3
\$\begingroup\$

How does this gate driver generate 200 V from a 12 V supply? And why when off does it never go below 50 V?

enter image description here

XIC1 Vosc N002 0 Vcc N001 N003 NC_01 NC_02 1EDN7511B
Vcc Vcc 0 PWL(0 0 100u 0 110u 10)
R1 0 N002 1
V1 Vosc 0 SINE(2 2 7MegHz)
Rload Drive 0 10Meg
C1 Vcc 0 1µF
C2 Drive 0 1nF
R2 Drive N001 100
R3 Drive N003 100
.lib 1EDN7511B.lib
.tran 0 2ms 0 1us

enter image description here

Lowering the output resistors R2 and R3 brings the high output voltage to something reasonable — but the low output voltage still stays at around 1.3 V.


Update

To clarify: Something is clearly off here. The question is:

  • Is it a problem with the simulator? What's wrong with the simulation? What would the circuit's output really be?
  • Is it a problem with the circuit itself? How does the circuit need to be changed?

What would the high and low voltages look like if the circuit were actually built? Note that lowering R2 and R3 drop the voltages, but the low voltage never goes beneath 1.2 V (on LTSpice).

Also, note below that setting Tamb to 25 V made the problem worse.

\$\endgroup\$
6
  • 1
    \$\begingroup\$ Why are you pulsing the supply voltage while forcing voltage into an input pin? Why is the device temperature undefined? \$\endgroup\$ Commented Jun 14 at 13:52
  • \$\begingroup\$ @TimWilliams Infineon's docs (in the zip that includes the model) recommend using a PWL voltage supply with those params, and to look at the circuit only after a ms or so, because the IC takes time to reach its operating state, which it does when power goes on. As for device temp, I'll work on implementing the suggestion from your answer. \$\endgroup\$ Commented Jun 14 at 14:45
  • \$\begingroup\$ Ah, is that a steady output then, not repetitive? \$\endgroup\$ Commented Jun 14 at 15:33
  • \$\begingroup\$ Your title says "12V supply" but your spice netlist doesn't have 12 anywhere. \$\endgroup\$
    – Ben Voigt
    Commented Jun 14 at 21:16
  • \$\begingroup\$ @BenVoigt Originally, it was 12V supply. In attempts to debug it, I pasted it the exact 10V PWL supply recommended by Infineon in their docs. It didn't solve the problem. \$\endgroup\$ Commented Jun 14 at 22:04

5 Answers 5

3
+50
\$\begingroup\$

I don't know exactly what's wrong with this model in LTspice (note that it does not claim to be compatible- "SIMetrix version 8.3g or higher") and I didn't try very hard to make it work, so you may well want to save your bounty for another, better, answer, but I did give it a try in Mike E.'s (free to download, free to use) Qspice - the symbol was autogenerated- with a minimal useful circuit.

enter image description here

Here is the input and output:

enter image description here

Completely hassle-free.

Simulating thermal response at the same time as trying to get accurate simulation during each 100ns-ish cycle is a bit of a fool's errand unless you have enormous computing resources, a lot of patience or a much better model/simulator combo.

In a few ms it's up to 60°C+ though (from 27°), and the average power from the supply as shown is about 1.17W using the .options savepowers=1 directive. That corresponds to a temperature rise of about 74°C using the best package with the thermal pad.

With the savepowers turned off to speed it up, a 10 minute thermal simulation on my i7 machine would take more than 2 years (and the amount of data would probably crash the machine). And we know what the answer will be anyway with a few seconds calculation from the average power dissipation.


As per request from @SRobertJames, I entered in the exact circuit in OP's image (with temperature input added 27°C). It failed with "timestep too small" but only when the sine wave input to the digital input was substituted for the digital input. Upon inserting a resistor between the sine wave source and input it gave expected results. Anything less than about 10Ω causes it to fail.

enter image description here

enter image description here

There's some wobble in the triangle-like output waveform that suggests the solver may have cut it a bit close to get accurate results, or it might be related to the behaviour of the "active filter" shown in the block diagram- but generally it looks okay.

Start-up:

enter image description here

The simulated input current through the added resistor, even during start-up is small, less than 10uA.

enter image description here

Not sure if this helps, but it indicates that your "weird" application of a sine wave to a digital input and pulsing Vdd with signal applied may be a factor.

