555 oscillator simulation in circuit maker

Discussion in 'Homework Help' started by mitza_h, Apr 12, 2010.

  1. mitza_h

    Thread Starter New Member

    Jun 24, 2009
    9
    0
    for my school project i chose "galactic voice changer" (from a 2008 epe magazine ), and as part of my project i need to simulate the functional blocks of the circuit. my problem is that i can't seem able to simulate in circuit maker the oscilator. there should be an output of about 50 mV but what i get is of uV magnitude. the only thing that i changed from the original circuit is a normal 555 timer instead of a cmos555 timer. any help is appreciated !
     
  2. R!f@@

    AAC Fanatic!

    Apr 2, 2009
    8,754
    760
    What is ur timer no. Is it a TTL version?
     
  3. mitza_h

    Thread Starter New Member

    Jun 24, 2009
    9
    0
    what number are you refering to? it's TTL, it's internal structure is made of gates and a flip-flop
     
  4. MAB

    Member

    Dec 30, 2009
    20
    1
    My circutmaker student version did the same thing until I switched over to the UA555 model.
    I suspect that the UA555=TTL, 555=CMOS???
     
  5. R!f@@

    AAC Fanatic!

    Apr 2, 2009
    8,754
    760
    the no. on the IC , the timer 555 something.. hello...
    gimme a no.
     
  6. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    The 555 is just a macromodel.
    The UA555 is a component model.

    Use the component model.

    If you try to run either too fast in Circuitmaker, you will have a reduced output from pin 3.

    Basically use a range of, 1/400th to 1/1000th of the start-stop time to get sufficient data points without taking a week to run. For example, if you're running an analysis 10mS in duration, use 10uS for step/max step. If you want more resolution, you can always decrease the step/max step. If you want it to run faster, increase step/max step.

    Checking the UIC box will help avoid cryptic errors when starting the transient analysis of an astable multivibrator.
     
  7. MAB

    Member

    Dec 30, 2009
    20
    1
    Ok Sarge, I don't mean to hijack the thread but...
    what's the difference between the models?
     
  8. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    Component model:
    Code ( (Unknown Language)):
    1. *Sngl Timer (Component Model) pkg:DIP8 1,2,3,4,5,6,7,8. pkg:DIP14 1,3,4,6,8,10,12,14. pkg:CAN8 1,2,3,4,5,6,7,8.
    2. .SUBCKT XUA555 99 32 30 19 23 33 1  21
    3. Q4 25 2 3 QP
    4. Q5 0 6 3 QP
    5. Q6 6 6 8 QP
    6. R1 9 21 4.7K
    7. R2 3 21 830
    8. R3 8 21 4.7K
    9. Q7 2 33 5 QN
    10. Q8 2 5 17 QN
    11. Q9 6 4 17 QN
    12. Q10 6 23 4 QN
    13. Q11 12 20 10 QP
    14. R4 10 21 1K
    15. Q12 22 11 12 QP
    16. Q13 14 13 12 QP
    17. Q14 0 32 11 QP
    18. Q15 14 18 13 QP
    19. R5 14 0 100K
    20. R6 22 0 100K
    21. R7 17 0 10K
    22. Q16 1 15 0 QN
    23. Q17 15 19 31 QP
    24. R8 18 23 5K
    25. R9 18 0 5K
    26. R10 21 23 5K
    27. Q18 27 20 21 QP
    28. Q19 20 20 21 QP
    29. R11 20 31 5K
    30. D1 31 24 DA
    31. Q20 24 25 0 QN
    32. Q21 25 22 0 QN
    33. Q22 27 24 0 QN
    34. R12 25 27 4.7K
    35. R13 21 29 6.8K
    36. Q23 21 29 28 QN
    37. Q24 29 27 16 QN
    38. Q25 30 26 0 QN
    39. Q26 21 28 30 QN
    40. D2 30 29 DA
    41. R14 16 15 100
    42. R15 16 26 220
    43. R16 16 0 4.7K
    44. R17 28 30 3.9K
    45. Q3 2 2 9 QP
    46. .MODEL DA D (RS=40 IS=1.0E-14 CJO=1PF)
    47. .MODEL QP PNP (BF=20 BR=0.02 RC=4 RB=25 IS=1.0E-14 VA=50 NE=2)
    48. + CJE=12.4P VJE=1.1 MJE=.5 CJC=4.02P VJC=.3 MJC=.3 TF=229P TR=159N)
    49. .MODEL QN NPN (IS=5.07F NF=1 BF=100 VAF=161 IKF=30M ISE=3.9P NE=2
    50. + BR=4 NR=1 VAR=16 IKR=45M RE=1.03 RB=4.12 RC=.412 XTB=1.5
    51. + CJE=12.4P VJE=1.1 MJE=.5 CJC=4.02P VJC=.3 MJC=.3 TF=229P TR=959P)
    52. .ENDS XUA555
    53.  
    Macromodel:

