Any idea about Spice funny?

P

Paul Burke

Guest
I've been getting some funnies with LTSpice (freshly downloaded version)
which seem to centre round this trivial circuit: just a differential
amplifier with a gain of 33 (if it looks a bit odd, it's because it's
extracted from the original circuit). I'd rather naively expect the
output to be a 3.33V 1kHz sinewave with a 7.5V offset. Instead of which
I get an initial spike of -27kV, which ramps at about 1.6V/us. Which
doesn't look right to me. It also takes an age to simulate, so much so
that I haven't had the patience to get to the running bit yet.

If I try to do an AC analysis I just get iteration limit. Again, the
circuit is pretty simple, I'd expect it to do this one, so i must be
doing something silly.

I hardly use Spice, but I'm sure it should be easier than this. Anyone
have any idea what egregious blunder I'm making? Any kind help for a
mostly digital bloke much appreciated.

Here's the source:

Version 4
SHEET 1 880 680
WIRE 608 0 304 0
WIRE 304 80 304 0
WIRE 448 80 384 80
WIRE 96 144 -160 144
WIRE 176 224 0 224
WIRE 384 224 384 160
WIRE 384 224 256 224
WIRE 608 272 608 0
WIRE -160 288 -160 144
WIRE 96 288 96 144
WIRE 384 304 384 224
WIRE 384 304 128 304
WIRE 0 320 0 224
WIRE 64 320 0 320
WIRE 304 336 304 160
WIRE 304 336 128 336
WIRE 304 352 304 336
WIRE 304 448 304 432
WIRE -160 544 -160 368
WIRE 96 544 96 352
WIRE 96 544 -160 544
WIRE 304 544 304 528
WIRE 304 544 96 544
WIRE 448 544 448 80
WIRE 448 544 304 544
WIRE 608 544 608 352
WIRE 608 544 448 544
FLAG 0 224 VIFB
SYMBOL Opamps\\opamp2 96 256 M0
SYMATTR InstName U1
SYMATTR Value TLC081
SYMBOL res 288 64 R0
SYMATTR InstName R1
SYMATTR Value 10k
SYMBOL res 288 336 R0
SYMATTR InstName R2
SYMATTR Value 333k
SYMBOL res 272 208 R90
WINDOW 0 0 56 VBottom 0
WINDOW 3 32 56 VTop 0
SYMATTR InstName R3
SYMATTR Value 333k
SYMBOL res 368 64 R0
SYMATTR InstName R4
SYMATTR Value 10k
SYMBOL voltage -160 272 R0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V1
SYMATTR Value 15
SYMBOL voltage 608 256 R0
WINDOW 3 24 160 Left 0
WINDOW 123 24 132 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V2
SYMATTR Value SINE(0 .1 1000)
SYMATTR Value2 AC .1
SYMBOL voltage 304 432 R0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V3
SYMATTR Value 7.5
TEXT -144 64 Left 0 !.tran 1
TEXT -152 8 Left 0 !.inc TLC081.mod

Here's the TLC081 (TLC081.mod):

* TL081 OPERATIONAL AMPLIFIER "MACROMODEL" SUBCIRCUIT
* CREATED USING PARTS RELEASE 4.01 ON 06/16/89 AT 13:08
* (REV N/A) SUPPLY VOLTAGE: +/-15V
* CONNECTIONS: NON-INVERTING INPUT
* | INVERTING INPUT
* | | POSITIVE POWER SUPPLY
* | | | NEGATIVE POWER SUPPLY
* | | | | OUTPUT
* | | | | |
..SUBCKT TL081 1 2 3 4 5
*
C1 11 12 3.498E-12
C2 6 7 15.00E-12
DC 5 53 DX
DE 54 5 DX
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 4.715E6 -5E6 5E6 5E6 -5E6
GA 6 0 11 12 282.8E-6
GCM 0 6 10 99 8.942E-9
ISS 3 10 DC 195.0E-6
HLIM 90 0 VLIM 1K
J1 11 2 10 JX
J2 12 1 10 JX
R2 6 9 100.0E3
RD1 4 11 3.536E3
RD2 4 12 3.536E3
RO1 8 5 150
RO2 7 99 150
RP 3 4 2.143E3
RSS 10 99 1.026E6
VB 9 0 DC 0
VC 3 53 DC 2.200
VE 54 4 DC 2.200
VLIM 7 8 DC 0
VLP 91 0 DC 25
VLN 0 92 DC 25
..MODEL DX D(IS=800.0E-18)
..MODEL JX PJF(IS=15.00E-12 BETA=270.1E-6 VTO=-1)
..ENDS

 
On Thu, 30 Nov 2006 10:15:37 +0000, Paul Burke <paul@scazon.com>
wrote:

I've been getting some funnies with LTSpice (freshly downloaded version)
which seem to centre round this trivial circuit: just a differential
amplifier with a gain of 33 (if it looks a bit odd, it's because it's
extracted from the original circuit). I'd rather naively expect the
output to be a 3.33V 1kHz sinewave with a 7.5V offset. Instead of which
I get an initial spike of -27kV, which ramps at about 1.6V/us. Which
doesn't look right to me. It also takes an age to simulate, so much so
that I haven't had the patience to get to the running bit yet.

