I would like to simulate the switching of this gate drive.

I am not very familiar with the operation of the bootstrap circuit etc. but I would like to do just a couple of simulations at least to verify that the SW output is consistent with what is stated in the datasheet (look to the right in the schematic image the "table" taken from the datasheet).



The problem is the too small timestep on node nn3 (i.e. HS pin)
I have tried varying/removing each individual component but the problem persists.
I have also tried varying these parameters, but it does not work:


I have attached the simulation and the library from which I auto-generated the gate driver.

 

Hi k89,
Please post the LMG model file.
E

 

Hi k89,
Please post the LMG model file.
E

I don't know what the LMG file is and where it is, but I have lmg5200.lib inside LTSpice and I generated the component from from ".subckt LMG5200_TRANS HB HI HS LI PGND AGND VCC VIN SW params: del_match=2n"

Where is the LMG file located?

 

hi k,
When I run the asc file I get this, ref image.

Requires the asy file.
E

 

hi k,
When I run the asc file I get this, ref image.

Requires the asy file.
E

 

hi @kalemaxon89
Try this, note the .options
E

 

hi k,
Try this, note the .options
E
View attachment 332923

hi @kalemaxon89
Try this, note the .options
E
View attachment 332923

It works! Thank you so much for your help
I just found all those options in the ltspice help.
Basically:
- increased cshunt (capacitance) from 0. to 10f
- increased gshunt (conductance) from 0. to 1n
- increased abstol (tolerance) from 1pA to 1n
- increased vntol (tolerance) from 1u to 1m
- nomarch: don't plot marching waveform .. what does it mean?

 

Hi k,
Check this link.
E
https://www.google.com/search?client=firefox-b-d&q=LTSpice+Nomarch

https://ltwiki.org/LTspiceHelp/LTspiceHelp/_OPTIONS_Set_simulator_options.htm

 

Hi @kalemaxon89
The easy way to show the effect of no march.
Change the .tran to say 200uSec, run the sim, note the waveform plot is slightly delayed, but when it appears it will be the complete waveform from 0uS to 200uS.

Delete the no march word from the options list.
Run the sim, you will see the plot waveform being generated slowly step by step from 0uS to 200uSec
The sim will take a little longer to run.

E

 

Hi @kalemaxon89
The easy way to show the effect of no march.
Change the .tran to say 200uSec, run the sim, note the waveform plot is slightly delayed, but when it appears it will be the complete waveform from 0uS to 200uS.

Delete the no march word from the options list.
Run the sim, you will see the plot waveform being generated slowly step by step from 0uS to 200uSec
The sim will take a little longer to run.

E

Thanks!
However, I do not understand why this "disturbance" on feeding occurs:


I varied the output (using L and R as a motor load)

 

Hi K.
This is what I see.
E

 

Hi K.
This is what I see.
E
View attachment 332964

I see those spikes but we have the same circuit.
What could it be due to?
Some spice setting?

 

Hi K.
This is what I see.
E
View attachment 332964

This is from 0 to 80us:

 

Hi,
The two inputs are overlapping, this will cause a high current spike.
E

 

Hi,
The two inputs are overlapping, this will cause a high current spike.
E
View attachment 332968

I eliminated in the two pwm generators the delay time and set to 1pF rise and fall times. It is a little better. The duration of the input current spikes is "only" 35ns, I don't think it will affect the average value.