I'm working on understanding bootstrapping, so I copied the schematic used in this YouTube tutorial in LTspice. However, my simulation doesn't appear to yield the results that I would expect from a properly bootstrapped circuit. While the gate-source voltage appears to be properly switching between zero and (approximately) twelve volts, the load doesn't have twelve volts across it, which is kind of the point, as I understand it...

Bootstrap Schematic and Simulation

I noticed that the content creator said repeatedly in the comments that this circuit is not intended for high-frequency switching, so I made the switch toggle very infrequently (once per second), but this didn't appear to fix the problem. I also added a gate-source capacitance to model the internal capacitance of the transistor and made sure that the bootstrap cap was ten times this value in accordance with rules of thumb, but this didn't help.

At this point, I can't tell if the problem is my implementation of the schematic or my simulation parameters (.tran 4). Does anyone have any ideas?

  • 3
    \$\begingroup\$ Please don't ever use the default NMOS model in LTspice. Right-click the symbol and select a specific part number. It's not as important for the NPN or the diode, but I suggest choosing 2N3904 and 1N4148 for those, respectively, if you need to just pick something "generic". \$\endgroup\$
    – Ste Kulov
    Jan 26, 2021 at 19:46
  • \$\begingroup\$ I just looked at the video and saw in the breadboard he has an IRF1405. This model is available in the part list for NMOS, so please select that one. \$\endgroup\$
    – Ste Kulov
    Jan 26, 2021 at 19:49
  • \$\begingroup\$ Oof... well, that's all it took. I swapped the MOSFET and adjusted the bootstrap cap, and it worked like a charm. Thanks! If you want to post your suggestion as an answer, I'd be happy to accept it and bestow some internet points upon you. \$\endgroup\$ Jan 26, 2021 at 19:49
  • 1
    \$\begingroup\$ Sure, I'll write something up a little more detailed since this is bound to come up again so we might as well archive it properly. I can care less about the points. haha. \$\endgroup\$
    – Ste Kulov
    Jan 26, 2021 at 19:50

1 Answer 1


The main thing I notice when looking at your LTspice schematic is that none of the semiconductors (MOSFET, BJT, and diode) have a specific part number defined. What this does is force the SPICE engine to use all default parameters for these devices. For a BJT and diode under generic use, it's usually not that big of a deal. However, with the MOSFET there is a huge problem. The default MOSFET models are for modeling integrated circuit (i.e. "monolithic") MOSFETs. First, they are not suited for modeling discrete VDMOS FETs, due to them having a completely different structure. Second, their default value for the Vto parameter (zero-bias threshold voltage) is set to zero, which is likely where your specific problems are stemming from.

To fix this, right-click on the symbol for the NMOS and then click the Pick New MOSFET button. A list of parts shows up. Since the video you linked shows an IRF1405 stuffed in the breadboard, let's try to find that. Click on the Part No. column header as shown to sort by part number.

enter image description here

Then, we can scroll to find the IRF1405 listed in alphabetical order. We can either double-click the line for IRF1405, or single-click it and then press the OK button to select it.

enter image description here

A good rule of thumb is to always avoid default semiconductor models, not just the MOSFET ones. You do that by always selecting a part number, even if you just need something generic to get the thing rolling. Using parts with non-default parameters can help avoid convergence problems and also model more real-world effects. Whenever I make a simulation using discrete semiconductors which have a non-specialized purpose, I typically select the following built-in LTspice model for each device type:

Silicon PN Diode -> 1N4148
Schottky Diode   -> BAT54
2.0V-ish LED     -> QTLP690C
3.5V-ish LED     -> NSCW100
NPN BJT          -> 2N3904
PNP BJT          -> 2N3906
N-chan JFET      -> 2N3819
P-chan JFET      -> 2N5460
N-chan VDMOS FET -> 2N7002
P-chan VDMOS FET -> BSS84

Therefore, I would also change your NPN transistor to 2N3904 and your silicon diode to 1N4148.


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.