Connect with us

Spice simulation far from actual circuit behaviour

Discussion in 'Electronic Design' started by [email protected], Mar 31, 2005.

Scroll to continue with content
  1. Guest

    I am trying to use the TLV2241 DIP package IC to make a relaxation
    oscillator(square wave oscillator using positive feedback). I first
    simulated the design in spice (both ORCAD PSPICE and WINSPICE). I used
    the SPICE model of the TLV2241 provided in the data sheet provided by
    TI.COM . Please see the spice circuit file below.

    Problem: In the simulated version I get an oscillation period of approx
    6.2ms. However when I built the circuit using the chip I actually got a
    frequency of 19Hz(Period approx 52ms)
    I have made sure that all components are close to the specs as
    specified in the spice simulation
    Question) Is the model provided by TI, as shown below, adequate to
    accurately model the opamp. Please suggest why is there such a
    disparity between spice simulation(s) and the actual circuit?
    Thanks
    SPICE CIRCUIT FILE FOR SQUARE WAVE GENERATOR USING TLV2241
    ----------------------------------------------------------
    *Relaxation oscillator using a single supply opamp
    * connections: non-inverting input
    * | inverting input
    * | | positive power supply
    * | | | negative power supply
    * | | | | output
    * | | | | |
    ..SUBCKT TLV2241 1 2 3 4 5
    C1 11 12 9.8944E-12
    C2 6 7 30.000E-12
    CEE 10 99 8.8738E-12
    DC 5 53 DY
    DE 54 5 DY
    DLP 90 91 DX
    DLN 92 90 DX
    DP 4 3 DX
    EGND 99 0 POLY(2) (3,0) (4,0) 0 .5 .5
    FB 7 99 POLY(5) VB VC VE VLP VLN 0 61.404E6 -1E3 1E3 61E6 -61E6
    GA 6 0 11 12 1.0216E-6
    GCM 0 6 10 99 10.216E-12
    IEE 10 4 DC 54.540E-9
    IOFF 0 6 DC 5E-12
    HLIM 90 0 VLIM 1K
    Q1 11 2 13 QX1
    Q2 12 1 14 QX2
    R2 6 9 100.00E3
    RC1 3 11 978.81E3
    RC2 3 12 978.81E3
    RE1 13 10 30.364E3
    RE2 14 10 30.364E3
    REE 10 99 3.6670E9
    RO1 8 5 10
    RO2 7 99 10
    RP 3 4 1.4183E6
    VB 9 0 DC 0
    VC 3 53 DC .88315
    VE 54 4 DC .88315
    VLIM 7 8 DC 0
    VLP 91 0 DC 540
    VLN 0 92 DC 540
    ..MODEL DX D(IS=800.00E-18)
    ..MODEL DY D(IS=800.00E-18 RS=1M CJO=10P)
    ..MODEL QX1 NPN(IS=800.00E-18 BF=27.270E21)
    ..MODEL QX2 NPN(IS=800.0000E-18 BF=27.270E21)
    ..ENDS

    XOP1 3 1 4 0 2 TLV2241
    Cout 2 6 0.033uF
    RF 1 6 9.99K
    CF 1 0 10uF
    R2 6 3 1.001K
    R1 3 0 19.97K
    VS1 4 0 5V
    ..TRAN 0.01ms 100ms
    ..PROBE
    ..PLOT TRAN V(2)
    ..END
     
  2. Jim Thompson

    Jim Thompson Guest

    [snip]

    Why don't you post a schematic on a.b.s.e, or an LTspice .asc listing
    here, so we can visualize your circuit?

    Working from a netlist we can only see the same result as you got,
    without the ability to visualize and find mis-use of the device.

