frequency response

R

ranger

Guest
I'm trying to plot the frequency of a power supply I've designed. Here
is the net list:

PowerSupply

v1 4 5 dc 0 sin(0 34 60)

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)

destroy all

ac dec 10 60Hz 7000Hz
plot ac1.v(out) vs ac1.frequency

..endc
..end
--------------------------------------------------------------

I'm not doing it correctly though. For the second plot (freq
response), I get values in excess of 6000V ! This is so wrong as my
calculations have shown just above 28V is possible.
Please assist me in doing a frequency response.

Thanks.
 
"ranger" <linuxfreak87@gmail.com> schrieb im Newsbeitrag
news:1179195349.937021.53950@y80g2000hsf.googlegroups.com...
I'm trying to plot the frequency of a power supply I've designed. Here
is the net list:

PowerSupply

v1 4 5 dc 0 sin(0 34 60)

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)

destroy all

ac dec 10 60Hz 7000Hz
plot ac1.v(out) vs ac1.frequency

.endc
.end
--------------------------------------------------------------

I'm not doing it correctly though.
Click to expand...
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.

For the second plot (freq
response), I get values in excess of 6000V ! This is so wrong as my
calculations have shown just above 28V is possible.
Please assist me in doing a frequency response.
Click to expand...
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?

Best regards,
Helmut

PS: Nobody can exactly reproduce your circuit wihout knowing your LM317
model.
 
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.
Click to expand...
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?
Click to expand...
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.


PS: Nobody can exactly reproduce your circuit wihout knowing your LM317
model.
Click to expand...
I'm using the following model:
http://www.industrycommunity.com/myforum/moazzam_mahmood_next1/messages/48.html

Thanks again.
 
"DDDiiD" <linuxfreak87@gmail.com> schrieb im Newsbeitrag
news:1179259959.208298.232300@h2g2000hsg.googlegroups.com...
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.
Click to expand...
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.
Click to expand...
 
"Helmut Sennewald" <helmutsennewald@t-online.de> schrieb im Newsbeitrag
news:f2d6up$pdc$00$1@news.t-online.com...
"DDDiiD" <linuxfreak87@gmail.com> schrieb im Newsbeitrag
news:1179259959.208298.232300@h2g2000hsg.googlegroups.com...

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.
Click to expand...
Sorry, it should be DC 34V in your cicuit.

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.
Click to expand...
 
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.
Click to expand...
I'm not sure I quite understand this. I am suppose to change "v1 4 5
dc 0 sin(0 34 60)" to "v1 4 5 dc 34 sin(0 34 60)" thereby giving it a
dc defintion?
 
"ranger" <linuxfreak87@gmail.com> schrieb im Newsbeitrag
news:1179282739.617971.151040@p77g2000hsh.googlegroups.com...
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.

I'm not sure I quite understand this. I am suppose to change "v1 4 5
dc 0 sin(0 34 60)" to "v1 4 5 dc 34 sin(0 34 60)" thereby giving it a
dc defintion?
Click to expand...
Hello,

A possible Spice-line could be as shown below.

V1 1 0 DC 38 AC 1

Overall I rate an AC-simulation useless at this point in the
circuit, because your diode bridge is acting like a switch
which conducts only for a fraction of each period.

Who the hell told you to do a .AC-simulation at this point
in the circuit and for what reason?

Best regards,
Helmut
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top