Full wave rectifier equivalent AC load

[SK245230]

Hi Edaboard community, I have a quick question about rectifiers.
It seems that when you run an AC simulation with a rectifier, the rectifier behaves like if there is nothing.
Below I show what i'm talking about. I simulate an AC source with a 5 ohm resistor (R1) and same resistor (R2) with a rectifier.

The current that goes in R1 is 200mA and the current that goes in R2 is 0. This is logic because there is no AC current that goes through R2, it is DC current.
But I have some troubles here with the AC source. In time based world, the source gives AC power to the rectified load, but when you run AC simulation with rectifier, the source gives nothing. This is disturbing for me.
AC simulation:
I(V2)= 0mA (AC)

Transient simulation:
I(V2)= 60mA (AC)

However, one question arrise. how can you run AC simulation with rectifiers so that the source behaves like it should. Is there maybe a kind of equivalent circuit or model for the rectifier?
How do you run AC simulation with rectifiers?
I'm asking this because I am working with AC to DC applications and I can't find a way to have a rectified load that behaves correctly in AC simulation.

 

[KlausST]

Hi,

If you go through existing "rectifier simulation" discussions....almost always there is a (known) issue:
During low input voltage the output voltage is indetermined, because all diodes are high impedance. This means the simulator is not able to find the operating point. Usually this leads to a simulation error.

Workaround:
To avoid this situation one simply has to connect one output node with one input node via a high impedance resistor.
Often one uses 1GOhms to GND.

Try this and check behaviour.

Klaus

 

[pancho_hideboo]

Use small signal analysis subjected to master large signal periodic steady state analysis.
https://www.edaboard.com/showthread.php?169169#7

 

[FvM]

You need to understand the nature of .AC analysis, which is always small signal. It analysis the circuit in it's operation point, in this case the rectifiers with zero DC voltage bias. Respectively you see only a bit of junction capacitance for it.

LTspice has no advanced analysis modes like periodic steady state or harmonic balance, you need to use transient analysis with a sine voltage source.

 

[vivekroy]

AC simulation is a small signal simulation. It assumes that initially everything is DC and then your actual stimulus, which is your AC source here, is a small variation on top of it.
Every circuit simulator does the following steps to do an AC simulation:
#1 --> It finds the DC operating point. It disregards any AC or transient sources in the circuit and finds the DC operating point.
#2 --> It linearizes the circuit about that point. I/P and O/P relationship of every circuit element is represented as a linear relationship (Frequency dependent effects can be taken into account here but ignore it for this discussion)
#3 --> For each of the frequency point, it solves the value of the transfer function from your I/P source to every node and current in the circuit.

The reason why AC is not going to work for this circuit is because your DC operating point is broken. And there is really no way to fix it because the circuit relies on the non-linear operation of diodes for it to rectify.
I strongly recommend using transient analysis.