Spice simulation far from actual circuit behaviour

[[email protected]]

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

 

[Jim Thompson]

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
----------------------------------------------------------

[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

 

[[email protected]]

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

 

[Jim Thompson]

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

Version 4
SHEET 1 880 680 [snip]
SYMATTR InstName R3
SYMATTR Value RF = 9.99K

Please include your simulation setups.

...Jim Thompson

 

[Jim Thompson]

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

[snip]

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

Did you actually run this in LTspice?

...Jim Thompson

 

[[email protected]]

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.

 

[Jim Thompson]

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.

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

 

[[email protected]]

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

 

[Jim Thompson]

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

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

 

[Fred Abse]

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

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.

 

[[email protected]]

Thanks Jim, Will wait for ure advice. The TLV2241 spice model was
printed inside the datasheet (Page 16) of the device available at:
http://focus.ti.com/lit/ds/symlink/tlv2241.pdf

 

[Mike Engelhardt]

Steve,

I am posting the LTSpice.asc listing.

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

 

[[email protected]]

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.

 

[Jim Thompson]

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

[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

 

[Mike Engelhardt]

Steve,

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.

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

 

[Jim Thompson]

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

His circuit swings below ground on both inputs.

...Jim Thompson

 

[Jim Thompson]

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

[snip]

See...

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

...Jim Thompson

 

[Fred Bloggs]

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.

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.

 

[[email protected]]

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

 

[Jim Thompson]

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?

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.

thanks again. I am currently trying to learn different opamp circuits
by simulation and then breadboarding them. I get stuck sometimes

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