    Code ( (Unknown Language)):
    1. *Sngl Timer (Macromodel) pkg:DIP8 1,2,3,4,5,6,7,8. pkg:DIP14 1,3,4,6,8,10,12,14. pkg:CAN8 1,2,3,4,5,6,7,8.
    2. .SUBCKT X555 1 2 3 4 5 6 7 8
    3. EREF 15 1 8 1 .5
    4. GSOURCE 8 3 8 26 12.5E-3
    5. GSINK 3 1 26 1 67E-3
    6. VD1 8 27 DC .8
    7. VD2 28 1 DC .85
    8. VREF 30 1 DC 1.2
    9. C1 29 1 700E-15
    10. RREF2 30 1 100E3
    11. RREF 15 1 100E3
    12. ROUT 3 1 100K
    13. R1 6 1 500E9
    14. R2 2 1 500E9
    15. R3 8 5 75E3
    16. R4 5 9 75E3
    17. R5 9 1 75E3
    18. R6 10 11 1E3
    19. R7 13 14 1E3
    20. R8 8 12 150E3
    21. R9 4 8 500E9
    22. R10 20 19 1E3
    23. R11 16 17 1E3
    24. R12 8 18 150E3
    25. R13 8 21 150E3
    26. R14 22 23 1E3
    27. R15 8 26 150E3
    28. R16 24 25 1E3
    29. R19 7 1 500E9
    30. R20 29 26 1E6
    31. D1 1 11 DMOD
    32. D2 12 11 DMOD
    33. D3 12 14 DMOD
    34. D4 1 14 DMOD
    35. D5 18 17 DMOD
    36. D6 1 17 DMOD
    37. D7 18 19 DMOD
    38. D8 1 19 DMOD
    39. D9 21 14 DMOD
    40. D10 21 25 DMOD
    41. D11 1 23 DMOD
    42. D12 18 23 DMOD
    43. D13 26 25 DMOD
    44. D14 1 25 DMOD1
    45. D15 3 27 DMOD
    46. D16 28 3 DMOD
    47. E1 10 1 6 5 1000
    48. E2 13 1 2 9 1000
    49. E3 16 1 15 12 1000
    50. E4 22 1 15 21 1000
    51. E5 24 1 15 18 1000
    52. E7 20 1 4 30 1000
    53. M1 7 29 1 1 MOSMOD
    54. .MODEL MOSMOD NMOS (LEVEL=1 KP=1 VTO=1 RD=5)
    55. .MODEL DMOD D (RS=1E-6)
    56. .MODEL DMOD1 D (RS=1E-6 IS=1E-9)
    57. .ENDS X555
     
