Colpitts generator Pspice

Discussion in 'Programmer's Corner' started by arek462, Jun 28, 2016.

  1. arek462

    Thread Starter New Member

    Jun 28, 2016
    15
    0
    Hello!

    I tried simulate Colpitts Generator from Horowitz's book:

    colpitts.png

    I use free pspice version, so there isn't crystal:

    colpitts_schematic.png

    Unfortunately it doesn't work like generator:

    colpitts_simulation.png

    If any expert could help me make it work right, i will be very grateful.

    Thank you!
     
  2. Bordodynov

    Active Member

    May 20, 2015
    643
    188
    See

    Draft300.png Draft300_plot.png
     
    arek462 likes this.
  3. arek462

    Thread Starter New Member

    Jun 28, 2016
    15
    0

    Thanks for your help!

    Now i have problem with "floating node".

    Błąd.png
    How did you set ic=1mA because it may help?

    Also i have problem with "Undefined layout format....". It shows after i added my own transistor:

    element.png

    Thank you!
     
  4. Bordodynov

    Active Member

    May 20, 2015
    643
    188
    floating node ==> comon node C1 and C7 add resistor 1Gig.
    IC = 1mA to speed up the calculation. It should .Tran 50m UIC. If you want to see the launch of the generator without these options, you must apply voltage leap. Note that I am one of the reduced capacities of up to 200 pF. There was no generation. Perhaps at a higher quality factor is generated. The lower quality factor, the faster the calculation.
    .model 2n5485 njf(is=.25p alpha=1e-4 vk=80 vto=-2.0 vtotc=-3m beta=3.5m lambda=10m betatce=-.5 rd=10 rs=10 cgs=4p cgd=4p kf=3e-17 )
    In your model, the transistor is too small capacity. See datasheet. Also, your transistor transconductance more than three times less. You may need to further reduce the capacity of the C3 (~100pF).
     
    Last edited: Jun 29, 2016
    arek462 likes this.
  5. arek462

    Thread Starter New Member

    Jun 28, 2016
    15
    0
    You mean add parallel resistor 1G?
    I've change C3 to 100p.
    How add .Tran 50m UIC?
     
    Last edited: Jun 29, 2016
  6. Bordodynov

    Active Member

    May 20, 2015
    643
    188
    The resistor is attached to the ground with one pin (you can parallel capacitor).
    Look in the job analysis. The option uic is valid for all Spice program (and for Pspice, ORCAD)
    I corrected my previous post!
     
    Last edited: Jun 29, 2016
  7. arek462

    Thread Starter New Member

    Jun 28, 2016
    15
    0
    Thank you.

    I added resistor and the floating node problem is gone. Howewer, circuit still doesn't work like i expected. Please help

    Node.png
     
  8. Bordodynov

    Active Member

    May 20, 2015
    643
    188
    You still get your hands on the option "uic".
    In another (initial voltage boost).
    Draft302.png
     
  9. arek462

    Thread Starter New Member

    Jun 28, 2016
    15
    0
    I really don't know how to make this tran 50m.

    Do you mean this?

    Błąd.png

    I should change only dc in source parameters??
     
  10. arek462

    Thread Starter New Member

    Jun 28, 2016
    15
    0
    I've change some simulation parameter and i got this:

    Błąd.png

    Is it correct?

    Thank you!
     
  11. Bordodynov

    Active Member

    May 20, 2015
    643
    188
    in Spice R3=1M=1m=0.001 !!! need 1Meg=1meg=1000000=1e6=1000k
     
    Last edited: Jun 29, 2016
  12. arek462

    Thread Starter New Member

    Jun 28, 2016
    15
    0
    Yea, you are right. My mistake.

    I change resistor's value to 1 Meg and now it looks this:

    Błąd.png
     
  13. Bordodynov

    Active Member

    May 20, 2015
    643
    188
    Just give me image of a circuit. Without waveforms. So that I can better see your circuit. Resistor correct. On waveform output power node. I want to be sure that in the zero voltage momet time zero and then changed to 24 volts.
    You may need to increase the accuracy of the calculation. Make reltol=10u. I did that when counting crystal oscillators. and I used Pspice4.
     
    Last edited: Jun 29, 2016
  14. arek462

    Thread Starter New Member

    Jun 28, 2016
    15
    0
    Now i know what you meant.

    So in the beginning voltage must be 0 and then after some short time 24V.
    Do you how to set it?

    Błąd.png
     
  15. Bordodynov

    Active Member

    May 20, 2015
    643
    188
    Yes, you understood me correctly. I usually use front enable 1 microsecond, but it is possible and faster. This gives the initial impetus fluctuations. And further. Do not use the default transistor. In the second scheme, I took the same model that you take.
     
    arek462 likes this.
  16. arek462

    Thread Starter New Member

    Jun 28, 2016
    15
    0
    So, what do you advice?

    Now i use this transistor .model 2n5485 njf(is=.25p alpha=1e-4 vk=80 vto=-2.0 vtotc=-3m beta=3.5m lambda=10m betatce=-.5 rd=10 rs=10 cgs=4p cgd=4p kf=3e-17 ).

    What should i do to get the same waveform like you in your first post?

    http://forum.allaboutcircuits.com/attachments/draft300_plot-png.108432/
     
  17. arek462

    Thread Starter New Member

    Jun 28, 2016
    15
    0
    Amplitude is to small. I don't understand it:

    Błąd.png


    I upload schematic.
     
    Last edited: Jun 29, 2016
  18. Bordodynov

    Active Member

    May 20, 2015
    643
    188
    You can simulate a text file. ORCAD allows you to do it.
    * D:\Program Files\LTC\LTspiceIV\Draft302.asc
    r1 g 0 1meg
    j1 out g 0 j2n5485
    r2 VCC out 4.7k
    c1 out n002 1000pf
    c2 out 0 1000pf
    c3 0 g 200pf
    l1 p001 g 0.159154943091895
    c4 p002 p001 1.59154943091895e-013
    r3 n002 p002 100
    c5 n002 g 2e-012
    v1 VCC 0 pwl(0 0 1us 24v)
    r4 n002 0 1g
    .model j2n5485 njf(beta=1.039m betatce=-500m rd=1 rs=1 lambda=4.25m vto=-2.5
    + vtotc=-2.5m is=33.57f isr=322.4f n=1 nr=2 xti=3 alpha=311.7 vk=243.6
    + cgd=1.6p m=362.2m pb=1 fc=500m cgs=2.414p kf=7.832e-003f af=1)
    .tran 0 50m 0 .1u
    .option reltol=1u
    .probe V(out) V(g) V(vcc)
    .end
     
    • gen.cir
      File size:
      581 bytes
      Views:
      2
  19. arek462

    Thread Starter New Member

    Jun 28, 2016
    15
    0
    I use pspice
     
  20. Bordodynov

    Active Member

    May 20, 2015
    643
    188
    This file is for Pspice. ORCAD Pspice uses. Before the calculation of the graphical design turns a text file. The text file and is used for the calculation. I used ORCAD9.1 and ORCAD9.2. They allow you to count text files, as well as other SPICE-program. I did it. Start my file!
     
Loading...