Guidelines for two cascaded amplifers (hmc618a)

Hello everyone,

for our telecom system, we need to cascade two selected amplifers (hmc618a, 1700 - 2200 MHz tuned) in order to obtain more than 30 dB gain.

We thought to follow the datasheet reference design.

Are there some guidelines or issues we have to know to do that? Or Have you some advices?

Could the two cascaded stages oscillate?

Many thanks.

best regards,

Antonio L.

  • 0
    •  Analog Employees 
    on May 19, 2017 9:32 PM over 3 years ago

    Hi Anton*89,

    Yes, the two cascaded gain stages could oscillate if the oscillatory criterion are met. To minimize the chances of that happening, I recommend that you try to maintain a good match between all RF ports to minimize reflections and maintain isolation between the DC bias networks by not ganging together the drains. Follow closely the layout shown on our EVB, using the gerber files found here: 

    http://www.analog.com/media/en/technical-documentation/evaluation-documentation/gerber-files/HMC618_1700-2200MHz-HMC618A-HMC717-HMC717A-Gerber.zip

    Possibly include provisions on your PCB to increase the RF isolation between the DC bias networks of the two amps and make sure to provide adequate capacitive bypassing for each amp.

    Regards,

    SMcBride

  • Hello SMcBride,

    thank you for reply.

    Is it possible to have the BOM (part list) used for evaluation board?

    Many thanks

    Best regards,

    Antonio L.

  • 0
    •  Analog Employees 
    on May 24, 2017 12:06 AM over 3 years ago

    Hi Antonio,

    Please see the attached LM in Excel format. Manufacturer names and part numbers are included. For many items there are several acceptable part numbers, which you will see in the form of multiple entries for Part Number (column C). Let me know if this is not clear. 

    There were some other questions to which I started to draft answers...but it appears that those questions have been deleted. Do those questions remain or do you no longer need answers?

    Regards,

    SMcBride

    HMC618ALP3E_1700-2200MHz_EVB_LM.xlsx
  • Hello SMcBride,

    I would like to thank you for all support you gave us.

    Regarding the deleted questions, I've deleted them accidentally. We would still need the answers to those questions.

    Many thanks.

    Best regards,

    Antonio L.

  • 0
    •  Analog Employees 
    on May 25, 2017 3:05 AM over 3 years ago

    Hi Antonio,

    What I have in my email alert are the following questions which are what I think you said were accidentally deleted:

    Could you explain a little bit better the sentence: "maintain isolation between the DC bias networks by not ganging together the drains"? What does the sentence "by not ganging together the drains" mean? Do we have to respect the layout shown in the gerber file literally? Even about the length of the trace on the RFin and RFout (from amplifier pin to the SMA connector)?

    What I meant was to make sure that your PCB layout does not allow feedback of RF from Vdd2 to Vdd1, for example. With high gain RF amps RF signal can sometimes couple from Vdd2 back to Vdd1 (for example) and contribute to oscillation. Notice how the EVBs make the Vdd1 and Vdd2 traces diverge from one another and orient L1 and L3 perpendicular to each other. I would recommend that you take the same approach on your PCB. By "not ganging the drains together" I was thinking more about our other amps that have bypass capacitors as the DC bias components closest to the part. In those cases you would not want to connect Vdd1 and Vdd2 together very close to the DUT pins, but rather you would want to keep their respective bypass caps as close to the DUT pins as possible and only connect the Vdd1 and Vdd2 traces together once they have reached a much greater distance away from the part. These concepts apply to individual parts as well as to your cascade of two parts on the same PCB; connect DC drain lines together only at points farther away from the part than the bypass caps.

    You don't have to follow the gerber layout exactly, but it can be considered as a good example of a successful design with this part. In your design you might choose (or need) to use different materials/a different stack-up that makes is necessary to deviate from our layout and stack-up. The length of the RFIN and RFOUT traces are not important, they are just 50 ohm transmission lines interfacing with the DUT's 50 ohm RFIN and RFOUT ports. You may have noticed the odd, wide pads to which the SMA connectors' center conductors get soldered. Those wide pads are not intended to provide tuning for the part but rather they are used because the main RF layer is 10 mil thick while the overall PCB thickness is 0.062" thick with SMAs . You will notice from the Gerber files that the internal ground layers MET-2 and MET-3 have been voided directly beneath that SMA pin so that the bottom layer MET-4 (0.062" away) functions as the RF ground reference at and near the RF launch and then transitions to where the MET-2 layer has become the RF ground reference for the remainder of the path the DUT pin.

    Regards,

    SMcBride