I have simulated the LM723 based regulator circuit in LTSpice
And after running it I got 16A currents (blue/green) on diodes in rectifier. The max current I supposed to get here was 3.3A. Please tell me what is wrong? I have tried to use different MUR860 models and it did not helped.
There are a few problems with this schematic
1) You are using an ideal voltage source, You may want to add some inductance and resistance to simulate wires. Mains power is not infinite, and neither is the current from a transformer. Your transformer is going to have a lag on power that it can deliver, you should probably simulate this. Another thing to watch out for is transformer saturation. (unless your not getting power from AC mains)
2) As the other answers say, you have a huge capacitor, is throwing more capacitance at the problem going to be a good solution? If the current is too high, then you need to change the design, not the parameters of the design. At these current levels you should probably use a DC to DC instead of a vreg unless price is an important consideration. You are going to burn up lots of power. Its better to put smaller amounts of current at a higher voltage through the rectifier You can get cheap DC to DC regulators that are 780X drop in compatible that will handle 1 amp, you can parallel them if you need more current. If that doesn't work then go find a DC to DC IC. Have you considered a AC to DC power supply such as a "wall wart"? People make these things for less than 20$.
It looks like you're trying to provide about 15 V to a 6 ohm load. Unless I misunderstand your schematic... So that's 2.5 A.
Now consider that the diodes only turn on and pull current from the AC source about 1/5 of the time (only when the 23 V sin goes above the 20 V or whatever rectified voltage you're getting).
In order to average 2.5 A (plus whatever is sloshed in the the parallel caps) at 20% duty, you'll need to average about 12.5 A during that 20% of the time. So, a max of 16 A doesn't seem unreasonable to me.
Add some series resistance to that 10mF capacitor.
Add some series resistance to the voltage source. In the real world that voltage source will be a transformer and it's secondary winding will have some series resistance.
I'm assuming you're using proper models for the diodes so they should already have some series resistance.
Think about what will limit that current in the real world: the series resistances of all the components through which that current flows. In a simulator it is easy to get 10 kA of current, in the real world it is not that easy.
I'm, not sure about the modeling but I've used the 723 a lot and found that if you've got the voltage headroom it's good to have a few transistors in Darlington configuration between the 723's Vout and the base of the final pass transistor. If you look at the schematic of the 723 you'll see that there's already one inside the chip, just add a couple more. It improves the active filtering and the regulation. I built a 12 volt 8 amp power supply once and I was able to get the load regulation to better than 1 mv full load to no load using about 3 driver transistors. Think current gain.
Could be a problem with the spice model you're using too, I stumbled on this trying to find a spice model for a 723.