If I try to do an AC analysis I just get iteration limit. Again, the
circuit is pretty simple, I'd expect it to do this one, so i must be
doing something silly.

I hardly use Spice, but I'm sure it should be easier than this. Anyone
have any idea what egregious blunder I'm making? Any kind help for a
mostly digital bloke much appreciated.

[snip]
Click to expand...

I didn't run it, but there's no GROUND (Node 0) in the schematic, so
that's likely your problem.

...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
 
Helmut Sennewald wrote:
"Jim Thompson" <To-Email-Use-The-Envelope-Icon@My-Web-Site.com> schrieb im
Newsbeitrag news:vsdum2l0i1b93qm99drjrhdnh6tnbg1pcc@4ax.com...
On Thu, 30 Nov 2006 10:15:37 +0000, Paul Burke <paul@scazon.com
wrote:

I've been getting some funnies with LTSpice (freshly downloaded version)
which seem to centre round this trivial circuit: just a differential
amplifier with a gain of 33 (if it looks a bit odd, it's because it's
extracted from the original circuit). I'd rather naively expect the
output to be a 3.33V 1kHz sinewave with a 7.5V offset. Instead of which
I get an initial spike of -27kV, which ramps at about 1.6V/us. Which
doesn't look right to me. It also takes an age to simulate, so much so
that I haven't had the patience to get to the running bit yet.

If I try to do an AC analysis I just get iteration limit. Again, the
circuit is pretty simple, I'd expect it to do this one, so i must be
doing something silly.

I hardly use Spice, but I'm sure it should be easier than this. Anyone
have any idea what egregious blunder I'm making? Any kind help for a
mostly digital bloke much appreciated.

[snip]

I didn't run it, but there's no GROUND (Node 0) in the schematic, so
that's likely your problem.

...Jim Thompson


Hello Paul,

This missing ground is indeed the reason for the convergence problem.

The next mistake is using the TL081 so very close(100mV) to the
negative supply rail. This will lead to a lot of distortion i the simulation
and in a real circuit too. Just add a negative supply voltage and the
distortion will disappear.

Why do you provide a TL081 model while using a TLC081 in the schematic?

Best regards,
Helmut


PS: If you want do a THD calculation, use the following setting.

.tran 0 0.01 0 10u
.options plotwinsize=0
.four 1k V(VIFB)

The .four result can be viewed with the following menu-comamnd.

View -> SPICE Errorlog
Click to expand...
 
Jim Thompson wrote:

I didn't run it, but there's no GROUND (Node 0) in the schematic, so
that's likely your problem.
Click to expand...

That is the problem, thanks. There was one on the circuit I abstracted
in from, and it didn't copy, and I didn't notice.

Paul Burke
 
Helmut Sennewald wrote:

This missing ground is indeed the reason for the convergence problem.

The next mistake is using the TL081 so very close(100mV) to the
negative supply rail. This will lead to a lot of distortion i the simulation
and in a real circuit too. Just add a negative supply voltage and the
distortion will disappear.

Why do you provide a TL081 model while using a TLC081 in the schematic?
Click to expand...
I kept changing the opamp trying to get it to work, and the problem with
the original circuit was operation too close to the power rails. Next,
to find an opamp that will take 15V supply (plus a reasonable margin)
AND do rail to rail IO, or change the circuit to work around a midpoint
reference.

I must practise this analog stuff more.

Paul Burke
 
"Jim Thompson" <To-Email-Use-The-Envelope-Icon@My-Web-Site.com> schrieb im
Newsbeitrag news:vsdum2l0i1b93qm99drjrhdnh6tnbg1pcc@4ax.com...
On Thu, 30 Nov 2006 10:15:37 +0000, Paul Burke <paul@scazon.com
wrote:

I've been getting some funnies with LTSpice (freshly downloaded version)
which seem to centre round this trivial circuit: just a differential
amplifier with a gain of 33 (if it looks a bit odd, it's because it's
extracted from the original circuit). I'd rather naively expect the
output to be a 3.33V 1kHz sinewave with a 7.5V offset. Instead of which
I get an initial spike of -27kV, which ramps at about 1.6V/us. Which
doesn't look right to me. It also takes an age to simulate, so much so
that I haven't had the patience to get to the running bit yet.

If I try to do an AC analysis I just get iteration limit. Again, the
circuit is pretty simple, I'd expect it to do this one, so i must be
doing something silly.

I hardly use Spice, but I'm sure it should be easier than this. Anyone
have any idea what egregious blunder I'm making? Any kind help for a
mostly digital bloke much appreciated.

[snip]

I didn't run it, but there's no GROUND (Node 0) in the schematic, so
that's likely your problem.

...Jim Thompson
Click to expand...

Hello Paul,

This missing ground is indeed the reason for the convergence problem.

The next mistake is using the TL081 so very close(100mV) to the
negative supply rail. This will lead to a lot of distortion i the simulation
and in a real circuit too. Just add a negative supply voltage and the
distortion will disappear.

Why do you provide a TL081 model while using a TLC081 in the schematic?

Best regards,
Helmut


PS: If you want do a THD calculation, use the following setting.

..tran 0 0.01 0 10u
..options plotwinsize=0
..four 1k V(VIFB)

The .four result can be viewed with the following menu-comamnd.

View -> SPICE Errorlog
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top