how to simulate schematic

[samoloko]

Hi

I have found interesting discrete voltage regulators Discrete Voltage Regulator - John Swenson - Computer Audio Asylum and would like to view how they are simulated
I have draw schematic but don't know what to do to get simulated results like noise vs freq and output impedance vs freq

[Oliphant]

Draw this circuit in any spice simulator. There are many free ones available such as Tina-TI or LTspice. Circuitmaker 2000 is also very good for this sort of thing.

[samoloko]

It Is drawn In LTSpice but when I run simulation I got error logs
have you seen attachment

[Elvee]

Originally Posted by samoloko

have you seen attachment

Why do you zip your files? It is a PIA, and with the new forum capabilities, you have no excuse to stick to it.

[jcx]

I1 is at least 10x too high

do a .TRAN type analysis for debugging a Spice sim - save the .NOISE for after the .TRAN shows proper cirucit operation

you can cruise the schematic following a successful .TRAN with the cursor and the DC operating point I, V will be displayed in the lower left corner as the cursor moves over wires, device terminals

[samoloko]

I have corrected I1 to 0,005A and also output cap to 100uF and program run simulating output voltage at 5V but I would like to know what settings to set to get noise of regulator and output impedance

[euro21]

Proper Noise syntact:
.noise V(out) V1 oct 5 2 25000

[samoloko]

thank you euro21

would you please tell me how can I view output impedance vs freq

regards

[euro21]

Originally Posted by samoloko

would you please tell me how can I view output impedance vs freq

Add signal generator to output. Signal AC=1V.
Run 'AC Analysis'. 1Hz-1MHz, 10 point/octave.
Click on 'out' node.
Edit 'AC Analysis' window title -right mouse click on title- (now V(out) ) to V(out)/I(V2).
Change 'AC Analysis' window left (vertical) menu (now decibel) -left mouse click- to 'Linear'. Thereafter it is Ohm.

[jcx]

a Current Source is more commonly used for testing Voltage Output node impedance - like the Output of Voltage Regulator circuit

and the I1 bais current is still totally unrealisitic - the LED would be a DED at 1/4 A

the .Noise and .AC analysis can be misleading - they only operate on the small signal linearized model derived from the DC operating point analysis on start up

they don't show any nonlinear, saturation, reverse bias conditions that your test signals could cause in a "real sim"

really the only "safe" way to use the .AC based sims is after you have tested with .TRAN, simmed with realistic load, test sources with sine, or pulse/ramp waveforms