3
\$\begingroup\$

I am currently designing a prototyping board for fast pulse detection with 4 amplification stages at the input. I am currently not able to provide a schematic portion of it as I don't have access to it right now, but I can provide it if requested.

Some info on the amplification stage :

  1. The frequency range I am interested in is between 10 MHz and 400 MHz.
  2. I have 3 different 50 Ohm matched RF amplifier ICs, one having a low noise figure and the other two for general purpose amplification. The stages will be somewhat similar to the following :

    FILTER -> A1 -> FILTER -> A2 -> A3 -> A3 -> FILTER

  3. I am planning to make the board 4 layers, with the stack-up SIG|GND|PWR|GND, although I am not sure.

  4. In the layout, A2 and first A3 will be by-passable via alternate routing through 0 ohm resistors.

I have no experience in laying a board like this, although I diagnosed and reviewed some. In one of my DigiKey researches, I stumbled upon some easy to use PCB mount RF shield enclosures and thought they might be a good idea to use. The max amplification will be around 110 dB. Which means I will be mostly amplifying noise. From my understanding those shielding products offer protection against inter-stage coupling of the signals in a layout like this, apart from their EMI shielding capabilities. I have some confusions and questions about this:

  1. Is there a chance that the shield will degrade an amplifier's performance by providing a radiating structure due to a signal leakage under the placed amplifier?
  2. When shielding stages, should I include close-by filters and other passive elements in the enclosure as well?
  3. Would the correct placement and performance evaluation of such shields be hard? I have a very tight schedule and I certainly can't test the effectiveness of them.
  4. Should I instead try to encapsulate all the amplifier stages in one shielding block? I don't mean an outer enclosure for the PCB as I will probably make one.

I am at least willing to try some of this as this will be a complete prototyping board anyway, but I would be very glad if I could gain some insight on the issue. Thanks in advance!

\$\endgroup\$
  • \$\begingroup\$ Are these pulses? or tone bursts? sinusoids will be more vulnerable to resonances in the gnd/vdd/signal chain \$\endgroup\$ – analogsystemsrf Apr 26 '17 at 6:06
  • \$\begingroup\$ These are bipolar pulses of approximately 1 ns width. The frequency spectrum of the pulse covers a range of 1 - 340 MHz approximately. I am filtering in between 20-240 MHz with 3rd order butterworth filters. But I see your point, and actually we are completely amplifying thermal noise in that frequency region so we have every frequency enough for oscillation unfortunately. \$\endgroup\$ – Çağlar Kutlu Apr 26 '17 at 6:57
  • \$\begingroup\$ A 1ns pulse cannot have a spectrum that only extends to 340MHz, the math does not work. If the pulses are 1ns then you actually need gain out to well over 1GHz, or they will be low pass filtered out by your amplifiers, really for a pulse you would want at least 5GHz of reasonably flat gain (And that only gets you fundamental plus a few harmonics, there will be pulse smearing and maybe some ringing). \$\endgroup\$ – Dan Mills Apr 26 '17 at 12:11
  • \$\begingroup\$ I'm sorry, I should have mentioned that my usage of "pulse" here is a smooth function over time that has a well defined peak in a well defined time period, which is 1 ns, not a square pulse. The signal is of an analog nature and a little bit stretched out version of the derivative of a gaussian with a sigma of 1 ns. \$\endgroup\$ – Çağlar Kutlu Apr 26 '17 at 13:02
2
\$\begingroup\$

