How can I use/model a custom diode in LTSpice?
The usual model (based on Spice 3f5) for breakdown in diodes is influenced by 4 parameters:


\$BV\$ - Reverse breakdown voltage in volts
\$IBV\$ - Current at reverse breakdown voltage
\$IS\$ - Saturation current
\$N\$ - Emission coefficient / Ideality factor


From these parameters, Spice will attempt to calculate (iteratively) the "real" breakdown voltage \$XBV\$ to make the curve go through \$(BV, IBV)\$. Spice does this once during setup (or whenever the temperature has changed).

In reverse breakdown, the following equation is subsequently used:

$$i_D = -IS_{eff}\cdot e^{-\frac{XBV + v_D}{N\cdot U_T}}$$

\$IS_{eff}\$ is the reverse saturation current after applying temperature-dependent effects.

LTSpice claims in their documentation that


  The other model available is the standard Berkeley SPICE semiconductor diode but extended to handle more detailed breakdown behavior and recombination current.


I believe that they point to the parameters:


\$ISR\$ - Recombination current in amps
\$NR\$ - \$ISR\$ injection coefficient
\$IKF\$ - High-injection knee current


Unfortunately, I don't know much about these parameters.



APPENDIX

I did found some information about similar parameters here on HSpice.


  Most diodes do not behave as ideal diodes. The parameters IK and IKR are
  called high level injection parameters. They tend to limit the exponential current increase.


$$i_{D,eff} = \frac{i_D}{1 + \left( \frac{i_D}{IKR_{eff}} \right)^{1/2}}$$

$$i_D = IS_{eff}\cdot \left(e^{\frac{v_D}{N\cdot U_T}} - 1 \right) - IS_{eff}\left[e^{-\frac{v_D + XBV}{N\cdot U_T}} - 1\right]$$