  9. mitza_h

    Thread Starter New Member

    Jun 24, 2009
    9
    0
    i think you were right with the component model, the signal looks different but unfortunatelly i stumbelled on another error:
    "Note: starting Gmin stepping
    Note: One successful Gmin step
    Note: One successful Gmin step
    Note: One successful Gmin step
    Note: One successful Gmin step
    Note: One successful Gmin step
    Warning: Gmin step failed
    Warning: Gmin stepping failed
    Note: starting source stepping
    Note: One successful source step
    Note: One successful source step
    Note: One successful source step
    Warning: source stepping failed
    doAnalyses: Iteration limit reached
    run simulation(s) aborted"

    I tried different steping times and durations but it's always the same error.
    and i noticed that if i don't check UIC then it doesn't even show the signal, it goes straight to the error.

    @ R!f@@ in my project i use TS555CN and because i didn't find it in circuit maker i tried to simulate with a normal 555 timer
     
  10. R!f@@

    AAC Fanatic!

    Apr 2, 2009
    8,754
    760
    sorry my bad...
     
  11. R!f@@

    AAC Fanatic!

    Apr 2, 2009
    8,754
    760
    connect a 0.01uf cap from pin 5 to ground and try
     
  12. mitza_h

    Thread Starter New Member

    Jun 24, 2009
    9
    0
    i did connect it but it had no influence, the error persists :( i think that maybe i didn't give the right values for step time and simulation duration. i tried with 10ms for simulation duration and 100uS, 200uS and 1 ms for steps but it's always the same error
     
  13. Audioguru

    New Member

    Dec 20, 2007
    9,411
    896
    The output pin 3 of a 555 switches quickly high and low, not a tiny triangle wave.
     
  14. R!f@@

    AAC Fanatic!

    Apr 2, 2009
    8,754
    760
    wait a minute, are u simulating this through multisim
     
  15. MAB

    Member

    Dec 30, 2009
    20
    1
    The OP is using Circuitmaker software package, very similar to multism.

    mitza, try checking the UIC box per SgtWookie's instructions.
    In my circuitmaker version, its found under:

    Simulation -> Analysis Setup -> Transient/Fournier
    The UIC box should be on the lower left hand corner.;)
     
  16. mitza_h

    Thread Starter New Member

    Jun 24, 2009
    9
    0
    i am simulating in circuitmaker 2000 and i have UIC checked (my checkbox is in the upper side of the window, in the middle) , but still have that error, however it shows me a signal like in the picture attached. if i leave UIC unchecked then that signal doesn't even show. the error is the same in both cases.
    i think that maybe i didn't chose the right steping times or simulation time
     
  17. R!f@@

    AAC Fanatic!

    Apr 2, 2009
    8,754
    760
    Did it occur for this circuit only. Try another to guarantee ur installation
     
  18. mitza_h

    Thread Starter New Member

    Jun 24, 2009
    9
    0
    I tried the example supplied with the program and it worked flawlessly. i also reinstalled the program.
    i will try and adapt the example circuit to what i need. will be back soon with results.
     
  19. mitza_h

    Thread Starter New Member

    Jun 24, 2009
    9
    0
    ok, i finally managed to get some good results ! :D . i modified the example schematic to do what mine does, and i saw that without the buble with .IC in it, it didn't work. i searched it and saw that it's a SPICE instrument. i don't know what it does, but without it the simulation doesn't work. if anyone knows please tell me too :) . anyhow thank's for helping me, you are a great comunity !
     
  20. MAB

    Member

    Dec 30, 2009
    20
    1
    Glad to hear that you are making progress

    The .IC stands for Initial Condition.
    In this case, It tells the software to set the 555 timer's Trig input at a logic 0 when starting its simulation.
    Chapter 6 of the users manual does a good job describing Transient Analysis setting. Worth reading.

    I did not need it on my software package, but it's a diferent version:rolleyes:
    Have you tried the UA555 (component model) yet?

    Edit:
    Here is my waveforms and setting
     
    Last edited: Apr 13, 2010
    mitza_h likes this.
Loading...