There are several factors to consider when assembling RF amplifiers in VHF range on a pcb. No claim of being exhaustive, just some thoughts for discussion.
1) amplifiers need supply that in turn need decoupling: this is the path #1 for undesired effects; in an old project I was distributing power to several modules using large traces from a common +28V and decoupling with pi C-L-C circuit; traces and not a single plane to avoid common impedance coupling through V+. For large power, and large current since supply voltage is never above some tenths of Volts, you need to design for heat dissipation in your traces (e.g. 35/70 micron of copper, outer traces for power, ...).
2) Spread around capacitors to improve supply impedance at VHF; not such a high frequency to require distributed capacitance, e.g. through pcb itself.
3) useless to say, a good ground plane gives capacitors a good reference and is beneficial to reduce ringing
4) you say that A2 and A3(1) can be bypassed by 0ohm resistors: consider that all these modules shall be fed with transmission lines built for 50 ohm (or whatever it is) characteristic impedance; those 0 ohm are a discontinuity and a cause of mismatch for return loss and backward power. Better if you use RF relays or you manually reconfigure a coax line.
5) if amplifiers are modules in metallic housing, probably they are already well shielded; if they are components/hybrids, then shielding is necessary as you propose, but ... first, the shield might electromagnetically load and change module response (not dramatically), and, second, considering your 110 dB gain, keep amplifiers and filters separated, using metallic separators, otherwise noise pickup between output and input and oscillations are likely to occur. What is normally done when using some kind of shielding enclosure is to use coax capacitors for decoupling when passing through the wall.
6) consider distributing signals as striplines inside the power layers, rather than microstrips, to reduce stray coupling and radiation; frequency is low enough so that both work from a purely RF viewpoint.

\$\endgroup\$
  • \$\begingroup\$ Thanks a lot for answering and general useful insights. 1) The board will have 8 identical & parallel amplification signal paths that will have their power distributed from a single connection to the PCB. So this is very much another point of decision for me. I am calculating that a single channel will have around 250 mA current with 50 ohm terminations almost everywhere. Do you think that I should change my layer stack-up? \$\endgroup\$ – Çağlar Kutlu Apr 26 '17 at 0:44
  • \$\begingroup\$ 2) Agreed 3) Agreed 4) I think I should go with 0 ohms, or maybe other jumper configuration? 4) Will think about it. 5) Custom metallic separators seems mechanically difficult to me, do you suggest that I layout premade SMD shielding gaskets for each amplifier and filter separately? Also, I don't really know about coax capacitors. Do I need to connect my trace leaving the shielding with such component or are you suggesting this for coax feeds? 6) I will think about this. Thanks! \$\endgroup\$ – Çağlar Kutlu Apr 26 '17 at 1:03
  • 1
    \$\begingroup\$ a) 250mA not large, thought you were in hundreds W range. Everything is SMD, then. b) you may think of PWR, GND, SIG, GND if only 1 SIG needed: PWR dissipates better and SIG refers well to GND. c) shielding is not such an headache: take a sheet of 0.2-0.5 mm Cu, tinned Cu, brass: cut it so to fold to create a small cube, solder it to pads on pcb (maybe with some short wires emerging from pcb vias to keep it in place). d) ..if you really need such shielding; ground traces around your ampli chips will help in any case. e) forget about coax stuff if all is smd. \$\endgroup\$ – andrea Apr 26 '17 at 7:21
  • \$\begingroup\$ Thanks a lot! I was thinking to make the signal layer on top for better diagnosis and modifications if necessary, this will be the first prototype so I'm trying to get it done as a demo board. What do you suggest for a SIG on top stackup? \$\endgroup\$ – Çağlar Kutlu Apr 26 '17 at 7:32
  • 1
    \$\begingroup\$ One tip with cascaded amplifier stages is to do the layout to accommodate an interstage pad between each stage, a few dB of resistive Pi attenuator can make one hell of a difference to stability, and is unlikely to cost you noise performance if the LNA has reasonable gain. \$\endgroup\$ – Dan Mills Apr 26 '17 at 12:07
1
\$\begingroup\$

Is there a chance that the shield will degrade an amplifier's performance by providing a radiating structure due to a signal leakage under the placed amplifier?

I don't know what you mean by this, use circuit theory to model what is going on in a cable. As in the diagram below from here. Electric fields couple via capacitance, Magnetic fields via inductance. It can be hard to model in the prototyping stage, usually you try your best and if you see noise in your signal you change the cable or the circuit (but it can be modeled, but usually with some kind of experiment with the actual cable)

Shielding blocks electric fields, but not magnetic. The other problem with shielding is you cannot have a large current running on the outside of the shield, or it will couple magnetically (via mutual inductance) to the inner conductor and create noise.

