1
\$\begingroup\$

I'm trying to simulate a band-pass transconductance amplifier in LTSpice, which looks like this:

enter image description here

I used the recommendations of this post - https://electronics.stackexchange.com/a/278870/87695 - and used a G component with a table to represent the voltage controlled current source in my LTSpice schematic.

enter image description here

I have done some estimations on the locations of the poles and zeros:

enter image description here

However, my simulation is not displaying the result I expect to see at all:

enter image description here

I suspect that I set up the voltage controlled current source incorrectly. Here are the parameters:

enter image description here

Any idea of what I did wrong? Thanks in advance.

\$\endgroup\$
5
  • 2
    \$\begingroup\$ I am neither sure how the table there works, nor what you wanted to really see, but I personally usually use BI as the current source and then use V(nxxx) as the value in similar cases. maybe try that? \$\endgroup\$
    – PlasmaHH
    Commented Oct 4, 2017 at 8:29
  • 1
    \$\begingroup\$ That worked and I got the result that I expected: i.imgur.com/ZMi3jZy.png Thanks! \$\endgroup\$
    – w00t
    Commented Oct 4, 2017 at 8:35
  • 2
    \$\begingroup\$ Try a transient analysis with both variants, probably your table thing is causing clipping, I would try -10V -1A, 10V 1A \$\endgroup\$
    – PlasmaHH
    Commented Oct 4, 2017 at 8:49
  • 1
    \$\begingroup\$ Using a table with parameters -10V -1A, 10V 1A gave me the expected results! Good point. \$\endgroup\$
    – w00t
    Commented Oct 4, 2017 at 8:56
  • 1
    \$\begingroup\$ I see nowhere the need of a table(), so you can just replace the whole line with 0.1. BTW, behavioural sources, while versatile, can prove sluggish the higher the numbers, and their dynamic range, both on y and x axis, are reduced. Using a G source is the most accurate and fastest way to do it. Behavioural sources are good when there are more complicated expressions. \$\endgroup\$
    – a concerned citizen
    Commented Oct 5, 2017 at 8:05

2 Answers 2

Reset to default
2
\$\begingroup\$

Creating the current source with a table starting at 0V 0A probably clips your swing into the necessary negative direction, thus distorting the waveform and messing up the frequency response plot.

Giving it a wider range (-10V 1A, 10V 1A) gives it more headroom, but it could be clipping there too.

It might make more sense to use a BI source and simply set the current to a formula depending on the voltage of your node, this will not cause any clipping. I recommend though to label the net, as the n### automated node names can change.

\$\endgroup\$
2
\$\begingroup\$

Why don't you use the arbitrary behavioral current source, called "bi" in the symbol library of LTSpice:

It will look like that:

enter image description here

Then the simulation results looks like that:

enter image description here

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.