Simulate HV Zener

[richsf]

I want to functionally simulate a circuit with a high voltage zener (5 watt around 200 V).  I would like to find a lib for the zener. 

As a substitute, is this circuit going to have the same behavior ?  The R1 in the schematic represents the impedance that zeners in that voltage range have.

[Andy Chee]

It’s evaluation as a substitute cannot be made with the information you have provided.

We need to see the rest of the circuit it is intended to connect to. For example, is it being used as a voltage reference or spike clamp?

[PCB.Wiz]

As a substitute, is this circuit going to have the same behavior ?  The R1 in the schematic represents the impedance that zeners in that voltage range have.

It will probably be 'near enough'.
You match the R1 to the impedance at your operating current, and match the voltage offset to the Zener breakover. (your drawing shows 220+220V = 440V ?)

It will not match the reverse conduction, or the temperature coefficient, but that may be ok ?

[Zero999]

What the part number of the zener?

What simulation software? Is it SPICE based?

Refer to the thread linked below. It's aimed at LTSpice, but is relevant to other SPICE simulators.
https://www.eevblog.com/forum/beginners/zener-diodes-in-ltspice/msg5779479/#msg5779479

[incf]

Creating [good] spice models can be fairly easy and is often worth the time when one desires accurate simulations.

But what you have might be good enough for your purposes. Like other have said, we would need more information about your intended use/circuit/the zener/your simulation software/etc.

In real life, zeners have "soft knees", temperature drift, and noise. But I have simulated many zeners exactly like you have shown for crude/simple circuits where performance didn't matter

Side question: At 200V is it really a zener or is it an avalanche diode?
Side question: Is this diode intended to be a voltage reference/regulator or is it for circuit protection against transients?

[richsf]

Thanks for the comments and advice.   This is a voltage clamp for a vacuum tube #80 power supply.  Since the #80 is a directly heated filament cathode it is alive quickly on power up, however the other tubes in the radio are indirectly heated cathodes.  It takes about 3 seconds for the other tubes to start conduction, so the voltage is high until they load the #80 rectifier.  So, this circuit would provide enough of a load to keep the voltage at a more reasonable level for 3 seconds.  I have a model of the #80 rectifier which seems to be follow the spec sheet curve, which gives me some indication of how much load I need to keep the voltage acceptable.

I still need to select a high voltage zener and will probably use 2 or 3 in series to spread the dissipation, maybe 5 watt range will be enough.  When the power stabilizes this circuit would not conduct any current, because the power is pulled down below the zener voltage in normal operation.    I should learn how to create models, but I think this is OK to get my thinking straight, and to choose the part.  Thanks again.

[richsf]

I'm using kicad which uses ngspice - ltspice compatible mode.  And I didn't pick a part number yet, it will be a 5 watt axial lead part plus a resistor similar to what was shown. 

The initial floating voltage is over 520V (depending on line voltage) then after the set warms  up it is down to about 390V, so there is a lot of room to do this.  In the antique days I think line voltage was lower than today, so the initial voltage is more than the capacitor breakdown for a few seconds.  So this circuit should remove that initial stress.

[moffy]

The SPICE model for a zener has a series resistance variable 'Rs' and a breakdown variable 'BV' e.g.
.model 1N5373B D(IS=1.54e-17 N=1 XTI=1 Rs=.1 Cjo=10p TT=10n BV=68  IBV=20m NBV=50 Vpk=68 mfg=OnSemi type=Zener)
You can create your own.

[Simmed]

I want to functionally simulate a circuit with a high voltage zener (5 watt around 200 V).  I would like to find a lib for the zener. 

As a substitute, is this circuit going to have the same behavior ?  The R1 in the schematic represents the impedance that zeners in that voltage range have.


(Attachment Link)

if on LTspice, open up the standard.dio file inside cmp folder
copy over some other model and add a temporary 200v
eg : BV = 200 just for quick test of the result
on further note, i think would add a series of NTC inrush at the inlet

[Zero999]

A copy of standard.dio can be found on the LTSpice Wiki.
https://ltwiki.org/index.php?title=Standard.dio

There is a model for the 1N5378B, a 5W zener with a breakdown voltage of 100V.

.model 1N5378B D(IS=1.54e-17 N=1 XTI=1 Rs=.1 Cjo=10p TT=10n BV=100 IBV=12m NBV=48 Vpk=100 mfg=OnSemi type=Zener)

Modify it so it's similar to the 200V version, which is the 1N5388B. Refer to the data sheet.

https://www.onsemi.com/download/data-sheet/pdf/1n5333b-d.pdf

Change the breakdown (BV) and peak (Vpk) voltage voltage to 200V.

Increase NBV to 100V.

The data sheet specifies I_ZT = 5mA rather than 12mA, so change IBV to 5m.

Now you have the following model, which should be good enough.

.model 1N5388B D(IS=1.54e-17 N=1 XTI=1 Rs=.1 Cjo=10p TT=10n BV=200 IBV=5m NBV=100 Vpk=200 mfg=OnSemi type=Zener)

[richsf]

Thanks Simmed and Zero999 and others, now I can learn something about making my own zener.  It looks pretty cryptic. 

I thought about the NTC inrush current limiters.  However, 2-4 seconds is a long time period. 

I'll try the zener model, it probably will be more realistic than my makeshift circuit.  There is a tradeoff of course between the clamping voltage and the zener dissipation, the simulation makes a few trials easy to do.  Series connection to spread dissipation should be problem free.  In a couple of weeks I might have parts to do a real world trial, I'll post again then.

Thanks

[Zero999]

If you want better accuracy, then you can cascode the TL431 with a transistor, a MOSFET is better than a BJT, at this voltage and power level.

Here's an example. C1 and C2 are there to improve the transient response. I don't know how accurate the model I've used here, so they might not be required or the values could be wrong. Note that the ratio of C1 & C4 = ¹/_R3 : ¹/_R4, so they form a capacitive voltage divider. C2 might need to be a bit smaller to compensate for the MOSFET's gate charge.