Shields also block noise from the conductor on the inside to the outside, and the shield is usually tied to chassis ground or PCB ground. If there is noise on these grounds, it can turn the shield into a nice antenna.

enter image description here

When shielding stages, should I include close-by filters and other passive elements in the enclosure as well?

The ideal shield would enclose all electronics and your sensor to keep any stray electric fields from impinging on your device, try and follow an ideal shield as closely as possible. If you think that there will be a crosstalk between amplifier stages, model this as a capacitor of a few pf's between stages (or 10's pfs as an upper bound) to simulate electric fields through air. If this caueses problems for your design, you may need to put shielding between stages. The ammount of capacitance will depend on the design of your board, but can be calculated with pcb trace calculators.

Would the correct placement and performance evaluation of such shields be hard? I have a very tight schedule and I certainly can't test the effectiveness of them.

If this is the case, then build in a solution before you build the board. For example, if you are unsure if you need shielding between stages, find an EMI gasket or copper wall that you could install later. Try it without and then add it later if needed. Copper tape goes a long way in prototyping, and if you only have small quantity for production, just use copper tape. Or if your manufacturing the shield (like with a CNC) then just build one shield with multiple rooms.

Should I instead try to encapsulate all the amplifier stages in one shielding block? I don't mean an outer enclosure for the PCB as I will probably make one.

Yes, for mechanical\machining reasons.

\$\endgroup\$
  • \$\begingroup\$ Thank you for your valuable response. The amplifiers I am using are of SMT type ICs, not shielded amplification blocks so I am not connecting them with cables. I don't know if that's what you thought. Thank you for the shielding suggestions. From what I understand, you are saying that I should aim for the full enclosure shielding first. I think 1-10 pF coupling in-between stages would definitely cause some serious problems. Do you think there could be that much capacitive crosstalk? I think I will follow your advice on EMI gasket if I can lay the mounting pads properly. \$\endgroup\$ – Çağlar Kutlu Apr 26 '17 at 1:06
  • \$\begingroup\$ For some reason I thought you had a cable in your design, the point is, if you don't have currents running through the shield you won't have a problem from an electric field. Look at how there is coupling inside the cable, the same goes for conductors inside of a shield. The shield potential needs to be zero \$\endgroup\$ – laptop2d Apr 26 '17 at 3:26
  • \$\begingroup\$ So from what I understand, suppose that I have shielded an amplification stage with a surface mount shielding gasket with appropriate placement of pads around the area and vias to the ground plane at every pad (i am just assuming this, is that good practice?) The signal return path should be from the ground plane not from the shield itself. Is that correct? And if it is so how can I ensure such a thing? \$\endgroup\$ – Çağlar Kutlu Apr 26 '17 at 4:05
  • \$\begingroup\$ Yes, if you have ground surrounding the bottom of the shield and low impedance to the shield then the shield will be the same potential. 10pf is a high number upper bound, it depends on the signal and the spacing. Use a pcb trace calculator to find mutual capacitance. Get electromagnetic compatiablity engineering by henry w ott \$\endgroup\$ – laptop2d Apr 26 '17 at 4:10
0
\$\begingroup\$

Here is one of the challenges with broadband amplifiers

schematic

simulate this circuit – Schematic created using CircuitLab

\$\endgroup\$
  • \$\begingroup\$ I guess I see your point. The amplifiers I am using for the gain block are 50 ohm matched transistor amplifiers for DC - 2GHz (BGA427, BGA28{69,51}). In the datasheet it says they are unconditionally stable so I actually didn't give it a much thought apart from trying to do best practices. Are you saying that such shielding could cause an inductive coupling that will make the circuit oscillate? If so I am guessing there is no way to figure it out without trying. What I am scared of is the current-feedback opamp stage I employ after amplification. \$\endgroup\$ – Çağlar Kutlu Apr 26 '17 at 7:05

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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