\$\endgroup\$
1
  • \$\begingroup\$ Thanks. As a true test, what does QSpice say about the OP's circuit? \$\endgroup\$ Commented Jun 18 at 1:30
3
\$\begingroup\$

That’s not realistic.

This is a low side driver, so it is limited to the supply voltage. High side drivers either require a floating supply or (sometimes) can bootstrap a high voltage using (essentially) a charge pump from fluctuations in a swing node, but in this case there isn’t anything like that.

I assume you’re just running a spice/ltspice model rather than testing a physical device? It’s probably an issue with how the model is constructed internally.

\$\endgroup\$
3
  • \$\begingroup\$ Yes, LTSpice. I accept that something is wrong. What should the high and low output of the circuit really be? \$\endgroup\$ Commented Jun 14 at 3:49
  • 1
    \$\begingroup\$ 0 and 12V. It drives the gate to its supply voltage when on, to ground when off \$\endgroup\$
    – Alex I
    Commented Jun 14 at 4:29
  • \$\begingroup\$ I don't see anything suggesting this was misinterpreted as, or is being applied as, a high-side driver. \$\endgroup\$ Commented Jun 14 at 14:00
1
\$\begingroup\$

From the simulation model support files:

enter image description here

Source: Infineon-Gate_driver_EiceDRIVER_1EDN7511B_TINA_PSPICE_SIM-SimulationModels-v02_00-EN.zip/Model/results/demo_testbench.png, downloaded from https://www.infineon.com/cms/en/product/power/gate-driver-ics/1edn7511b/?tab=~%27simulation_models#!designsupport

Vtamb sets the ambient temperature of the device. With TAMB floating, your simulation results are probably not meaningful.

I'm surprised it didn't simply fail with a divide-by-zero error or something to that effect; floating connections tend to be poorly behaved.

\$\endgroup\$
1
  • \$\begingroup\$ Adding 25V to TAMB raised it to 300V. Even more impossible! And the off voltage dropped to about 2V - still not 0. \$\endgroup\$ Commented Jun 14 at 15:37
0
\$\begingroup\$

why when off does it never go below 50V?

Because the discharge time is too short. Make the "off" time period 10x longer (keeping the "on" time unchanged) and see what happens.

In theory, a simple exponential decay never reaches 0.000 V. In practice, it does. In EE school, the first thing you learn after Ohm's Law is the transient response of an R-C circuit.

https://en.wikipedia.org/wiki/RC_circuit

\$\endgroup\$
3
  • 1
    \$\begingroup\$ Even at 1 MHz, I get an off voltage of 1.4V. Do you mean the discharge time is too short for the simulator to produce realistic results? Or that in real life, the off voltage will never drop beneath 1.4V? \$\endgroup\$ Commented Jun 14 at 4:40
  • \$\begingroup\$ See answer update. \$\endgroup\$
    – AnalogKid
    Commented Jun 14 at 12:49
  • \$\begingroup\$ It's a gate driver, the output voltages are constrained to -0.3 ... VDD+0.3 by body diodes. The RC time constant is irrelevant; something else must be the problem here. \$\endgroup\$ Commented Jun 14 at 13:59
0
\$\begingroup\$

If the supply voltage is 12V, then the maximum output voltage can only be 12V. Because this is a gate driver, not a boost converter.

I don't think this is a mistake of LTSPICE. Because on the website of 1EDN7511B, the model is based on the software SIMetrix. So there may be some compatibility issues between different software.

This is a common issue when you are using a different software for simulation. And even Infineon will suggest you to use SIMetrix when someone tried to do it on LTSPICE. See the below link.

https://community.infineon.com/t5/MOSFET-Si-SiC/Error-in-Simulation-of-Spice-Model-IMZA120R007M1H-L3-for-Dynamic-Test-Circuit/m-p/479650#M3864

So I guess if you contact Infineon, you will get the same reply.

Two solutions:

(1) Use a different gate driver, since the low-side gate driver is easy to find. I will suggest you to use gate drivers from ADI, since they develop LTSPICE.

(2) If you have to use 1EDN7511B, test it on a real circuit.

\$\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.