    ...Jim Thompson
     
  3. Guest

    I am posting the LTSpice.asc listing. Please excuse the poor
    drawing.Thanks
    -----------------------------------------------------------------------------------------------------

    Version 4
    SHEET 1 880 680
    WIRE -112 160 -112 48
    WIRE -112 256 -112 224
    WIRE -80 416 -80 304
    WIRE 32 160 -112 160
    WIRE 32 208 32 192
    WIRE 32 304 0 304
    WIRE 32 304 32 208
    WIRE 64 160 32 160
    WIRE 64 192 32 192
    WIRE 96 48 -112 48
    WIRE 96 112 16 112
    WIRE 96 144 96 112
    WIRE 96 240 96 208
    WIRE 96 304 32 304
    WIRE 192 176 128 176
    WIRE 256 48 176 48
    WIRE 256 96 256 48
    WIRE 256 176 256 96
    WIRE 256 304 176 304
    WIRE 256 304 256 176
    FLAG -80 416 0
    FLAG -112 256 0
    FLAG 96 240 0
    FLAG 32 160 1
    FLAG 32 208 3
    FLAG 160 192 2
    FLAG 256 96 6
    FLAG 16 128 Node4_5V
    SYMBOL Opamps\\UniversalOpamp 96 176 R0
    SYMATTR InstName TLV2241
    SYMBOL res 16 288 R90
    WINDOW 0 0 56 VBottom 0
    WINDOW 3 32 56 VTop 0
    SYMATTR InstName R1
    SYMATTR Value R1 = 19.97K
    SYMBOL res 192 288 R90
    WINDOW 0 0 56 VBottom 0
    WINDOW 3 32 56 VTop 0
    SYMATTR InstName R2
    SYMATTR Value R2 = 1.004K
    SYMBOL cap -96 224 R180
    SYMATTR InstName C1
    SYMATTR Value CF = 10µF
    SYMBOL cap 256 160 R90
    WINDOW 0 0 32 VBottom 0
    WINDOW 3 32 32 VTop 0
    SYMATTR InstName C2
    SYMATTR Value Cout = 0.033UF
    SYMBOL res 192 32 R90
    WINDOW 0 0 56 VBottom 0
    WINDOW 3 32 56 VTop 0
    SYMATTR InstName R3
    SYMATTR Value RF = 9.99K
     
  4. Jim Thompson

    Jim Thompson Guest

    Please include your simulation setups.

    ...Jim Thompson
     
  5. Jim Thompson

    Jim Thompson Guest

    [snip]

    Looks like LTspice is balking at "values" R1, R2...

    Did you actually run this in LTspice?

    ...Jim Thompson
     
  6. Guest

    THanks Jim
    No i did not run the simulation of the schematic in LTSpice , i just
    downloaded LT to make the schematic. I simulated the spice netlist(my
    first post) using ORCAD Pspice and winspice.
    I didnt choose any simulation setups, except for those mentioned in the
    spice netlist for transient time step.
    I simulated the spice netlist in LTSpice and got the same results as
    PSPICE and winspice
    thanks.
     
  7. Jim Thompson

    Jim Thompson Guest

    Please post PSpice .CIR and .NET files

    (Because a little poking around shows floating nodes in the LTspice
    schematics, misnamed values... RF=9.99K WRONG, just 9.99K CORRECT)

    ...Jim Thompson
     
  8. Guest

    Jim
    My first post already has the PSPICE .cir file. I did not make/use any
    ..net file. I simulated using a .cir file only ill post it again .
    Thanks

