OPA349 spice model acting weird

[Tom (at tomsweb.net)]

Everyone,

I am trying to simulate a circuit (using LTSpice) with a OPA349 from
Burr-Brown: 1 microamp Iq, 70kHz GBW, CMOS rail-rail I/O, 1.8V-5.5
opamp. According to the datasheet
(http://focus.ti.com/lit/ds/symlink/opa349.pdf) this one can drive 8mA
without problems.

The OPA349 appears to misbehave in my circuit simulations, so I created
a simple test circuit consisting of a simple unity gain inverter with 1
Meg input, feedback and load resistors.

With a 1 MEG load the opamp seems to go out of closed-loop at Vin<0.8V
with a 2.2V single supply, whereas the output is supposed to swing to
350mV from the rails with a 10K load, and the input CM range extends
200mV past either rail. If I load the opamp with 10 MEG or more it
seems to work. At 100K load or less the simulations become total crap.
Changing the feedback resistors to higher or lower values does not
improve things either.

Is this a bug in the model? Or am I missing something? I don't have a
physical chip to test it on right now, but since the opamp can drive
8mA (and is specced for a rail-to-rail output at 10K load) I really
don't think this is how the real hardware should behave!

Substituting a different opamp model (e.g. OPA336) works as expected.
Any suggestions? Below spice netlist, opamp model, LTSpice schematic
and LTSpice symbol for OPA349...

Spice netlist:
* d:\tom\spice\opa349test.asc
XU1 V+ V- VDD 0 VO opa349 opa349
R1 V- Vi 1MEG
R2 VO V- 1MEG
RL VO 0 1MEG
V1 V+ 0 1.2V
V2 Vi 0 PULSE(0 2.2 0 500ms 500ms 0ms 1s)
V3 VDD 0 2.2V
..tran 1s
..include opa349.mod
..backanno
..end

OPA349 model (from
http://focus.ti.com/docs/prod/folders/print/opa349.html)
*
* OPA349 operational amplifier "macromodel" subcircuit
* REV A created using Parts release 8.0 on 11/23/99 at 17:01 by Vadim
Ivanov
* REV B Revised 25 August 2000 by Vadim Ivanov
* Parts is a MicroSim product.
*
* connections: non-inverting input
* | inverting input
* | | positive power supply
* | | | negative power supply
* | | | | output
* | | | | |
..subckt OPA349 + - V+ V- OUT
*
*

* INPUT STAGE

*

iin V+ 5 200n

m7 550 vswitch 5 5 pix l=.6u w=20u m=2

m8 550 550 V- V- nix l=4u w=4u m=1

m9 553a 550 V- V- nix l=4u w=4u m=1

m9c 66 nvsat 553a V- nix l=.6u w=4u m=1

Vpvsat V+ vswitch DC 1.3

Vnvsat nvsat V- DC 1.37

iin1 + 98 .2p

iin2 - 98 .2p

d3 5 V+ dx

d4 V- 66 dx

d5 - V+ dx

d6 + V+ dx

d7 V- - dx

d8 V- + dx

m1 33 - 66 V- nix l=5u w=5u m=1

m2 4 + 66 V- nix l=5u w=5u m=1

m3 8 - 5 5 pix l=5u w=5u m=1

m4 9 + 5 5 pix l=5u w=5u m=1

r1 V+ 33 .1meg

r2 V+ 4 .1meg

r3 8 V- .1meg

r4 9 V- .1meg


*

* GAIN STAGE

*

eref 98 V- poly(2) V+ V- V- V- 0 0.5 0.5

g1 98 21 poly(2) 4 33 9 8 0 2.3u 2.3u

rg 21 98 2e10

cc 21 OUT 2p

d1 21 22 dx

d2 23 21 dx

v1 V+ 22 1.37

v2 23 V- 1.37

*

* COMMON MODE GAIN STAGE

*

*ecm 24 98 poly(2) + 98 - 98 0 0.5 0.5

*r5 24 25 1e6

*r6 25 98 10k

*c1 24 25 0.75p

*

* OUTPUT STAGE

*

* isy V+ V- 450.4u

* gsy V+ V- poly(1) V+ V- -3.334e-4 6.667e-5

ep V+ 39 poly(1) 98 21 0.7515 .01

en 38 V- poly(1) 21 98 0.7515 .01

vh OUT 6h DC 1e-2

vl 6l OUT DC 1e-2

m113 6h 39 V+ V+ pox l=.6u w=1500u

m114 6l 38 V- V- nox l=.6u w=1500u

c15 OUT 39 3p

c16 OUT 38 3p

..model dx d(rs=1 cjo=0.1p)

