Frequency response using SPICE

slackjack said:

I've made a spice netlist of a circuit I am designing. The input to the circuit is an AC signal source --> v1 1 0 dc 0 sin(0 34 60). Well I can do a transient analysis on this easily. But I also want to see what happens at the output as I vary the frequency of the AC signal source. Unfortunately using .AC simply doesnt work (to vary the frequency). I suspect that I defined my signal source incorrectly to be used with .AC.

Click to expand...

Sceadwian said:

Replace the variable in question with {AC}
Not .AC
.AC is the spice directive for AC measurement. If it doesn't have a value with {AC} in it in the circuit it has nothing to vary. From what little I know only voltage/current sources can be asigned {AC} Voltage/frequency/current

Click to expand...

The .AC directive tells the simulator to perform an ac analysis in a frequency interval you have to specify. For example: .AC DEC 101 1 100k for the interval [1Hz, 100kHz].
You need to define an AC source, for example V1 1 0 DC 0 AC 1
By the way, which program are you using? if you get LTSpice from linear.com you can enter those parameters without editing the netlist manually.

Click to expand...

slackjack said:

Thanks for the quick responses guys.


I'm a little comfused when you say "Replace the variable in question with {AC}". Does this mean I have to add an AC component to v1?

I'm using spice opus. So I see that I dont have a source defined with AC. Is there a simple way to fix "v1 1 0 dc 0 sin(0 34 60)" while retaining the initial frequency and amplitude?

Click to expand...

Ron H said:

v1 1 0 sin(0 34 60) AC 1

Click to expand...

Hero999 said:

Watch out for the difference between, peak, peak to peak and RMS voltage. SPICE uses peak voltage, if you want RMS then multiply it by √2, if you want peak to peak then multiply it by 2.

Click to expand...

slackjack said:

Unfortunately, that doesnt work.

Click to expand...

Ron H said:

Did you use the complete .AC directive, as posted by eng1? Otherwise, it won't work.

Click to expand...

PowerSupply

[b]v1 4 5  sin(0 34 60) AC 1[/b]

D1 4 2 1N4007
D2 0 5 1N4007
D3 5 2 1N4007
D4 0 4 1N4007

c1 2 0 1000u
c2 2 0 100n
cout out 0 100n

radj adj 0 5k
r1 out adj 240

x 2 adj out LM317

.include parts.lib
.control
set units=degree
destroy all

tran 0.01ms 100ms
plot v(4,5) v(out)  vs (time*1000)

[b]destroy all

ac dec 10 60Hz 7000Hz
plot ac1.v(out) vs ac1.frequency[/b]

.endc
.end

Ron H said:

If you want to simulate line rejection, get rid of the bridge and replace it with a battery of whatever DC value you want, with an AC source "in series".
v1 2 0 DC 32 AC 1
Run an AC sim (AC dec 100 10 10k).

Or, run a transient sim:
v1 2 0 sin(32 0.5 120).

Click to expand...

v1 2 0 dc 34 ac 1



c1 2 0 1000u 
c2 2 0 100n
cout out 0 10u

radj adj 0 5k
r1 out adj 240  

x 2 adj out LM317

.include parts.lib
.control

destroy all


ac dec 5 10 10k
plot v(out)

.endc
.end