I am attempting to build the following amplifier

  • The amps used are MAR-8A+'s from minicircuits
  • C1, C2, C3, L1 - while these are available on the board they have not been placed
  • The filters are epcos saw filters with a Pass Band Frequency: 433MHz to 434.71MHz

    I have designed and built the following PCB:

Upon building it the first few times I found the amps were blowing, I changed the resistor values and seem to have fixed this (schematic shows updated values).

Then I discovered it was oscillating, after fiddling with the physical power connections I found using pins and croc clips did not work and resorted to soldering wires on. This fixed the issue on the boards and subsequent ones up until now.

However recently they have started oscillating again at approx. 433MHz. First off it is just small oscillations, and then when the antenna is attached they multiply massively. I have noticed there is interference at 1.825 GHz and 945 MHz, this happens even when the board is not populated. As the board size is a quarter wavelength of the higher frequency I suspect this may have a lot to do with it.

I think I may also be needing the front end tuning that I have left out (due to not being able to make it accurate enough). Is there anything major I have missed? such as 50 ohm matching and termination?

Example Traces:

Many Thanks, let me know if I have missed any important info and I will add it.

  • 4
    \$\begingroup\$ Just a tip: to prevent your amps from blowing, make an estimate of how much current the circuit needs. Then use a current limited power supply to feed the circuit and set the current slightly higher than the value you estimated. That way the power is limited and your amps should be safer. \$\endgroup\$ – Bimpelrekkie Nov 17 '15 at 16:20

Those amplifiers have 30dB+ gain each. You need a longer, skinnier board, to keep the output tracks further away from the input tracks.

I presume the board is solid ground plane on the reverse? If not, that needs doing. The peppering with vias suggests that that is it ground, and also that you have top ground. Let's have a look at the copper on all the layers.

I don't know what the board thickness is. I would guess that the signal path through the board is not 50\$\Omega\$, as the tracks look quite thin. Rule of thumb for FR4 and 4350, a microstrip track should be 2 substrate thicknesses wide to be roughly 50\$\Omega\$ impedance.

I hope those Epcos filters are 50\$\Omega\$ match. Add their part number, or better still a link to the data sheet to your question. I notice they do filters that while the data sheet is headed 50\$\Omega\$, they require matching inductors.

Generally, your layout looks like the first RF design you've ever done. It looks like a low frequency design, with long tracks, wandering about coupling with their neighbours.

The signal path through should be microstrip. The bias inductors should be right on top of the amps. The bias resistors should go directly to a good short decoupling C. Your decoupling caps C9, 10 etc are too long. These bias loops should be away from other stuff.

  • \$\begingroup\$ Yes board has copper ground plane on both front and back. Have added the link to the saw filters. I don't understand what you mean about FR4 and 4350? Board thickness is 1mm. Will take on board the other points and tweak my board. As you have said it was my first RF design. \$\endgroup\$ – Stuart Rayner Nov 18 '15 at 9:21

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.