..model nix nmos(vto=0.75 kp=205.5u rd=1 rs=1 rg=1 rb=1 cgso=4e-9

+cgdo=4e-9 cgbo=16.667e-9 cbs=2.34e-13 cbd=2.34e-13)

..model nox nmos(vto=0.75 kp=195u rd=.5 rs=.5 rg=1 rb=1 cgso=66.667e-12

+cgdo=66.667e-12 cgbo=125e-9 cbs=2.34e-13 cbd=2.34e-13)

..model pix pmos(vto=-0.75 kp=205.5u rd=1 rs=1 rg=1 rb=1 cgso=4e-9

+cgdo=4e-9 cgbo=16.667e-9 cbs=2.34e-13 cbd=2.34e-13)

..model pox pmos(vto=-0.75 kp=195u rd=.5 rs=.5 rg=1 rb=1 cgso=66.667e-12

+cgdo=66.667e-12 cgbo=125e-9 cbs=2.34e-13 cbd=2.34e-13)

..ENDS OPA349
*
*

LTSpice schematic:
Version 4
SHEET 1 880 680
WIRE -240 256 -240 208
WIRE -160 208 -240 208
WIRE -112 208 -160 208
WIRE -64 288 -64 240
WIRE -64 304 -64 288
WIRE 0 208 -32 208
WIRE 0 208 0 128
WIRE 16 208 0 208
WIRE 16 240 -64 240
WIRE 32 128 0 128
WIRE 48 288 48 256
WIRE 144 128 112 128
WIRE 144 176 144 128
WIRE 144 224 80 224
WIRE 144 224 144 176
WIRE 192 176 144 176
WIRE 192 208 192 176
WIRE 192 304 192 288
FLAG 48 288 0
FLAG 48 192 VDD
FLAG 144 176 VO
FLAG 192 304 0
FLAG -160 208 Vi
FLAG -64 288 V+
FLAG 0 208 V-
FLAG 272 48 VDD
FLAG 272 128 0
FLAG -64 384 0
FLAG -240 336 0
SYMBOL opa349 48 160 R0
SYMATTR InstName U1
SYMBOL res -16 192 R90
WINDOW 0 -3 94 VBottom 0
WINDOW 3 -27 39 VTop 0
SYMATTR InstName R1
SYMATTR Value 10MEG
SYMBOL res 128 112 R90
WINDOW 0 -4 87 VBottom 0
WINDOW 3 -31 30 VTop 0
SYMATTR InstName R2
SYMATTR Value 5MEG
SYMBOL res 176 192 R0
SYMATTR InstName RL
SYMATTR Value 100K
SYMBOL voltage -64 288 R0
SYMATTR InstName V1
SYMATTR Value 1.2V
SYMBOL voltage -240 240 R0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
WINDOW 0 -76 25 Left 0
WINDOW 3 -477 74 Left 0
SYMATTR InstName V2
SYMATTR Value PULSE(0 2.2 0 500ms 500ms 0ms 1s)
SYMBOL voltage 272 32 R0
SYMATTR InstName V3
SYMATTR Value 2.2V
TEXT -282 490 Left 0 !.tran 1s
TEXT -280 464 Left 0 !.include opa349.mod

OPA349 LTSpice symbol:
Version 4
SymbolType CELL
LINE Normal -32 32 32 64
LINE Normal -32 96 32 64
LINE Normal -32 32 -32 96
LINE Normal -28 48 -20 48
LINE Normal -28 80 -20 80
LINE Normal -24 84 -24 76
LINE Normal 0 32 0 48
LINE Normal 0 96 0 80
LINE Normal 4 44 12 44
LINE Normal 8 40 8 48
LINE Normal 4 84 12 84
WINDOW 0 16 32 Left 0
WINDOW 3 16 96 Left 0
SYMATTR Value opa349
SYMATTR Prefix X
SYMATTR SpiceModel opa349
SYMATTR Description Precision Operational Amplifier
PIN -32 80 NONE 0
PINATTR PinName In+
PINATTR SpiceOrder 1
PIN -32 48 NONE 0
PINATTR PinName In-
PINATTR SpiceOrder 2
PIN 0 32 NONE 0
PINATTR PinName V+
PINATTR SpiceOrder 3
PIN 0 96 NONE 0
PINATTR PinName V-
PINATTR SpiceOrder 4
PIN 32 64 NONE 0
PINATTR PinName OUT
PINATTR SpiceOrder 5

 

[Helmut Sennewald]

Everyone,

I am trying to simulate a circuit (using LTSpice) with a OPA349 from
Burr-Brown: 1 microamp Iq, 70kHz GBW, CMOS rail-rail I/O, 1.8V-5.5
opamp. According to the datasheet
(http://focus.ti.com/lit/ds/symlink/opa349.pdf) this one can drive 8mA
without problems.