    ..CIR SPICE CIRCUIT FILE FOR SQUARE WAVE GENERATOR USING TLV2241
    ----------------------------------------------------------
    *Relaxation oscillator using a single supply opamp
    * connections: non-inverting input
    * | inverting input
    * | | positive power supply
    * | | | negative power supply
    * | | | | output
    * | | | | |
    ..SUBCKT TLV2241 1 2 3 4 5
    C1 11 12 9.8944E-12
    C2 6 7 30.000E-12
    CEE 10 99 8.8738E-12
    DC 5 53 DY
    DE 54 5 DY
    DLP 90 91 DX
    DLN 92 90 DX
    DP 4 3 DX
    EGND 99 0 POLY(2) (3,0) (4,0) 0 .5 .5
    FB 7 99 POLY(5) VB VC VE VLP VLN 0 61.404E6 -1E3 1E3 61E6 -61E6
    GA 6 0 11 12 1.0216E-6
    GCM 0 6 10 99 10.216E-12
    IEE 10 4 DC 54.540E-9
    IOFF 0 6 DC 5E-12
    HLIM 90 0 VLIM 1K
    Q1 11 2 13 QX1
    Q2 12 1 14 QX2
    R2 6 9 100.00E3
    RC1 3 11 978.81E3
    RC2 3 12 978.81E3
    RE1 13 10 30.364E3
    RE2 14 10 30.364E3
    REE 10 99 3.6670E9
    RO1 8 5 10
    RO2 7 99 10
    RP 3 4 1.4183E6
    VB 9 0 DC 0
    VC 3 53 DC .88315
    VE 54 4 DC .88315
    VLIM 7 8 DC 0
    VLP 91 0 DC 540
    VLN 0 92 DC 540
    ..MODEL DX D(IS=800.00E-18)
    ..MODEL DY D(IS=800.00E-18 RS=1M CJO=10P)
    ..MODEL QX1 NPN(IS=800.00E-18 BF=27.270E21)
    ..MODEL QX2 NPN(IS=800.0000E-18 BF=27.270E21)
    ..ENDS

    XOP1 3 1 4 0 2 TLV2241
    Cout 2 6 0.033uF
    RF 1 6 9.99K
    CF 1 0 10uF
    R2 6 3 1.001K
    R1 3 0 19.97K
    VS1 4 0 5V
    ..TRAN 0.01ms 100ms
    ..PROBE
    ..PLOT TRAN V(2)
    ..END
     
  9. Jim Thompson

    Jim Thompson Guest

    OK. I'll load it into PSpice sometime this afternoon... have REAL
    work simulating right now ;-)

    (Where did the TLV2241 model come from? BF=27.270E21 is a bit absurd
    :)

    ...Jim Thompson
     
  10. Fred Abse

    Fred Abse Guest

    What does "CF=10\x{00B5}F mean?

    You need to lose the "R1=" etc. from the component values, else LTspice
    barfs. just specify a resistor as, say "1.6K" or "1K6", or "1600", or
    "1.6e3"

    You need to specify a voltage source for your 5V supply. Just writing it
    on the schematic won't work.

    I took a blind guess that "10\x(00B5) meant 10^-5 Farad, ie. 1e-5F. With
    that value, I get 1.74 milliseconds low and 1.50 milliseconds high at node
    002 (pin 2)

    Guess what? I was right. I just took a look at your netlist, and CF is
    10uF = 10e-6 = 1e-5.
     
