I can't create the model for you (it isn't my area of expertise),
however, I can answer some of your other questions. The short answer is
that you probably don't want to be doing code modelling, instead, you
need someone to modify the SPICE macro model.
In case your interested, I'll also give the long answer.
There are several levels of 'models' in SPICE, and unfortunately, we
often use the word 'model' to mean several different things.
The core of SPICE is an equation solver. The equations SPICE is solving
represent things, such as a resistor or a MOSFET. However, these are
only approximate representations of these devices. For example, you
could describe a resistor as only having 'resistance' excluding other
effects such a temperature. Similarly, there are a variety of MOSFETS,
so one single set of equations does not describe all MOSFETS well.
Consequently, there are several devices that represent MOSFETs to
SPICE. This is the most basic level. When you create a code model, you
are working at this level.
One step up from devices is SPICE macro models. These combine a number
of primitive devices into a single unit. For example, an Opamp is
constructed from resistors, capacitors, transistors, etc. Rather than
create a primitive and generic Opamp, the model for an Opamp is a
combination of these primitive units. The actual units may not be the
same as the construction of the Opamp - for speed, it is often better
to focus on specific characteristics of interest, rather than
representing the topology of the Opamp exactly.
So, for your main question. When you edit a component's model, you are
doing one of two things. (1) You are changing the values of parameters
in the device - typically when you modify RLC, diodes, transistors.
This is because usually these are often represented by primitive
devices with different parameters. (2) Alternatively, you are changing
the SPICE macro model - typically for things such as Opamps or more
complex ICs, but it can also apply to describing components such as
diodes where the device does not adequately represent the important
characteristics.
For the avalance breakdown case, the primitive diode device does not
include effects of avalance breakdown. To include this effect, there
are two possible approaches (1) create a new SPICE diode device that
includes this effect, or (2) create a SPICE macro model using some
combination of devices to include this effect. Option 1 is very
difficult. Researchers often spend years working at this level. Option
2, while not necessarily easy, is usually much easier (orders of
magnitude easier).
The model from diodes.com for the FMMT413 is a SPICE macro model. You
can see this if you look at the model, you see ".subckt" and there are
a number of different primitives in the SPICE macro model. I think Max
created a Multisim component for you that uses this SPICE macro model.
The model seems to be from the manufacturer, so it is probably the best
model that currently exists for this particular component. What you
need is someone to modify the SPICE macro model to include this effect.
