Implementing the EKV MOSFET model for DC in Visual Basic (long)

Andy C

unread,

Sep 11, 2007, 8:28:21 PM9/11/07

to

Hi all,

You may be wondering why anyone would want to implement the EKV MOSFET
model in Visual Basic. I'm working on audio power amplifier design, and to
accurately simulate crossover distortion of a MOSFET class AB output stage,
it's necessary to take into account MOSFET subthreshold conduction. The
EKV model seems to be the simplest MOSFET model that does subthreshold
conduction. Also, in the past I've had good luck with DC model parameter
fitting using the Excel solver. Using a freeware called the Engauge
Digitizer, it's possible to capture datasheet graphs of drain current into
.csv files containing graph data that can be imported into Excel. Then one
implements the DC equations of the device model in Excel Visual Basic for
Applications (VBA). One defines a cell that represents, say, the sum of
squares of the errors between measured and simulated drain currents, and
some other cells containing model parameter values. Then you just tell the
Excel solver to adjust the model parameters to minimize the value of the
cell containing the aggregate error. The solver works pretty nicely as an
optimizer in this way - surprisingly well, actually.

Of course, these are vertical MOSFETs, so there are other issues like
simulating the nonlinear gate-drain capacitance. I won't get into that
here.

Anyway, I downloaded the EKV model manual from the EKV web site. That
manual is here:

http://legwww.epfl.ch/ekv/pdf/ekv_v262.pdf

I implemented the DC equations in a big VBA function. This function takes
gate, drain and source voltages, along with about 20 EKV parameters as
arguments and spits out a drain current. Once it's implemented, it can be
called from Excel just like a built-in Excel function.

The problem is, I can't get the predicted drain current to be dead-on equal
to what a simulation of the same circuit in LTSpice gives me. The example
I tried was from the EKV chapter of the book called "Device Modeling for
Analog and RF CMOS Circuit Design" by Ytterdal, Cheng and Fjeldly (Chapter
7). The model parameters are as follows:

.model ekv_test nmos level=12 cox=3.45m xj=0.15u
+ vto=0.6 gamma=0.71 phi=0.97 kp=150u e0=88e6
+ ucrit=4.5e6 dl=-0.05u dw=-0.02u lambda=0.23
+ ibn=1.0 iba=200e6 ibb=350e6
+ weta=0.05 q0=280u lk=0.5u
+ leta=0.28

The Level 12 thing for EKV is LTSpice-specific. In Micro-Cap it's level 44
and varies with other simulators. The circuit I used is a simple DC bias
circuit with Source = Body = ground, gate = 0.7 Volts (just above
threshold) and drain = 5 Volts. LTSpice gives me a drain current of 10.794
uA. My function gives 10.297 uA. A friend with Micro-Cap simulated this
and got 10.795 uA, almost exactly matching LTSpice. I'm trying to figure
out how to get my function to be this accurate. I am currently about 4.6
percent off.

Here's what I've tried so far. In the EKV model, there's the weak
inversion region (subthreshold conduction) where the drain current looks
like an exponential function of Vgs. Then there's strong inversion, where
it's a square law relationship. There is an interpolation function, not
specified in the EKV model manual, that joins the two regions together in a
continuous way. Another paper on EKV specifies the interpolation function
as i = (ln(1+exp(v/2))^2, where i = normalized current and v = normalized
voltage. When I use this function, the current in the VBA code is way off
from the SPICE simulation - about 20 percent. The EKV web site says the
full Verilog-A code of the model (version 2.6) is available on request, so
I sent a request for it. Unfortunately, I haven't heard back from them.
In the meantime, I found the Verilog-A EKV 2.6 source code available for
download at the Silvaco web site. So I downloaded and translated it into
VBA and got data much closer to the simulation. Here is the Verilog-A code
for the interpolation function:

// Normalized forward current is iff (equations 43-44 in the EKV manual)
// Normalized forward voltage is fv
fv=(VP-VS)/$vt;

if (fv >= -0.35)
z0=2.0/(1.3 + fv - ln(fv+1.6));

if (fv>=-15 && fv<-0.35)
z0= 1.55 + exp(-fv);
else
z0=1;

z1=(2.0 + z0) / (1.0 + fv + ln(z0));

if (fv > -15.0)
y=(1.0 + fv + ln(z1)) / (2.0 + z1);
else
y= 1.0 / (2.0 + exp(-fv));

iff = y*(1.0 + y);

When I translated this code into VBA and used it for my interpolation
function, I went from 20 percent error to 4.6 percent. However, this code
is suspect. If the first "if" statement evaluates to true, z0 gets
assigned. But then it will just get reassigned in the "else" branch of the
next "if" statement. Unfortunately though, fixing the first "if" statement
to put an "else if" in there doesn't help beyond the improvements I got by
replacing the interpolation function I was using before (the one with logs
and exponentials). So I'm still at 4.6 percent error. I'd like to get as
close as the two simulators from two different vendors are. The friend who
tried the sim with Micro-Cap also tried it with the option to use the
interpolation function with exponentials and logs. When I use that same
interpolation function in my VBA code, I still get errors from his result
on the order of 5 percent. So it's not just the interpolation function
that's causing the problem.

