[sdiy] Spice simulation of diff amp

[Andrew Simper]

I have been researching manufacturing mismatch for some time. Certain
simulators have a randomiser built in which applies noise to the model
parameters and can show multiple plots to show the variation. The
filter designer link that was recently posted has this feature. There
is also an "area" parameter I know that Qucs has (and possibly more
simulators?), which modifies multiple parameters at once. Neither of
these approaches is actually going to simulate manufacturing variation
that well, but they are good starting places.

The best paper I've found on the subject so far is:
"INTEGRATED CIRCUIT DEVICE MISMATCH MODELING AND CHARACTERIZATION FOR
ANALOG CIRCUIT DESIGN" by Patrick Drennan
http://citeseerx.ist.psu.edu/viewdoc/download?doi=10.1.1.111.6715&rep=rep1&type=pdf

Which splits things up into different geometrically and spatially
derived variations which intuitively seems like the correct approach
and the actual variations measured look good when compared to real
world examples show in the paper. Using these types equations and
Quc's inbuilt function specifications you could generate multiple
spice parameters and have a look at the results, although this will
take a long time since you'll need to define every device you want to
randomise with a set of functions like this, so lots of copy and paste
and editing and room for error.

I'm trying to automate the process at the moment, but it is early
days. I'm writing a basic circuit simulator that takes a spice netlist
type definition and automatically generates a either c++ sse2 (for
stereo), c++ scalar (for mono), or Mathematica code to solve the with
as few branches and divisions as possible. To this I've begun adding a
"manufacturing" process, where all model parameters are derived from
basic geometric variations described in the Drennan paper. I either do
plots or compile the code into an audio plugin so I can mess around
with things in real time in a DAW and listen to the results.

Andy



On 11 February 2014 02:39, Rutger Vlek <rutgervlek at gmail.com> wrote:
> Thanks Tim! I'll have a look at the books.
>
> Anyone else have experience Monte Carlo-ing Vbe matching in Spice?
>
> Best,
>
> Rutger
>
>
> On 6 feb 2014, at 23:11, Tim Stinchcombe wrote:
>
>>> I'm trying to simulate a differential amplifier circuit in
>>> Spice and hope to be able to run a Monte Carlo test that
>>> allows me to see how various circuit properties respond to
>>> component tolerances. I have an differential pair of
>>> transistors that I figured out how to simulate current gain
>>> variations (within a certain matching accuracy) for, but I
>>> don't know how to do this for Vbe matching. Does the Spice
>>> BJT model have a parameter that corresponds directly to Vbe,
>>> such that I can use this to simulate matching of Vbe within a
>>> certain range? Or is this a case of: move to reality instead
>>> of the virtual domain? :).
>>
>> In a word, 'no'. SPICE uses the Gummel-Poon model, which has about 40
>> parameters to play with:
>>
>> http://en.wikipedia.org/wiki/Gummel%E2%80%93Poon_model
>>
>> but that link doesn't actually give the equations! This here looks to be an
>> early(ish), original SPICE document:
>>
>> http://www.ece.umn.edu/~harjani/courses/common/spice2G6.pdf
>>
>> and the equations are given near the end. So you'll probably have to juggle
>> with things like saturation current, IS, and emission coefficient, NF
>> instead of 'Vbe' (others around here must surely have dabbled in this, so
>> hopefully they will speak up...?). There is tons of stuff about SPICE BJT
>> parameters out there on the net just waiting to be found, or grab a couple
>> of books - I particularly like 'SPICE: Practical Device Modeling' by
>> Kielkowski as it shows how to obtain these parameters from actual measured
>> curves taken from devices, which of course you can _simulate_ and then see
>> how altering the parameters affects the normal BJT-type curves that many of
>> us are more used to dealing with. The other book I frequently refer to for
>> such matters is 'The SPICE Book' by Valdimirescu, which is a fairly
>> down-to-earth book about SPICE and gives the parameters and equations in
>> appendices, again in a fairly concise manner.
>>
>> Tim
>> __________________________________________________________
>> Tim Stinchcombe
>>
>> Cheltenham, Glos, UK
>> email: tim102 at timstinchcombe.co.uk
>> www.timstinchcombe.co.uk
>>
>>
>
> _______________________________________________
> Synth-diy mailing list
> Synth-diy at dropmix.xs4all.nl
> http://dropmix.xs4all.nl/mailman/listinfo/synth-diy