In LTspice is there any way of editing a silicon bjt model to make it behave like a germanium bjt model, at least approximately? I've tried tinkering with various model parameters to no avail: LTS always thinks Vbe ~0.6V rather than ~ 0.2V as I'd hoped.

 

@Bordodynov has some germanium models.

 

Yes. Thanks for reminding me. However, I was wondering if a silicon model could be hacked in some way.

 

Yes. Thanks for reminding me. However, I was wondering if a silicon model could be hacked in some way.

Go to the groups.io website for the LTspice Users Group. Our good friend Alex @Bordodynov has a germanium library that might give you some clues. On the same site you can find models for the AC127 and AC128 transistors contributed by Helmut Sennewald.

 

Diodes and bipolar transistors have a parameter "is". The larger it is, the smaller the drop across the PN junction at the same current.
And for the mentioned transistors I made my models using detailed datasheet.

 

Diodes and bipolar transistors have a parameter "is". The larger it is, the smaller the drop across the PN junction at the same current.

Ah. That's useful info. Thanks.

 

In LTspice is there any way of editing a silicon bjt model to make it behave like a germanium bjt model, at least approximately? I've tried tinkering with various model parameters to no avail: LTS always thinks Vbe ~0.6V rather than ~ 0.2V as I'd hoped.

Hi,

Start with a silicon diode and go from there.
Ask what can you change to make the forward voltage at a particular forward current what you want it to be.
The answer will come mostly in the form of three variables:
IS, often called the "saturation current",
N, often called the "ideality constant", and
Rs, the series resistance associated with the internal contact resistance.

IS and N play together and since Rs is in series, it must be small enough at the desired current in order to keep the forward voltage as low as 0.2 volts for example. If you fool around with it enough, you can even get a forward voltage of 0.02 volts for example, which is good for simulating something that acts like an ideal diode.

You can also calculate the values for N and IS from one of the diode equations:
V=0.026*ln(i/IS+1)+i*Rs {where ln() is the natural log, 'i' is forward current, V is forward voltage}

You can start with just:
V=0.026*ln(i/IS+1)

and set for example V=0.2 and I=1 amp, then solve for IS.
Those examples assume N to be of some reasonable value, but because you probably want to set that in the spice model too, you can use:

V=Vt*ln(i/IS+1)*N

Vt here is usually taken to be 0.026 and that gets you pretty far. You can add Rs later.

You can solve that for N:
N=V/(Vt*ln(i/IS+1))

This allows you to set the forward voltage V and the forward current 'i' and IS, then solve for N.

Note that most math software uses "log(x)" rather than "ln(x)" for the natural log.

Once you get the values you need, plot the voltage over a range of currents 'i' and see if you like how the plot looks.

Rs causes the latter part of the response to look like a straight line, so you can look at the first derivative dv/di if you want to match that to some data sheet plot. If not, just choose some Rs that seems appropriate. It should be relatively low though. The derivative near i=max would probably be the best place to find the slope and thus Rs. That's if you have a particular curve for the diode in mind.

Just to note: as IS gets larger, the diode curve becomes more rounded, with a more gradual rise in voltage with current. This assumes you calculate a new N for each value of IS, which would be required in order to maintain the desired forward voltage at the desired forward current. See attached plots.

 

Thanks for the detailed response. The spice parameters have always been a bit of a mystery to me.