I've also noticed other discrepancies and tried other things. For example,
the EKV manual states the dielectric constants of the silicon and the oxide
as:

EKV manual:
eps_si 1.045e-10
eps_ox = 3.45e-11

but the EKV Verilog-A code says this:

Verilog-A code:
eps_si = 1.0359e-10
eps_ox = 3.453143E-11

Anybody know which should be used? I actually get closer to the SPICE
simulation by using the values from the EKV manual, not the Verilog-A code.

At one point I figured that if I just translated the entire Verilog-A code
line-by-line into VBA I'd be able to get agreement. I did so, and the
result is the exact same as the code created when I followed the algorithm
specified in the EKV manual, before I had access to the Verilog-A code.
This required changing the interpolation function and the dielectric
constants to match the Verolog-A code.

So I am absolutely stumped. One thing I thought of was that SPICE is
taking into account extrinsic elements of the model, such as a MOS diode
from drain to body. The equations in the EKV manual are for the intrinsic
device only. If this were the cause of the 0.5 uA discrepancy though,
you'd think it would show up in the body current. But the computed body
current in my code is extremely close to what LTSpice reports. This
current is only about 0.25 uA or so, or about half of the discrepancy I'm
seeing. Another thing I thought of is that the EKV equations in the manual
don't take into account the extrinsic resistances. But my code gives drain
current that's low for this example, and extrinsic resistances would reduce
the current still further, and require iterative solution as well.

Is there anybody out there (Mike E. maybe?) that has implemented this thing
and might provide some hints? Is the Verilog-A code on the Silvaco site up
to date? Is there something undocumented I'm not taking into account? I'm
starting to run out of ideas.

Any help appreciated,
Andy C

Jim Thompson

unread,

Sep 12, 2007, 9:41:13 PM9/12/07

to

On Wed, 12 Sep 2007 00:28:21 GMT, Andy C <no...@none.invalid> wrote:

>Hi all,
>
>You may be wondering why anyone would want to implement the EKV MOSFET
>model in Visual Basic. I'm working on audio power amplifier design, and to
>accurately simulate crossover distortion of a MOSFET class AB output stage,
>it's necessary to take into account MOSFET subthreshold conduction.

[snip]

PSpice Level=7 (which I think is the same as HSpice Level=49) BSIM3
supports modeling the sub-threshold region.

Awhile back I did a rudimentary cut at some of Win's data to show that
it could be done.

Andy C

unread,

Sep 14, 2007, 12:07:09 PM9/14/07

to

On Wed, 12 Sep 2007 18:41:13 -0700, Jim Thompson wrote:
>
> PSpice Level=7 (which I think is the same as HSpice Level=49) BSIM3
> supports modeling the sub-threshold region.
>
> Awhile back I did a rudimentary cut at some of Win's data to show that
> it could be done.
>

Hi Jim,

I'm aware that the BSIM models support subthreshold conduction. But I
found after studying them that they were quite complex. Check out the
manual for BSIM3v3 here:

http://nikola.com/pdf/bsimset.pdf

Contrast this with the simpler and clearer EKV docs here:

http://legwww.epfl.ch/ekv/pdf/ekv_v262.pdf

I know which one I'd rather code up :-). Also, it appears that the EKV
model does quite well considering that it has far fewer parameters than
BSIM3. Check out this comparison by a guy from LSI Logic:

http://www.nsti.org/Nanotech2002/WCM2002/WCM2002-PBendix.pdf

At any rate, the problem is solved. The manual linked above is for 2.62 -
their latest documentation. It appears that the simulators out there are
implementing a later version. On the EKV web site, there is VHDL-AMS code
for the model. It is here:

http://lsmwww.epfl.ch/models/compact/

When I ported the VHDL-AMS to Visual Basic, the currents of the test
circuit and the VB implementation matched up. So I am a happy camper :-).

Jim Thompson

unread,

Sep 14, 2007, 12:33:55 PM9/14/07

to

I'll have to try that. PSpice supports the EKV model, so I'll have to
try fitting some data... just for fun ;-)

Andy C

unread,

Oct 21, 2007, 3:08:34 PM10/21/07

to

On Fri, 14 Sep 2007 09:33:55 -0700, Jim Thompson wrote:

>
> I'll have to try that. PSpice supports the EKV model, so I'll have to
> try fitting some data... just for fun ;-)
>

Well, here's an update. I transcribed the VHDL-AMS code from the EKV web
site, listed here:

http://lsmwww.epfl.ch/models/compact/files/ekv2.6_e/dc.vhd

from the VHDL-AMS to VBA. This code *mostly* gives answers that compare
very closely with commercial simulators. However, there's still some
corner cases that have problems. One such case that I've found relates to
the parameter PHI. The EKV 2.6 manual, available here:

http://legwww.epfl.ch/ekv/pdf/ekv_v262.pdf

states that PHI can be as low as 0.1. However, the VHDL-AMS code linked
above limits PHI to a minimum value of 0.2. Checking LTSpice, it clearly
allows PHI down to 0.1. Also, I've found several cases where the VHDL code
allows a condition for legal device parameter sets where the square root of
a negative number is taken, resulting in errors. The VHDL-AMS code, even
though it is a more recent revision than the EKV 2.6 manual, is still not
the same as what current simulators implement.

So I've pretty much exhausted my possibilities here. Repeated attempts to
contact the EKV developers to simply have the latest source code sent to me
(in whatever language is available) have resulted in no reponse whatsoever.
They claim on their web site that they support their models, but they don't
even answer their emails.