[sdiy] SSM2164 Spice Model

[David G. Dixon]

> Does anyone have a spice model for the 2164 that would be suitable for
> LTSpice that they could email me please?

>From the SDIY archives:

To: "'SDIY'" synth-diy at dropmix.xs4all.nl,
From: "David G. Dixon" dixon at interchange.ubc.ca,
cc: 
Subject: [sdiy] Need a SPICE model for SSM2164?
Date: Tue, 09 Jun 2009 23:00:51 -0700


----------------------------------------------------------------------------
----
Here's a tip for all you simulators out there:

As part of my foray into SSM2164-based VCAs, I wanted to do some Multisim
simulations. However, it turns out that there is no SPICE model for the
2164; at least, none that I can find on the web. I tried simulating the
"simplified" schematic in Figure 23 of the datasheet, but this was a
disaster.

Then I found the solution (at least in Multisim): simply use a user-defined
component known as a "dependent nonlinear source". This bad boy has
non-inverted and inverted outputs which can be defined as either voltage or
current, and its transfer function can be defined with a nonlinear
mathematical formula which depends on as many as 4 different input voltages
and 2 different input currents. Hence, in order to simulate the 2164, all I
had to do was invoke the following formula:

I = I(V5)*10^(-1.5*V(1))

Note that I(V5) is one of the two possible input currents, and corresponds
to the input signal. V(1) is one of four possible input voltages, and
corresponds to the control voltage. This very simple function describes the
current gain of the 2164. I've tested it within a simulation of the test
circuit given in Figure 1 of the datasheet, and it works like a charm. I'd
be happy to send the simulation file to any Multisim users who are
interested. Please let me know offline.

----------------------------------------------------------------------------
----

Further to this, I would add that you can also add the 5k VC pin impedance
to this model in Multisim, and if you want you can even hide the 510R/560pF
input stability network in this model.  I have never used any simulator
other than Multisim, so I don't know if yours has these options or not.

Finally, remember that the output conformance of 2164 is only about +/-0.1V,
and it must really be fed to the virtual ground of an opamp.  This simple
model does not reflect this fact, and thus makes it fairly easy to forget
and misapply the chip in a schematic (I speak from bitter experience
here...)