Dismiss Notice
Join Physics Forums Today!
The friendliest, high quality science and math community on the planet! Everyone who loves science is here!

Dual gate mixer help

  1. Sep 2, 2014 #1

    perplexabot

    User Avatar
    Gold Member

    Hello all. So i have been trying to simulate a ndg transistor mixer in LTSpice. Here is what I have so far, but I am missing something and I can't figure what it is... Here is the schematic along with the waveforms.
    dg_mix_v4.png
    For some reason the output will not go over 0.3V (do I have to bias it?). Anyone know what is wrong?

    Thank you for your time.
     
  2. jcsd
  3. Sep 2, 2014 #2

    analogdesign

    User Avatar
    Science Advisor

    You have to bias the second gate (G0) I think at a higher voltage than the first one (whatever the vdsat of gate one is).

    Think of a dual gate as a simple cascode amplifier (look it up in wikipedia). Then it will be obvious how to bias the two gates.
     
  4. Sep 2, 2014 #3

    davenn

    User Avatar
    Science Advisor
    Gold Member

    dunno if this helps

    here's an example of a working dual-gate MOSFET mixer in a VHF receiver
    that I have done much work on over the years

    attachment.php?attachmentid=72650&stc=1&d=1409717082.jpg


    Maybe give you some ideas :smile:
    as you can see there is no direct DC biasing applied to either of the gates

    cheers
    Dave
     

    Attached Files:

  5. Sep 2, 2014 #4

    perplexabot

    User Avatar
    Gold Member

    Thank you for your help. I have tried biasing both gates and nothing worked for me. So Vg2 = (Vg1 - Vto) + Vgs2 = 4 - 1 + 2 = 5?

    I am not sure if this is right. But here is the schematic with the biasing of G2 and the corresponding output. It is still not working :(
    dg_mix_v5-1.png
     
  6. Sep 2, 2014 #5

    perplexabot

    User Avatar
    Gold Member


    Hey! Thank you for that schematic and your help. Pretty cool, the dual gate mosfet seems to be used almost the same way. You pointed out it wasn't dc biased... It also isn't using emitter feedback... It is also using the tuned LC at the output to resonate the signal needed. I tried adding that LC circuit at the output but it still didn't help. I will study your schematic a bit more. Hmmmm. I wonder what is wrong...
     
  7. Sep 2, 2014 #6

    davenn

    User Avatar
    Science Advisor
    Gold Member

    no probs
    As said .. maybe an actual cct will give you some ideas to experiment with :smile:

    The output from the drain of the MOSFET is 10.7MHz, followed by L16 LC filter, followed by a 10.7MHz crystal filter

    The receiver is operating at ~ 151 MHz, therefore the LO is ~ 140 MHz

    cheers
    Dave
     
  8. Sep 3, 2014 #7

    vk6kro

    User Avatar
    Science Advisor

    The gate 1 resistor should return to ground, not to the source.

    The resistor and capacitor in the source circuit are there to develop a positive voltage on the source.
    Grounding the gate resistor makes the gate negative relative to the source, biasing it.

    Also, try reducing the drive voltage to a small value. Maybe 50 mV. This will stop overdriving the gate 1 input.
     
  9. Sep 3, 2014 #8

    perplexabot

    User Avatar
    Gold Member

    Thank you, so I have changed the G1 input to 50mV amplitude. This has had a dramatic effect on the output. So if I am not mistaken, one of the gate inputs will constantly turn on and off by going above and below the Vto (threshold voltage)? That is why you chose 50mV?

    So i also need to limit the incoming signal's voltage to 50mV... That's probably where a step down transformer would come in handy, right?

    Here are the waveforms and the new schematic.
    dg_mix_v6.png

    I believe it is working correctly now. Thanks...
     
    Last edited: Sep 3, 2014
  10. Sep 3, 2014 #9

    vk6kro

    User Avatar
    Science Advisor

    The FET Gate 1 has to be biased negatively relative to the source so that the input waveform does not drive the gate positive or more negatively than the cutoff voltage.

    So there is a region of negative voltage where the output should be a sinewave.

    You need to set the G2 voltage temporarily to some fixed value (say 2 volts DC) and get the output to be a clean sinewave, but hopefully larger than the input.

    After that, you can try applying an AC signal to G2. This signal should not drive G2 negative, so it must have a peak amplitude of less than 2 volts if that is the DC bias level on G2.

    You should not be getting square waves out.
     
  11. Sep 3, 2014 #10

    perplexabot

    User Avatar
    Gold Member

    So just to make sure I get this, you are saying, the first step is to dc bias gate 2 and send a sin wave through gate 1. Make sure to have a sin wave with some gain at the output.

    After this step is complete, REPLACE the dc bias at gate 2 with a sin wave who's peak does not exceed the previous DC bias. Is this correct? Or do we add (or superpose) the sin wave at gate 2 to it's dc bias? Basically, does the signal at gate2 ride a dc voltage or not?

