Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Very basic Zener Diode/LTSpice simulation question

Status
Not open for further replies.

eranrund

Newbie level 5
Joined
Feb 12, 2005
Messages
8
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
75
Hello.

I have set a very simple circuit in LTSpice: Voltage source of 12v connected to a resistor connected to a 8.2v Zener diode.
When measuring the voltage between the diode and the zener I notice two things I cannot explain:
1) The measured voltage is around 8.7v (i was expecting 8.2)
2) From 0ms to ~1.5ms I see the voltage slightly dropping. Why is that?

Attached is a screenshot.

Many thanks:)
 

Attachments

  • zener.png
    zener.png
    54.5 KB · Views: 141

1) The measured voltage is around 8.7v (i was expecting 8.2)
2) From 0ms to ~1.5ms I see the voltage slightly dropping. Why is that?

1) The datasheet states 8.2V as typical, 8.7V as max. value for a current of 5mA !
2) You're running 189mA thru the Z-diode, resulting in 1.64W of power dissipation. The transient result shows a very very small negative temperature coefficient, which surely is wrong, as Z-diodes with Vz >≈ 6V have positive TCs.

It does not show that the diode already would have blown up before the end of simulation, as 1.64W of power dissipation would heat it up to nearly 1000°C (free air cooling on an FR-5 board) :) .
 

I see. What a dumb mistake :)
I switched the resistor to 730ohm, resulting in 5.03ma current and voltage of 8.3v. At least I'm not frying it up this time.

In this case however, what would be the cause of seeing 8.3 and not 8.2? How does the Zener model determine this? Simply by assuming a possible 5% variation?

Thanks for the reply
 

No. I think it considers the diode's TC:
8.3V*5mA=41.5mW ; 41.5mW*556°C/W≈23°C=ΔT ; 23K*(+4.7mV/K) ≈ +0.1V
 

The transient result shows a very very small negative temperature coefficient, which surely is wrong, as Z-diodes with Vz >≈ 6V have positive TCs.

Do you think that the LTSpice diode model implements a mixed physics simulation considering power dissipation and respective temperature variations? If so it's not documented anyhow. Known standard SPICE models don't, they would need to define a chip and package geometry and material properties as a prerequisite.
 

You're right, that's unusual. Diode models just contain their inherent T-dependency. I don't know, however, if LTSpice models perhaps add the (trivial) power calculation and a (default?) thermal resistance value. On the other hand, I can't imagine the ΔV=0.5V in the OP's 1st post, which suggests the breakdown voltage of this individual Zener diode package (in case of free air cooling) for its max. permitted junction temperature (150°C).
 

The difference is about 50 uV and looks more like a simulation artefact. No idea how it's generated.

There's nothing like Rth in the model, see below. Ibv=1m clarifies, why a higher voltage is measured at 5 mA.

Code:
.model BZX84C8V2L D(Is=.8n Rs=.5 Cjo=135p nbv=3 bv=8.2 Ibv=1m Vpk=8.2 mfg=Motorola type=zener)
 

LTspice allows you to define a global temperature for the simulation, but it does not automatically calculate temperature rise. Unless you tell it otherwise, it assumes everything is at 25 degrees C (I think).
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top