LTspice giving weird results in simulation of Phase Shifted Full Bridge Converter.

Thread Starter

Darrell_3011

Joined Jun 12, 2021
6
I am trying to simulate a Phase shifted full bridge converter in LTspice. I had already simulated it in matlab simulink and obtained the desired results, but I am redoing it in LTspice to include the effects of non-ideal components. In order to avoid the pulse generation, I imported the switching pulses datapoints from simulink. I have thoroughly checked it and there's no issue with my switching pulses. However, the same circuit in LTspice behaves very weirdly.

This is my model:

1648911503396.png


First of all the current on primary is weirdly high around 3kA, around where as it is 25A in simulink.
1648912156567.png


This is the output DC waveform ( whereas I am expecting stable DC of around 85V as I had obtained in simulink.)

1648912178819.png

I suspect it is an issue with the transformer, but I am not able to pin-point it exactly. Any suggestions are greatly appreciated.

I have attached my .asc file and switching files. Switching files are here: https://drive.google.com/file/d/1tLZM8kkn67f_8aJ7yVGEoM2VJtFOKcpa/view?usp=sharing
 

Attachments

crutschow

Joined Mar 14, 2008
29,800
Do you have a small non-overlap time in the switch timing?

Try grounding one terminal of the the switch control lines and one terminal of V1.
Spice doesn't like floating nodes.
 

Thread Starter

Darrell_3011

Joined Jun 12, 2021
6
Do you have a small non-overlap time in the switch timing?
No, there's no deadtime in the switch pulses. Is that what you meant? The pulses work perfectly alright in MATLAB simulink, its a LTspice specific issue.

Try grounding one terminal of the the switch control lines and one terminal of V1.
Spice doesn't like floating nodes.
Doing that it tells me matrix irregular. And anyway I can have only 1 ground, either on primary or secondary.
 

crutschow

Joined Mar 14, 2008
29,800
The pulses work perfectly alright in MATLAB simulink, its a LTspice specific issue.
MATLAB may not simulate the large cross-through currents.
Add a small amount of deadtime to the LTspice simulation and see if that makes a difference.
I can have only 1 ground, either on primary or secondary.
That may be true in practice, but Spice is problematic with floating components.
You can simulate two grounds by connecting the input circuitry common connection to the output ground through a 10megohm resistor.
 

eetech00

Joined Jun 8, 2013
3,154
There should be dead time (at least 150ns-300ns) between the opposite polarity switches.
The transformer ratio should include a secondary peak output voltage of 85v + the diode bridge voltage drop.
The voltage sources should be grounded.

Yikes!...the stimulation files are gigantic and take quite a while to load.
Better to have a single clock/deadtime generator.
 

Danko

Joined Nov 22, 2017
1,302
I suspect it is an issue with the transformer, but I am not able to pin-point it exactly. Any suggestions are greatly appreciated.
Found error: In TS circuit parallel resistance of L2 is 18mΩ.
Should be something like this:

1648943513104.png
1649038217554.png__ 1649038049077.png
ADDED:
From 4.076 kW consumed by circuit from V1,
2.937 kW dissipated by diodes D1 - D4,
and 1.0675 kW go to load R2.
 

Attachments

Last edited:
Top