, they're not all that
hard to use.

At 3 GHz, you might be able to get away with ignoring the issue or just
guessing. And, with FR-4, you face significant uncertainty in terms of
material permittivity, so a nominal EM simulation will only be so useful
(you'd really want to perform a tolerance analysis).

The added metal from the center pin and via adds capacitance to the
transmission line, lowering the characteristic impedance, hence the need
to pull back the ground plane nearby. You might be able to try to
calculate this effect for your particular connector and setup, but it
would be easier and more accurate to just fire up an EM simulator.

I appreciate that this probably isn't the easy answer you were looking
for, but it is the best answer. This is how this is done professionally.

Some possibly useful resources:

-
-

Good luck,
Matt

Just another data point, I just powered up a 5334B counter with the 1.3GHz input C option. With no signal connected to input C it counts randomly. With a signal connected to input C it seems to work fine.
I have not tried to determine the minimum signal level yet or checked to see if there is a sensitivity adjustment internal to the counter.

ed

Ok, I took a look and tried to figure it out, but the calculations and simulations are far beyond my comprehension...

Does anyone here have the ability to run the simulation for this single through-hole pad? :)



Jared

Alrighty, PCB's were ordered, soldering iron was warmed up and I made some boards.

I took a stab at the connector through-hole pad to ground plane clearance and used the Saturn PCB toolkit software, treating the through hole as a via for the calculations.
It gave a clearance that seemed reasonable so I rolled with it.

I have tested one board so far, and it looks good enough for me to call it done for now.

In the attached graph, the blue line is the minimum signal strength required for the instrument to get a stable lock on the signal, and anything in the white area meets or exceeds HP spec on their original design.



Test setup was:
Function gen feeding into a 11667A splitter, one side to an N8482A power sensor connected to an E4418B Power Meter, the other side connected directly to the counter input (with attenuators added to provide lower signal levels than the power sensor could measure where needed).

Performance at the top end isn't as sensitive as I'd like, but without more knowledge or design help, I'm done for now, it works well enough for my purposes (maybe swapping from coplanar waveguide to a microstrip would reduce parasitic capacitance and help improve sensitivity?)


I'll release design files etc once I have it all sorted out and tidied up.


Jared.

Jared:

Is this the response curve of your board or the response of an HP/Agilent prescaler in the unit?

ed

Random related question but has anyone ever seen the option 124 board? This is the 12GHz one I think.?

I've never seen any 53131a over 3GHz and was just wondering.?

TonyG

On Fri, Mar 1, 2024 at 04:52 AM, Ed (scskits) wrote:

Jared:

Is this the response curve of your board or the response of an HP/Agilent prescaler in the unit?

ed

It's the response curve of the board.

I've uploaded the data here, so it should be easier to order boards if needed.
I can provide the original Diptrace PCB files on request if anyone wants to have a go at improving it.




Jared

Jared:

I was looking at the 53131A specs and the minimum input spec for 100MHz to 2.7GHz is -27dBm and from there to 3Ghz is -21dBm.
I guess actual levels would be less than that , but not significantly or Agilent would have taken credit for it.

For the channel A and B inputs the levels range from 20mV to 40mV (-21dBm to -15dBm if terminated in 50 ohms).

Your board must have a lot of gain at the low end for the minimum input to be below -50dBm for frequencies below 800Mhz as seen in the PNG image you posted.

Like you, I also noticed that the input protection diodes affected the signal levels. More effect than I expected.?

I am currently using two Mini Circuits ERA amplifiers for the gain stage with a 3dB attenuator in line with the input.

My minimum input levels from 750MHz to 3GHz are somewhat in line with the Agilent spec, -34dBm to -21dBm.
At 500Mhz, the input level drops to -13dBm, I think my input cap and those in line may be too small.

ed

Tony:

The 53131A had three options for the channel 3 input, 3GHz, 5GHz, and 12GHz.

I have never seen anything on EBAY over 3GHz installed in a unit.

I have seen Chinese Channel 3 boards for 3GHz (a lot of them) and 6GHz (just 1) currently listed.
I do not see the 12GHz board listed at this time, although it was listed in the past.

I did a board a few years back using the HMC432 (divide by 2) and two HMC434 (divide by 8) that could get to 6GHz or higher.

A less expensive version would use the HMC432 driving an MC12079 programmed to divide by 64, have the layout for it but never made it.

Never did any follow up on these because the Chinese clone boards were so inexpensive it was not worth pursuing.

ed