--- 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