    You say, I should not be getting square waves at the output? I am not getting any square waves at the output...

    Thank you for your help. I need to finish with this mixer once and for all.
     
  12. Sep 4, 2014 #11

    vk6kro

    User Avatar
    Science Advisor

    The AC signal on G2 should be superimposed on the DC voltage of about 2 volts. Try to optimise the level of this signal to get the best conversion gain. Ie best production of sum or difference products.

    20 volts supply is probably too much. Maybe 12 volts.

    The drain load should be about 1000 ohms. This will give more gain than 100 ohms.
    You should aim for about half the supply voltage across the FET from drain to source.

    Note that you will get an output of both input voltages (on G1 and G2) as well as the sum and difference of these.

    So, you need to filter out the ones you don't want.
     
  13. Sep 4, 2014 #12

    perplexabot

    User Avatar
    Gold Member

    Thank you. So right as soon as I bias gate2 at 2v DC, the output seems to be losing its "modulating effect." Here is a update schematic and waveforms:
    dg_mix_v7.png
     
  14. Sep 4, 2014 #13

    vk6kro

    User Avatar
    Science Advisor

    That model doesn't seem to be working as a mixer. Where did you get it from?

    My LTSpice doesn't seem to have a BF981 model in it.

    I can't read the parameters of your BF981 on my monitor, but maybe it isn't complete enough to work as a mixer?
     
  15. Sep 4, 2014 #14

    perplexabot

    User Avatar
    Gold Member

    Here is what i got from yahoo group LTSpice:

    Code (Text):
    *.SUBCKT BF981 1 2 3 4
    *Drain  Gate2 Gate1 Source  

    * Pin order changed in BF981 model
    *   1.: SOURCE;  2.: DRAIN;  3.: GATE 2;  4.: GATE 1;
    .SUBCKT BF981 4 1 2 3

    *Dual Gate Mosfet
    MD1 5 3 4 4 BF981A
    MD2 1 2 5 4 BF981B W=50U
    .MODEL BF981A NMOS (LEVEL=1 VTO=-1.1 KP=15M GAMMA=3.3U
    + PHI=.75 LAMBDA=3.75M RS=2.2 IS=12.5F PB=.8 MJ=.46
    + CBD=3.43P CBS=4.11P CGSO=240P CGDO=200P CGBO=20.5N)
    .MODEL BF981B NMOS (LEVEL=1 VTO=-.9 KP=18M GAMMA=19.08U
    + PHI=.75 LAMBDA=13.75M RD=41.3 IS=12.5F PB=.8 MJ=.46
    + CBD=3.43P CBS=4.11P CGSO=240P CGDO=200P CGBO=14.5N)
    * Philips
    * N-Channel Depletion DG-MOSFET
    .ENDS BF981
     
  16. Sep 4, 2014 #15

    vk6kro

    User Avatar
    Science Advisor

    OK

    Could you try grounding the bottom end of R7?
     
  17. Sep 4, 2014 #16

    perplexabot

    User Avatar
    Gold Member

    I just did that, and got the same result as the last image attached.
     
  18. Sep 4, 2014 #17

    vk6kro

    User Avatar
    Science Advisor

    The gain of the FET should be changing with G2 voltage and this model doesn't do that.

    Try this: remove everything from G2.
    Connect a voltage source to G2 and vary it from 0 volts to 12 volts using the DC sweep function. This is in the Edit Simulation Cmd section

    See if this has any effect on the gain of the FET.
    The output sinewave should get bigger with more G2 voltage.

    Where are you?
     
  19. Sep 4, 2014 #18

    perplexabot

    User Avatar
    Gold Member

    Hey, thank you for the input and sorry for the late reply. Here is the result of your suggestion. Interesting that it plateaus at around 9.25v. I wonder why. Here is the result:
    Green: V2 sweeped
    Blue: Output taken at drain of dgmos.
    dg_mixer_v8.png
     
  20. Sep 4, 2014 #19

    vk6kro

    User Avatar
    Science Advisor

    The output should be a sinewave but you would see it as varying thickness on the blue line.

    Try not plotting the sweeping voltage (the green line) and zoom in on the blue trace (by varying the voltage range in the vertical scale) to see if the thickness of the line varies across the screen.
     
  21. Sep 5, 2014 #20

    perplexabot

    User Avatar
    Gold Member

    Hey, I don't believe it is varying in thickness. I never even knew varied thickness was something to look at in LTSpice. Here is a plot:
    dgmixer_swOut.png

    Thank you.
     
Know someone interested in this topic? Share this thread via Reddit, Google+, Twitter, or Facebook




Similar Discussions: Dual gate mixer help
  1. Logic Gates Help (Replies: 2)

  2. And gate (Replies: 8)

  3. AND gate (Replies: 1)

  4. RF Mixer circuit help (Replies: 25)

Loading...