Re: frequency response


"DDDiiD" <linuxfreak87@xxxxxxxxx> schrieb im Newsbeitrag
news:1179259959.208298.232300@xxxxxxxxxxxxxxxxxxxxxxxxxxxxxx

Hello,

I tried a transient analysis of your netlist with LTspice and it worked
in
principle
but there is a small oscillation at the output. The value of Cout is
undersized.
Just increase its value to 10u and you will be saved.

Thanks for the suggestion.

How can you run any .AC-analysis without any source having AC specified?
It's impossible. Please explain where your AC is specified.
AC-analysis is a linear system analysis in SPICE!
It has nothing to do with the AC-voltage applied to your rectifier
diodes.
Where do you want to apply the AC-voltage or current?

I thought having "v1 4 5 dc 0 sin(0 34 60)" would allow me to do an ac
analysis because its an ac source. But from your reply, I see that
this is not the case. The applied ac voltage should be applied to the
rectifier as v1 is now. What changes should I make to the v1 to allow
me to perform this ac analysis, while retaining my peak value of 34v
and frequency of 60Hz.

Hello,

I still think you expect something different from the .AC simulation.
The .AC simulation could be used to measure the small signal input
"noise" rejection of the regulator versus frequency or it could be
used to measure the dynamic output resistance of your regulator.
All these .AC simulations will require to setup the appropriated
DC condition for the LM317. This means you would apply a DC
voltage of e.g. 32V at the input with an additional AC definition.
It would be also necessary to add the correct load device,
e,g, a resistor load or a current source load.

The normal 60Hz ripple rejection has to be simulated with .TRAN
because this is a really nonlinear system.

Best regards,
Helmut

PS: Nobody can exactly reproduce your circuit wihout knowing your LM317
model.

I'm using the following model:
http://www.industrycommunity.com/myforum/moazzam_mahmood_next1/messages/48.html

Thanks again.



.