The OPA349 appears to misbehave in my circuit simulations, so I created
a simple test circuit consisting of a simple unity gain inverter with 1
Meg input, feedback and load resistors.

With a 1 MEG load the opamp seems to go out of closed-loop at Vin<0.8V
with a 2.2V single supply, whereas the output is supposed to swing to
350mV from the rails with a 10K load, and the input CM range extends
200mV past either rail. If I load the opamp with 10 MEG or more it
seems to work. At 100K load or less the simulations become total crap.
Changing the feedback resistors to higher or lower values does not
improve things either.

Is this a bug in the model? Or am I missing something? I don't have a
physical chip to test it on right now, but since the opamp can drive
8mA (and is specced for a rail-to-rail output at 10K load) I really
don't think this is how the real hardware should behave!

Hello Tom,
I tried the model with LTspice and see the same problem as you
have described. I recommend you write a letter to AD.

Best regards,
Helmut

 

[Helmut Sennewald]

,,,,

Hello Tom,
I tried the model with LTspice and see the same problem as you
have described. I recommend you write a letter to AD.

Sorry, it's TI and not AD,
Helmut

 

[Tom (at tomsweb.net)]

I tried the model with LTspice and see the same problem as you

Sorry, it's TI and not AD,

TI just confirmed that their model is crap (actually I would prefer
them not offering a model at all in that case!).

--snip--
You were requesting the information about OPA349 Spice macro model. Our
OPA349 macromodel is not a very good one. It was written 5 years ago
and I've found that it does have some problems (Especially Low Voltage
problems,less than 3Volts) .Sorry for the inconvenience caused.

You might want to consider using the TLV2401 device and the
specifications are almost similar to OPA349. The TLV2401 device has a
Spice model and it can be downloaded from TI website
(http://focus.ti.com/docs/prod/folders/print/tlv2401.html#productmodels
).
--snip--

I'm now simulating with the TLV2401 model, which works. However, the
real circuit will use a OPA349, because my supply is less than 2.5V
(the minimum for TLV2401).

greetings,
Tom

 

[Helmut Sennewald]

TI just confirmed that their model is crap (actually I would prefer
them not offering a model at all in that case!).

--snip--
You were requesting the information about OPA349 Spice macro model. Our
OPA349 macromodel is not a very good one. It was written 5 years ago
and I've found that it does have some problems (Especially Low Voltage
problems,less than 3Volts) .Sorry for the inconvenience caused.

You might want to consider using the TLV2401 device and the
specifications are almost similar to OPA349. The TLV2401 device has a
Spice model and it can be downloaded from TI website
(http://focus.ti.com/docs/prod/folders/print/tlv2401.html#productmodels
).
--snip--

I'm now simulating with the TLV2401 model, which works. However, the
real circuit will use a OPA349, because my supply is less than 2.5V
(the minimum for TLV2401).

greetings,
Tom

Hello Tom,

thanks for this information. I will keep this message in my folder.

It sounds like TI will not spend any money/time to correct
this model. What a bad service to their customers when I assume
that they eventually know since 5 years that the model is wrong.

Best regards,
Helmut

 

[Jim Thompson]

Hello Tom,

thanks for this information. I will keep this message in my folder.

It sounds like TI will not spend any money/time to correct
this model. What a bad service to their customers when I assume
that they eventually know since 5 years that the model is wrong.

Best regards,
Helmut

They (and others are not willing to spend the money it takes to
derive a good model.

But that provokes a question to you... Would you PAY for a good
model?

...Jim Thompson

 

[Helmut Sennewald]

They (and others are not willing to spend the money it takes to
derive a good model.

But that provokes a question to you... Would you PAY for a good
model?

...Jim Thompson

Hello Jim,

I expect for standard parts that the manufacturer provides
the model. If not then I would firstly try to make my own
model before I spend money for unknown quality.

Best regards,
Helmut

 

[Jim Thompson]

Hello Jim,

I expect for standard parts that the manufacturer provides
the model. If not then I would firstly try to make my own
model before I spend money for unknown quality.

Best regards,
Helmut

I was inquiring to see if it were worthwhile to add model creation to
my repertoire... they would not be of "unknown quality" ;-)

But I doubt anyone would pay.

I have had occasional RFQ's from AD, but they always go with the low
bidder ;-)

...Jim Thompson

 

[Winfield Hill]

Jim Thompson wrote...

But that provokes a question to you... Would you PAY for a good
model?

I would (and have, with lots of lost time making and vetting my
own, that is). But before laying out my cash I'd want to see
some documentation that it was good enough for my needs - sort
of a spice- model datasheet with specs and plots.

I wouldn't want to pay thousdands of dollars.