Post Go back to editing

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.

  • 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.

  • 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.

  • 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

  • Hello SMcBride,

    with respect your explanation, in the gerber file of the amplifier I see the bypass capacitors far away from the power supply pins of part. I don't understand...

    Anyway, your explanation helped me to understand how to cascade the two amplifers.

    Many thanks.

    Best regards,

    Antonio L.

  • Hi Antonio,

    Yes, for the HMC618A the bypass caps are out past the inductors. When I was talking about the bypass caps I was more thinking about some of our other products that don't have inductors right near the pins but instead have caps very close to the pins with just short lengths of PCB trace between cap and pin. For the HMC618A my recommendation is to follow the top layer layout shown in the gerber files as closely as possible with respect to the positions of the inductors and bypass caps for the Vdd1 and Vdd2 traces, then connect them together out past those caps (i.e. farther away from the part). Once past those caps, you should be able to connect all of the drains together (for both amps in your cascade) without causing problems.

    With most (or possibly all) of our HMC parts we generally recommend to customers that, in order to obtain performance similar to that shown on the data sheet and to increase the chances of first-pass success with their designs, they follow our EVB gerbers as closely as possible. That includes not just the traces but also the grounds and ground vias. Grounds and ground via diameter, quantity, placement, and type (PTH vs. solid/filled, etc.) can have significant effects on both the electrical and thermal aspects of circuit performance. If the thermal considerations are new to you and/or you're interested to learn more about them, here is a link to a relevant application note:

    http://www.analog.com/media/en/technical-documentation/application-notes/thermal_management_for_surface_mount_components.pdf

    If your design uses a different stack-up than our EVB then you might need to make adjustments to some of the trace widths and gaps in order to maintain the same trace impedance. Stack-up differences might also require you to increase your ground via coverage (for thicker substrates) or allow you to decrease your ground via coverage (for thinner substrates). As always with RF design, there are many factors to take into account.

    I'm glad that you found this discussion helpful. Let me know if you have more questions.

    Regards,

    SMcBride 

  • Hello,I am now also try to use HMC618A ,I plan to use it @1400MHz and  trying to find the gerber file of EVM board (1200 - 1700 MHz tuned) ,the part number is EV1HMC618ALP3,but the file provided was 1700 - 2200 MHz tuned,So could you please help me find the gerber file?

  • Hi reeze,

    I have submitted to our website team a request that the 1200-1700 MHz eval board gerber files be uploaded to the HMC618A product page. Several days may elapse before the upload and link become active.

    In the meantime, please see the attached gerber files for EV1HMC618ALP3.

    Regards,

    SMcBride

    EV1HMC618ALP3_gerber.zip