  11. Guest

  12. Steve,
    OK, I corrected a few circuit errors. Now it runs as a
    relaxation osciallator.

    --Mike

    Version 4
    SHEET 1 880 680
    WIRE -304 144 -304 112
    WIRE -304 256 -304 224
    WIRE -192 112 -304 112
    WIRE -192 304 -192 112
    WIRE -160 304 -192 304
    WIRE -96 400 -96 368
    WIRE -64 368 -96 368
    WIRE -32 160 -32 48
    WIRE -32 176 -32 160
    WIRE -32 256 -32 240
    WIRE 32 304 -80 304
    WIRE 32 304 32 192
    WIRE 32 368 16 368
    WIRE 32 368 32 304
    WIRE 64 160 -32 160
    WIRE 64 192 32 192
    WIRE 96 48 -32 48
    WIRE 96 112 -192 112
    WIRE 96 144 96 112
    WIRE 96 240 96 208
    WIRE 96 304 32 304
    WIRE 256 48 176 48
    WIRE 256 176 128 176
    WIRE 256 176 256 48
    WIRE 256 304 176 304
    WIRE 256 304 256 176
    FLAG -96 400 0
    FLAG -32 256 0
    FLAG 96 240 0
    FLAG -304 256 0
    SYMBOL Opamps\\UniversalOpamp 96 176 R0
    SYMATTR InstName TLV2241
    SYMBOL res 32 352 R90
    WINDOW 0 0 56 VBottom 0
    WINDOW 3 32 56 VTop 0
    SYMATTR InstName R1
    SYMATTR Value 10K
    SYMBOL res 192 288 R90
    WINDOW 0 0 56 VBottom 0
    WINDOW 3 32 56 VTop 0
    SYMATTR InstName R2
    SYMATTR Value 100K
    SYMBOL cap -48 240 M180
    SYMATTR InstName C1
    SYMATTR Value 10µ
    SYMBOL res 192 32 R90
    WINDOW 0 0 56 VBottom 0
    WINDOW 3 32 56 VTop 0
    SYMATTR InstName R3
    SYMATTR Value 10K
    SYMBOL voltage -304 128 R0
    SYMATTR InstName V1
    SYMATTR Value 5
    SYMBOL res -64 288 R90
    WINDOW 0 0 56 VBottom 0
    WINDOW 3 32 56 VTop 0
    SYMATTR InstName R4
    SYMATTR Value 10K
    TEXT 88 376 Left 0 !.tran 1 startup
     
  13. Guest

    mike i already mentioned in my first post that the circuit runs as an
    oscillator. My problem is that the spice simulation of the .cir spice
    netlist(first post) and the 'actual' circuit on breadboard do not run
    at the same frequency. I only made the LT .asc schematic so that
    readers could visualize the circuit.
     
  14. Jim Thompson

    Jim Thompson Guest

    [snip]

    Most likely it's that the model doesn't properly reflect the true
    device operation when the inputs go below ground...

    The OpAmp +IN has +/- 400mV of signal on it.

    Redesign to have the inputs near supply mid-point and then it'll
    become predictable.

    ...Jim Thompson
     
  15. Steve,
    Sorry. The schematic I saw didn't run. Once you get the simulation
    issues cleared up, since you have hardware, scope out the real circuit
    and find what the difference is between the model and device at the
    inputs and outputs. Don't trust your average opamp macromodel
    over the full input and output ranges.

    --Mike
     
  16. Jim Thompson

    Jim Thompson Guest

    His circuit swings below ground on both inputs.

    ...Jim Thompson
     
  17. Jim Thompson

    Jim Thompson Guest

    [snip]

    See...

    Newsgroups: alt.binaries.schematics.electronic
    Subject: Re: Spice simulation far from actual circuit behaviour
    (S.E.D) - RelaxationFromSED-Fixed.pdf
    Message-ID: <>

    ...Jim Thompson
     
  18. Fred Bloggs

    Fred Bloggs Guest

    You were told 12 hours earlier on SEB how to fix your sloppy circuit
    which had a capacitor between the op amp output and both feedback
    circuits. If you want to ask a question about electronics that is one
    thing, but when you really want someone to troubleshoot your slipshod
    mistakes then that's another.
     
  19. Guest

    Thanks much Jim. Am i Correct in understanding that the 10K resistor
    from Vcc to INP is to set up a dc offset of 2.5V in the Voutput?
    thanks again. I am currently trying to learn different opamp circuits
    by simulation and then breadboarding them. I get stuck sometimes :)
     
  20. Jim Thompson

    Jim Thompson Guest

    It biases the input (along with the feedback R) such that, when output
    is at 0V, input is at +1V, when output is at +5V, input is at +4V.
    This keeps the OpAmp within its guaranteed operating range.
    Note that the chosen OpAmp is rather gutless, and SLOW... the output
    does not "snap" as I like to see in precision oscillators.

    ...Jim Thompson
     
Ask a Question
Want to reply to this thread or ask your own question?
You'll need to choose a username for the site, which only take a couple of moments (here). After that, you can post your question and our members will help you out.
Electronics Point Logo
Continue to site
Quote of the day

-