0
\$\begingroup\$

I'm currently troubleshooting an issue with two circuits involving LC components and TVS diodes. Both circuits are designed to ensure the output voltage (Vout2 for the first circuit and Vout3 for the second circuit) does not exceed 20V, as exceeding this threshold triggers the over-voltage protection lock of the connected DC-DC converters.

To address potential overshoot, I've used TVS diodes with a 20V breakdown voltage. Despite this, I'm encountering some unexpected behaviors:

Circuit 1 (Vout2): When I disconnect the TVS diode, the voltage seems to start from 10V instead of 0V. This behavior is puzzling, and I'm not sure why it occurs. Can anyone explain why this initial voltage is observed and how to address it?

Circuit 2 (Vout3): Seems like max voltage reaches 20.2315V although the diode is rated for 20V, how is this possible?

Note: the 33uH is changed manually to try to see the extreme case where the ferrite is an actual inductor. and the purpose was to try to see the difference between the two circuits and fine-tune the values in order to eliminate the overshoot with the wanted output voltage.

Any insights or suggestions on how to mitigate these issues would be greatly appreciated. Thank you! enter image description here enter image description here

22uF Caps: GRM21BR61E226ME44

1uF Cap: GRM155R61E105KE11

TVS: B520C

Link for LTSPICE Schematic & Plot Settings.

Additional Information:

  • The two circuits are used for power connector design.
  • The simulations tries to imitate real life situation where the power plug is connected and reconnected frequently, which can cause this overshoots to happen.
  • The overshoot issue is particularly critical because it can lock the connected DC-DC converters in over-voltage protection mode.
  • Components involved include LRC elements and TVS diodes rated for 20V.

UPDATE: Based on Vincent's Answer, here are some updates:

  1. Added 10K resistors to set the start state.
  2. Picked SMBJ24CA diode to match to the real product voltage (24V instead of 20V in the question).
  3. Removed the short on the GND ferrite beads (the idea was to connect them between GND and GNDC so there will be a high impedance path that will cause the external power surges to make their way to the PSU power instead of being delivered to the system GND.
  4. Added 5 ohm load so it will resemble real life situation where the load is a system that includes many high power consuming devices (all together can reach 66W = 18.44V X 3.68 = 67.85W)

One thing that I still can't figure out, why did the voltage fall to 18.44 W?

A follow up question: raised by Raonoke in the comments: why is the TVS Diode after the 33u Inductor?

Answer: since SMBJ24CA has a large package the only place I can put it is 30mm from the phoenix power connector, since the inductors/ferrite beads were already next to the connector so I left them there, I can move them after the diode, but I saw that electrically (in simulation) that doesn't make any difference.

I would appreciate if someone can add any comment regarding the location of the diode in case it's problematic.

enter image description here enter image description here

\$\endgroup\$
4
  • 4
    \$\begingroup\$ Datasheets for the TVS, ferrite beads, and capacitors, please. And yes, they really are required. \$\endgroup\$
    – Fabio Barone
    Commented May 26 at 9:21
  • \$\begingroup\$ You rely on a very lossy switch and a supply/battery with high internal resistance. Of course there will be no overshoot to talk about. Is that realistic? Why is the TVS diode in front of the 33uH inductor? You could also change the 1M load to something more practical. \$\endgroup\$
    – Raonoke
    Commented May 26 at 14:24
  • \$\begingroup\$ @Raonoke since SMBJ24CA has a large package the only place I can put it is 30mm from the connector, since the inductors/ferrite beads were already next to the connector so I left them there, I can move them after the diode, but I saw that electrically (in simulation) that doesn't make any difference. \$\endgroup\$
    – Firas Abd El Gani
    Commented May 27 at 8:58
  • \$\begingroup\$ FYI, you can't see a difference in the simulation unless you model the trace inductance or other characteristics of the path between LC, TVS and load. \$\endgroup\$
    – Tim Williams
    Commented May 27 at 9:16

2 Answers 2

Reset to default
2
\$\begingroup\$

Insert pulldown resistors (R3 and R5) to set the start state.

Insert source resistors on V3 and V5 to increase the reality of the simulation. In the absence of source resistors, these have zero impedances and the effect of the TVS cannot be simulated.

enter image description here

\$\endgroup\$
2
  • \$\begingroup\$ Hi, Thanks, can you check my question update? \$\endgroup\$
    – Firas Abd El Gani
    Commented May 26 at 13:10
  • \$\begingroup\$ @RussellH, I had assumed that this was the result of trials. It wasn't blocking a simulation because, as you say, "They have no effect" \$\endgroup\$
    – Vincent
    Commented May 26 at 14:06
1
\$\begingroup\$

When I disconnect the TVS diode, the voltage seems to start from 10V instead of 0V.

The reason is a simple voltage divider: S2 has a resistance of 1MEG when off; with R4 at 1MEG, the initial voltage across R4 is half the voltage of V3, so 10V. This doesn't happen with the other circuit; most likely reason being that the LTspice model for D2 has a relatively high leakage current.

enter image description here

Seems like max voltage reaches 20.2315V although the diode is rated for 20V, how is this possible?

Reasons for exceeding 20.00V:

  1. Any circuit with some L & C will have some degree of overshoot when switched.
  2. Because the diode you used is not really a TVS; and even if it was, it would not have a "brickwall" reverse breakdown voltage right on 20.000V.

The part number quoted B520C is not really a TVS, it is a Schottky barrier diode. According to the datasheet, its maximum reverse voltage is 20V, but that does not mean it will safely clamp at 20.00V. The datasheet also lacks the parameters typically provided for diodes intended for transient voltage clamping, such as energy ratings for clamp events, such as "Peak Pulse Power Dissipation with a 10/1000us waveform" (refer to datasheet snippet below). Suggest looking at the P6KE series of TVS diodes.

Link to datasheet:
https://www.vishay.com/docs/88369/p6ke.pdf

enter image description here

UPDATE:

One thing that I still can't figure out, why did the voltage fall to 18.44V?

Answer: simple voltage divider action again.

Looking at the left-side circuit, R1 is 0.5Ω, and S2 has an on resistance of 1.0Ω, and R4.
Voltage divider of 5Ω / 6.5Ω x 24V = 18.46V.

\$\endgroup\$
2
  • \$\begingroup\$ Hi, Thanks, can you check my question update? \$\endgroup\$
    – Firas Abd El Gani
    Commented May 26 at 13:10
  • 1
    \$\begingroup\$ @FirasAbdElGani Done. \$\endgroup\$
    – Fabio Barone
    Commented May 27 at 21:34

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.