LTspice active load/ current source used and using DC sweep

[House_number]

Hi,

i wonder if anyone can advise please regarding LTspice v 26.0.2

example is a mc34063 in buck configuration 24v to 5v and works great with a resistor load and .step etc.

i’m trying to use a current source and a dc sweep to simulate a load on a power supply to show voltage drop /regulation as the currents get higher.

i’ve tried the current source symbol arrow pointing up and down, tried the ‘This is an active load option’ on and off

Tried on MC30463 and i get a curve but the wrong output voltage? (expecting about 5v for certain currents)

it works if using .step showing separate traces, and the idea works with a zener diode model.

Tried on LT317 Linear power regulator same problem, it cant calculate the output voltage.

is this idea possible with LTspice with MC34063 or LT317?

photo attached shows plot


Thanks in advance
Steve

[ledtester]

Can you attach your .asc file?

Attached is an example using the .DC directive with a LT1587 linear regulator (should be included with LTspice).

It seems to give reasonable results.

[House_number]

Thanks
asc attached
 
mc44063 was the .asy file (changed to .txt to attach) was in the sub folder symbol shape
and
MC34063A was the .lib file (changed to .txt to attach) library

[House_number]

Yes LT1587 works ok good
same
.dc sweep works for ADP7182 (-ve -5v out < 300mA then drops) see photo (with current arrow pointing up
and ‘this is a active load’ was not selected.

but could not get dc sweep to work for LT317 and MC34063? it must be the model files.

[ledtester]

This LT317A simulation seems to work for me.

[House_number]

LT317A as per your setup above works fine.
LT317A using single load of 200mA works fine on my setup includes C1,R1,R2

but
adding the dc sweep (and with  C1 and R2 and R1), results in model error as per attached photo?

[Jay_Diddy_B]

House_number and the group,

You have too many ground connections in this LTspice circuit:



D3 is shorted in the bridge rectifier. You need to remove the ground connection connected to V1.


The DC operating point calculation treats capacitors as open circuits and inductors as short circuits, giving you the steady-state bias voltages and currents.

In this circuit:




The DC operating point is calaculated at time=0. At time equals 0, sine(0) = 0, there is no voltage on any of the nodes in the model.


Changing the model to start with the sine wave at a peak, 90 degrees, SINE(0 17 50 0 0 90), the model starts with the sine wave at a peak.



There is voltage on C1. The voltage is 17V from V1, minus two time the forward voltage drop of the diodes. There is no ripple. The DC analysis is snap shot in time.


This is the wrong type of analysis for this circuit. Use the .step param ... directive to change the load current



Regards,

Jay_Diddy_B

[House_number]

Thanks!
Thats working now.