--- In LTspice@..., "john_oztek" <joconnor@o...> wrote:
--- In LTspice@..., "Helmut Sennewald"
<helmutsennewald@y...> wrote:
--- In LTspice@..., "john_oztek" <joconnor@o...>
wrote:
Are there any special considerations with using P-spice op-amp
macro
models with LTspice? I'm trying to simulate a circuit that
uses
a
Burr Brown/TI electrometer op-amp (OPA128 or OPA129) and I'm
getting
incorrect results. I downloaded the models from TI's
website.
The
circuit's been built and thoroughly debugged, so I'm confident
in
the
design.
When I couldn't get the circuit to operate correctly, I entered
a
simple test circuit to verify some of the basic op-amp
characteristics. I found that the input bias current was way
to
high
(about 12nA instead of 100fA), and the gain-bandwidth of the
OPA129
was high by about a factor of 10. I suspect that the models
are
just
screwed up, but since I'm new to LTspice I'm not completely
confident
with my conclusion. Any help would be greatly appreciated.
Hello John,
I tried to verify your results and the bias currents are indeed a
lot
higher than expected. I looked around in the LTSPICE settings for
possible leakage currents and other precision important
parameters.
Finally I have found that we need the command line
.OPTIONS gmin=0 (or at least <1e-18)
It defines the minimum conductance added to every node.
The simulated input bias current is then 40pA for the OPA128 and
OPA129.
The AC-gain results are really by a factor of ten too high for
the
OPA129/OPA129E.
I still don't know why the enhanced models OPA128E and OPA129E
still
shows bias currents of about 30pA instead of 40fA.
I tried the OPA129E with the PSPICE 8.0 demo.
Surprise, surprise! Even with the OPA129E, the bias current has
been
40fA. Something seems to go wrong in LTSPICE with this enhanced
model
in the .OP calculation.
The .AC simulation shows exactly the same results in PSPICE as in
LTSPICE.
Best Regards
Helmut
Helmut,
Thanks for looking into this and going to the trouble of
duplicating
my results. I've also had problems with the enhanced model for the
INA128 instrumentation amplifier. The standard model seems to work
OK although it does have a little trouble converging. One thing
for
sure, it's definitely worth the effort of proving the model in a
simple circuit against data sheet specs, particularly when second
order effects are critical.
Hello John,
I have to take back my statement that LTSPICE was wrong with the
OPA129E input bias current. I further investigated the enhanced(E)
model and it is obvious that it isn't modelled correctly for bias
current. Now it seems the PSPICE simulation has been wrong with the
OPA129E.
These are the two critical lines of the enhanced model.
g11 2 4 poly(4) (10,2) (11,2) (4,2) (66,0) 0 1E-12 1E-12 1E-12
100E-9
g21 1 4 poly(4) (10,1) (12,1) (4,1) (68,0) 0 1E-12 1E-12 1E-12
100E-9
Node 1 and 2 are the input pins. g11 and g21 should simulate input
currents proportional to the negative supply voltage(4), the common
source point(10) the drain(11 close to V-) and node 66 which is close
to (0). Assuming 15V for the negative supply gives bias currents of
15V*1e-12 = 15pA.
Finally I am wondering how PSPICE can calculate 40fA bias current.
Best Regards
Helmut
