Hello guys! I'm using LT8705 to make a battery charger to charge my 6s NCM battery pack. But It seems that the LT8705 don't have the reverse current protection and will start in CV mode and then into CC mode thus presenting a high current before getting into CC mode. So I'm trying to use LT4364 to solve these two problems, Which are preventing reverse current and high forward current that appears during startup.
The model below is my LTspice project. It will always stuck at around 4ms when doing transient analysis, so I can't get any information. Can anybody tell the reasons? By the way, can the second problem which is a high current causing by CV mode be solved theoretically?

 

hi lian
Add a 10uSec step in .tran
Also, what is the purpose of the 12v voltage source load, with a 1mOhm Rser.?
I also tried a 100R in place of that voltage source.

The simulation takes a long time to run, time for a coffee or saki.
E

 

hi lian
Add a 10uSec step in .tran
Also, what is the purpose of the 12v voltage source load, with a 1mOhm Rser.?
I also tried a 100R in place of that voltage source.

The simulation takes a long time to run, time for a coffee or saki.
E
View attachment 291410

Thank you for the reply! The reason why I set a voltage source as load is that I used this voltage source as 6series battery pack, as I found that the "battery module" in LTspice is a voltage source. And I have tested my pack which has a 1mohm impedance. My 6s battery's minimum voltage is 18 volts, 12V is wrong, sorry.
If I don't use the LT4364, I can charge my "battery" without any big faults as I showed below. I just want to add the reverse protection feature to my circuit to prevent the misoperation during connecting the batteries. And control the charge current as a function of Battery Management by the way.
However, when I put the voltage source load back and 10uSec in .tran and then run the project, it will still stuck at 4.1ms.
The bigger question is, when I try to put my voltage soure in reverse in the LT4364 demo circuit to test the reverse protection fuction, it works very well. But when I try this method in the LT8705+LT4364 circuit, it seems to be compeletly wrong and the big reverse current always exist. I just can't figure out.

 

hi lian,
Your original asc file, a 10uSec step, runs OK for me, but takes some time to run.
E

Update:
This is your circuit with the 18v, V2 voltage source reversed, the plot shows no high reverse current.?

E

 

Below is the sim, which did not stop.
I added a 1 ohm series resistance in the output V1 to eliminate some oscillations after the output current came up.




Below is the reverse output bias simulation.
I did see a high reverse current in my first simulation, but none when I delayed the application of the reverse voltage by 1.8ms until after U1's voltage came up.

 

hi lian,
Your original asc file, a 10uSec step, runs OK for me, but takes some time to run.
E

Update:
This is your circuit with the 18v, V2 voltage source reversed, the plot shows no high reverse current.?

E
View attachment 291507

Thank you for the reply! When I try to run the project as you mentioned, it says there's an error
I have checked the circuit, it seems to be the same. Could you tell me if you have changed any simulate settings in LTSpice? I suspect I have to change some of my settings in the software, as I stay all the settings default at the moment.

 

Below is the sim, which did not stop.
I added a 1 ohm series resistance in the output V1 to eliminate some oscillations after the output current came up.

View attachment 291518


Below is the reverse output bias simulation.
I did see a high reverse current in my first simulation, but none when I delayed the application of the reverse voltage by 1.8ms until after U1's voltage came up.

View attachment 291517

Below is the sim, which did not stop.
I added a 1 ohm series resistance in the output V1 to eliminate some oscillations after the output current came up.

View attachment 291518


Below is the reverse output bias simulation.
I did see a high reverse current in my first simulation, but none when I delayed the application of the reverse voltage by 1.8ms until after U1's voltage came up.

View attachment 291517

Thank you for changing these circuits and giving all the results! By adding the delay, I can run the project successfully and present the same result as yours, which is no reverse current.
However, in the original sim as you provided with a 1 ohm series resistance in the output V1. I didn't see the series resistance in your picture? I have added this resistance and try to run, an hour has gone, it still stuck.

Anyway, your results shows that this circuit seems to be promising and works well. Maybe I have to figure out some settings I need to change, as I want to see the same results in my computer finally.
View attachment 291542

 

This is the project.

 

you provided with a 1 ohm series resistance in the output V1. I didn't see the series resistance in your picture?

My mistake.
It's part of the V2 source, not V1.

 

My mistake.
It's part of the V2 source, not V1.

View attachment 291545

It works! It seems that the LTSpice don't like the minor values components such as nano-ohms or milliohms resistors.
Thank you very much!

 

It seems that the LTSpice don't like the minor values components such as nano-ohms or milliohms resistors.

It's not LTspice per se, but that its voltage source is ideal with no resistance.
This may affect the circuit stability (even the real circuit, as it may not be designed to be stable with a zero resistance load).
A real battery would always have some finite (albeit small) resistance.