[EE] LTSPICE tinkering

[Neil]

I recently installed LTSpice again after quite some time and having a
concern with a simple buffered voltage divider. I tried the same thing
using Multisim and getting different (but expected) results.
But perhaps there's something I don't understand that makes LTSpice more
correct?

See these 2 images... the voltage at Vdiv is correct if the op-amp is
not connected but as soon as I connect the op-amp, Vdiv goes 32%
*HIGHER* than expected. If anything, I would've expected it to come
down a tad. What am I missing here?

https://bit.ly/2zrqzWN

https://bit.ly/2zpcBV3

Cheers,
-Neil.

[Jason White]

I'd suggest using the ideal opamp model instead of the LT6013.

Use the symbol "[opamps]/opamp" and then add the Spice directive ".lib
opamp.sub" to your simulation.

You can adjust the parameters (GBWP , Input impedance, etc.) of the
ideal model to get arbitrary levels of "correctness" from it.

-Jason White

Post by Neil
I recently installed LTSpice again after quite some time and having a
concern with a simple buffered voltage divider. I tried the same thing
using Multisim and getting different (but expected) results.
But perhaps there's something I don't understand that makes LTSpice more
correct?
See these 2 images... the voltage at Vdiv is correct if the op-amp is
not connected but as soon as I connect the op-amp, Vdiv goes 32%
*HIGHER* than expected. If anything, I would've expected it to come
down a tad. What am I missing here?
https://bit.ly/2zrqzWN
https://bit.ly/2zpcBV3
Cheers,
-Neil.
--
http://www.piclist.com/techref/piclist PIC/SX FAQ & list archive
View/change your membership options at
http://mailman.mit.edu/mailman/listinfo/piclist

[RussellMc]

At a glance only, what happens if you reduce the divider resistors values
to say 10k and 1k?
Very much depending on the opamp spec, input bias currents can have an
affect. Input offset is unlikely to be that large.



Russell

[Sean Breheny]

The LT6013 datasheet states that it is only guaranteed to be stable for
gain of 5 or more. Since you are using the .op directive to simulate only
the operating point, it may be unable to determine it accurately if the
op-amp is unstable. Try a transient sim and see if the op-amp is
oscillating.

Another point is that this op-amp can only swing down to within 40mV of the
negative rail. You aren't very far away from that at 100mV. I suspect that
this is not the cause of your problem but I wanted to give a heads up.

For LTSpice, I usually keep notes on some general purpose op-amps to use in
simulations. Unfortunately I don't have my notes handy but you could
consult LT's web site for some gp op amps

The ideal op-amp model should work but it can also lead you to think a
circuit will work when in reality it won't

Sean

Post by RussellMc
At a glance only, what happens if you reduce the divider resistors values
to say 10k and 1k?
Very much depending on the opamp spec, input bias currents can have an
affect. Input offset is unlikely to be that large.
Russell
--
http://www.piclist.com/techref/piclist PIC/SX FAQ & list archive
View/change your membership options at
http://mailman.mit.edu/mailman/listinfo/piclist

[RussellMc]

Post by Sean Breheny
The LT6013 datasheet states that it is only guaranteed to be stable for
gain of 5 or more. Since you are using ...

- Read the data sheet in all areas which may be relevant to the observed
effects.

- Read the data sheet in all areas which may NOT be relevant to the
observed effects.

- An oscilloscope (and a camera) should be surgically attached to your
right arm. (Or to your SPICE virtual right arm where relevant).

- Try a "perfect" component.

- In SPICE et al, de-perfectise perfect components which have imaginary
components. (eg add a small series resistance to "perfect" inductors, ...
).

- Have a virtual (or real) talk with Murphy. "How would you mess this up IF
you wanted to ...?" (he always does.)

- If software is involved, consult Grace Hopper.

- Have ............ ?

R

[Sean Breheny]

I finally replicated this circuit in LTSpice and using the same initial
circuit as Neil, I got exactly the same operating point prediction which he
got.

I then did a transient sim as I had suggested and it matched the operating
point sim - there was no instability.

I noticed, though, that the inverting input was drawing around 30nA which
is about 300x the datasheet value for input bias current. This usually
indicates that we are violating the input voltage range. Lo and behold, the
datasheet indicates that the inputs must not go closer than about 0.75 V of
the negative supply or the op-amp gain will drop to zero. So, actually, it
looks pretty certain that the direct cause of the strange result is trying
to operate the op-amp outside of its allowed common mode input voltage
range. If this were cleared up, however, it would likely oscillate unless
you implemented one of the workarounds in the datasheet for obtaining a
unity gain, or (much better) find a different op-amp for your application.
The datasheet states that their absolute focus in designing this op-amp was
low noise and small package size so they purposely traded-off common-mode
range and stability at gain<5 to achieve these goals.

Sean

Post by RussellMc

Post by Sean Breheny
The LT6013 datasheet states that it is only guaranteed to be stable for
gain of 5 or more. Since you are using ...

- Read the data sheet in all areas which may be relevant to the observed
effects.
- Read the data sheet in all areas which may NOT be relevant to the
observed effects.
- An oscilloscope (and a camera) should be surgically attached to your
right arm. (Or to your SPICE virtual right arm where relevant).
- Try a "perfect" component.
- In SPICE et al, de-perfectise perfect components which have imaginary
components. (eg add a small series resistance to "perfect" inductors, ...
).
- Have a virtual (or real) talk with Murphy. "How would you mess this up IF
you wanted to ...?" (he always does.)
- If software is involved, consult Grace Hopper.
- Have ............ ?
R
--
http://www.piclist.com/techref/piclist PIC/SX FAQ & list archive
View/change your membership options at
http://mailman.mit.edu/mailman/listinfo/piclist