18
\$\begingroup\$

This question is an extension of Homebrew differential 'scope probe. I thought I should make this a new question though.

I need to measure a 100Mb/s LVDS signal to check its integrity. I will try to get hold of a 'scope with a 600MHz bandwidth, but I need a differential probe, and can't afford a real one. So I have designed a solution using the THS3201DBVT 1.8GHz current feedback op amp.

This is my first design using a current feedback amp, and my first high bandwidth design. I would be very grateful for any feedback (pun, sorry).

Differential probe schematic

Differential probe rendering

Differential probe layers

Added: Thanks to The Photon for suggesting removing the ground plane under the input pins of the OpAmps. Here's the layer just below the top layer, showing the new cutouts. The same thing has been done to the other layers too. Lower capacitance.

\$\endgroup\$
7
  • 1
    \$\begingroup\$ Input buffer amps should probably be connected with negative feedback instead of positive feedback. \$\endgroup\$
    – The Photon
    Apr 5, 2012 at 21:15
  • 1
    \$\begingroup\$ Ahem, er, yes. Spot the deliberate mistake to check who's paying attention... \$\endgroup\$ Apr 5, 2012 at 21:48
  • \$\begingroup\$ OK, I fixed the schematic. \$\endgroup\$ Apr 5, 2012 at 21:57
  • \$\begingroup\$ this is an interesting project, thanks for posting. Did you manage to get it built? Does it work? Gerry \$\endgroup\$
    – user11446
    Aug 11, 2012 at 23:51
  • \$\begingroup\$ A 50 ohm series resistor that matches the coax 50 ohm impedance which should also match the scope's 50 ohm input impedance would be good. This does provide a 2:1 reduction, but it will eliminate ringing etc. Also many op amps cannot drive much of a capacitive load. Use RG-174 as it is small and flexible. \$\endgroup\$ May 8, 2013 at 21:15

4 Answers 4

13
\$\begingroup\$

A classic layout rule for high-speed op-amps is to remove the power and ground planes beneath the nets connected to the input pins. You'll find this as the first bullet point in the PCB layout section of the datasheet for your op-amp.

That means, basically, remove all copper from the plane layers underneath any copper that is connected to pins 3 or 4 of your amplifiers.

Practically, it probably also means moving R1 and R2 closer to the input pins to minimize the size of the void you'll be cutting in the plane layers.

This has several benefits:

  1. Reduce the input capacitance of your circuit.

  2. Minimize ripples on the power and ground nets being coupled into the inputs of your circuit.

  3. Improve the stability of your circuit because some of those power/ground ripples may be caused by the varying current draw of the amplifier's output stage, resulting in unwanted feedback.

Another concern is with your decoupling capacitors. When you use multiple decoupling capacitors, if their values are different by more than about 1 decade (you have a factor of 1000 between 100 pF and 100 nF), it can result in an antiresonance at some frequency between the resonance frequencies of the two capacitors. This results in an exceptionally high power supply impedance at the anti-resonant frequency. This has been discussed, vaguely, around here several times recently, and its also documented in a Murata application manual. I'd advise to change your smaller decoupling capacitor to 10 nF.

\$\endgroup\$
6
  • \$\begingroup\$ Thanks Photon. Yes, I wondered about the ground plane. I'll make the change. About the capacitors: 100pF and 100nF are shown on the schematics on page 16. I also read the Murata app note, but I wasn't sure who to believe, so I went for the datasheet's suggestion. \$\endgroup\$ Apr 6, 2012 at 8:56
  • \$\begingroup\$ Anyway, the capacitor value is easy to change later if you have a problem...at least you know to look out for it. \$\endgroup\$
    – The Photon
    Apr 6, 2012 at 16:30
  • \$\begingroup\$ How will I recognize anti-resonance? \$\endgroup\$ Apr 6, 2012 at 18:58
  • \$\begingroup\$ Some kind of bad behavior at a specific frequency, probably somewhere between 10 and 100 MHz, like a low response or oscillation or ringing. \$\endgroup\$
    – The Photon
    Apr 6, 2012 at 23:30
  • \$\begingroup\$ Also it would be worth looking at the noise spectrum when you have nothing connected to the probe. If you see a peak in the 10 - 100 MHz range, you could suspect a capacitor problem. \$\endgroup\$
    – The Photon
    Apr 6, 2012 at 23:32
1
\$\begingroup\$

You don't have bulk decoupling for ground. Connect the middle of the CP1 and CP2 to ground.

Your input signal is between 0 and +3.3V. So no need for the -6 V rail, at least in this case. However that would make it a more general probe.

\$\endgroup\$
2
  • \$\begingroup\$ OK, that's fixed now. \$\endgroup\$ Apr 5, 2012 at 21:56
  • \$\begingroup\$ I made it +-6v to give the op-amps some headroom. Don't they prefer that? \$\endgroup\$ Apr 5, 2012 at 21:57
1
\$\begingroup\$

A series resistor (50 ohms) is a good idea. The scope should also be set for 50 ohms. The resulting scope trace will be 1/2 value, but the termination is critical for high speed signals.

I would also recommend a small (10-47pF) cap across each of the feedback resistors to improve stability. This will have an effect on frequency response, so check that against what you plan to measure. Use Tina-TI to simulate the response.

\$\endgroup\$
0
\$\begingroup\$

Does this really require 4 layers?

It looks to me like the only thing that's using +/- 6V are the op amps.

You might be able to cut down on cost significantly by using a 2 layer board, but it could affect your signal integrity (thus defeating the purpose of the design).

I hope someone chimes in on this point...

\$\endgroup\$
1
  • \$\begingroup\$ Possibly not, but it's a one off, and going in with a batch of other 4-layer boards. So cost isn't a problem. \$\endgroup\$ Apr 6, 2012 at 8:17

Not the answer you're looking for? Browse other questions tagged or ask your own question.