Re: gEDA-user: SPICE/gEDA updated. . . . .

[mcmahill@mtl.mit.edu]

On Mon, 24 Mar 2003, Stuart Brorson wrote:

> Sorry for the delay in responding. . . . .
> 
> > As a more concrete example, suppose you have a standard CMOS process.  You
> > may have only 2 models for transistors.  One is NMOS and one is PMOS.  If
> > you take a look at the line in a spice netlist for say the nmos
> > transistor, it looks something like:
> > 
> > M1 drain_node gate_node source_node bulk_node model_name list_of_parameters
> > 
> > This may look like:
> > 
> > M1 2 1 0 0 nmos W=100u L=0.6u
> > 
> > in its most basic form where W and L are gate width and length.  So far,
> > we can get by with a simple .include statement to pull in a model file for
> > the process which would include a nmos model (plus probably a pmos model
> > and perhaps some resistor and capacitor models).
> > 
> > 
> > However to properly model the diode formed by the source/drain diffusions
> > and the substrate, you also need to specify the AS, AD, PS, PD parameters.  
> > Now your FET call looks more like:
> > 
> > M1 2 1 0 0 nmos W=100u L=0.6u AS=200p AD=200p PS=204u PD=204u
> > 
> > where the exact calculation of what AS, AD, PS, and PD is based on 
> > 
> > - what are W and L
> > - how many fingers used in the device (you wouldn't make a 100u x 0.6u
> >   rectangle but would break this into perhaps 10 rectangles which are 10u
> >   x 0.6u)
> > - what is the minimum gate to contact spacing
> > - what is the contact size
> > - what is the minimum amount the diffusions must enclose contacts by.
> > 
> > So in practice what happens with a tool such as cadence, a process design
> > kit has been developed so that when you enter W and L for a device, the
> > tool calculates what AS, AD, PS, and PD will be so that when the netlist
> > is created for simulation, those values (fully evaluated, ie, the
> > netlist doesn't have equations but rather the outputs of equations) are
> > included in the netlist.
> > 
> > To summarize, for IC work, you typically have both a model file which gets
> > included somehow and some other technology specific setup which affects
> > how a schematic gets netlisted including doing things like calculating
> > additional parameters from a set of specfied parameters.
> > 
> > Hope this clarifies things a little bit.
> 
> 
> Yeah, thanks.  Now some questions:
> 
> 1.  Will the parameters of the calculations apply to *all* MOSFETs?
> Or to just those whose model-name is "nmos"?    The point here is that
> I need to know what attribute to key off of -- the (DEVICE or REFDES)
> or the MODEL-NAME.

The parameters can be expected to vary based on the device.  For example,
some MOS processes offer options like a low threshold voltage device or a
thicker oxide device to support a higher voltage I/O.  The design rules
would be different for these devices.

> 2.  Are the formulas used the same for  all MOSFETs?  Or does they vary
> from model to model?  (Note that I don't mean the coefficients, but
> rather the actual form of the formulae.)
> 
> This is important because if the formulae are the same for all
> MOSFETs, you can build them into the netlister.   The netlister
> recognizes different components based upon their DEVICE attributes, or
> the first letter of their REFDESs.  Once  the device type is
> recognized, a different Scheme function is used to handle each
> different device.  If the formulae are the same for any particular
> device,  the scheme function can just parse up the component
> parameters, get the coefficients from the tech file, and use built-in
> formulas to get the desired output  parameters.  Although it is not
> trivial, I can envision how to do this. 
> 
> However, if the forumlae are different depending upon the individual
> device (i.e. depends upon the model), you need to build the formula
> itself into the technology file, create an execuitable Scheme
> expression from it, and then execute an "eval" in Scheme.
> This seems to me to be fairly difficult, or at least more of a PITA. 

I _think_ the formulas should be constant for different processes but with
different parameters.  However, I can't claim to have enough experience in
delving into that level of detail on the cad system for enough different
processes to be sure.

-Dan