3
\$\begingroup\$

I want to model a GaN transistor and include a diode to simulate its reverse conduction above ~2 V with an adjusted diode using the following model statement:

.model revGan D(Vj=2 Eg=3.4)

enter image description here

The result is essentially that of a regular Si diode:

enter image description here

I also tried changing the Eg and Vj parameters, but they seem to have no effect whatsoever. Is that LTspice help page outdated? When using the VDMOS instead of the diode D, which has the body diode integrated, the parameters Eg and Vj still have no effect on the behavior.

\$\endgroup\$
6
  • 1
    \$\begingroup\$ Have you considered that N and ISAT (and the series bulk impedance RS) all impact the forward voltage? \$\endgroup\$
    – periblepsis
    Commented Feb 3, 2023 at 18:51
  • \$\begingroup\$ @periblepsis Yes. These all have the expected influence on the behavior, when I change them..So I surely could create the desired behavior with them alone. Or even just with a voltage dependent resistor... Still I am wondering why the Eg and Vj settings have no effect, because I guess they were intended for changing the diode material. \$\endgroup\$
    – tobalt
    Commented Feb 4, 2023 at 3:59
  • 1
    \$\begingroup\$ I remember that Eg does affect the temperature dependence of ISAT. So, try to adjust the operating temperature to see if your value of Eg does show up as a change in the V-I curve at different temperatures. \$\endgroup\$
    – periblepsis
    Commented Feb 4, 2023 at 4:51
  • 2
    \$\begingroup\$ Correct. Eg only effects temperature dependence (not just on Is, but on Vj too). However, Vj itself only affects the nonlinear junction capacitance. If you want to change the static DC characteristics, you need to adjust Is, N, and Rs (as already mentioned). If you want more direct control over the forward voltage, it might be better to use LTspice's alternate piecewise-linear diode model along with the epsilon parameter. A great answer for working with the standard model can be found here: electronics.stackexchange.com/a/9543 \$\endgroup\$
    – Ste Kulov
    Commented Feb 4, 2023 at 7:59
  • \$\begingroup\$ If you're modeling the MOS, you already have this: there is no body diode on these devices, it's simply the Vgs curve for D/S swapped and Vgs = 0. That is, it should have a quadratic not exponential asymptotic shape, which a SPICE diode won't fit well. (To say nothing of tempco, but alas I'm very unfamiliar with all the MOS parameters in SPICE.) \$\endgroup\$
    – Tim Williams
    Commented Feb 4, 2023 at 7:59

1 Answer 1

Reset to default
3
\$\begingroup\$

No, you cannot. You have a misunderstanding of the function of those parameters. It's not really your fault or the fault of any typical SPICE user, since one would need a fundamental understanding of the underlying device equations used within the software to make sense of it.

Eg is described in SPICE documentation as the "Activation Energy" or the "Energy Gap" of the semiconductor material. Silicon defaults to 1.11eV, and it looks like you set this to 3.4eV for GaN. This is correct, but the effects of Eg in a SPICE diode model is for temperature dependence purposes as it modifies the effective values of the Is (saturation current) and Vj parameters based on simulation temperature. It has no effect on the DC (static) characteristics of the semiconductor itself. Vj (junction potential or built-in potential) itself also has no effect on the DC characteristics. It is purely used for modeling the junction capacitance along with Cjo, M, and Fc. See section 7.3 of the ngspice user manual for more details on the actual device equations.

The parameters of the standard SPICE diode model used to model the main DC characteristics are Is, N, and to a lesser extent Rs. There is a very good answer to an LED modeling question found here which outlines a procedure for empirically determining these values from a datasheet plot: https://electronics.stackexchange.com/a/9543

If you want more direct control over the forward voltage (and/or reverse voltage) of a diode, you can use LTspice's alternate piecewise-linear model. I suggest using the Epsilon (and/or Revepsilon) parameter to smooth the transition regions for more stable SPICE convergence.

Lastly, if you want to use the piecewise-linear model along with a VDMOS MOSFET model, you can put an explicit diode across the MOSFET and disable its internal body diode by setting Is to zero (and also Cjo & tt if you want no capacitance effects). See the example below:

enter image description here

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.