real noise plots in SPICE?

"Helmut Sennewald" <HelmutSennewald@t-online.de> wrote in message
news:d2meq6$i20$05$1@news.t-online.com...

Example:
--------

This is the error message which you will get if you have written
.noise out v2 oct 100 100 1k

instead of the correct
.noise V(out) v2 oct 100 100 1k


Circuit: * F:\Programme\Ltc\SwCADIII\examples\Educational\noise.asc

Error on line 67 : .noise out v2 oct 100 100 1k
bad syntax [.noise v(OUT) SRC {DEC OCT LIN} NP FSTART FSTOP
PTSPRSUM>]
Fatal Error: .NOISE syntax error


Best Regards,
Helmut

To all:
The .NOISE analysis correctly works in LTspice.
A user should ask himself why it doesn't work as expected.
Click to expand...
Thanks for taking the time over this one.

I just spotted it.

I've been writing

..noise V(out) V(vset) dec 20 1 100K

Where V(vset) references an output port, called VSET
connected to a voltage source, called V3.

That messes up the analysis and corrupts the data in
the noise dialog tab. I should be writing.

..noise V(out) V3 dec 20 1 100K

whoops

DNA


DNA
 
On Sun, 03 Apr 2005 00:21:17 -0800, qrk <SpamTrap@reson.com> wrote:

Helmut, you have amazing patience! I think we should nominate you as
mentor of the decade!

Aloha, Mark
Click to expand...
Seconded ;-)

...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.
 
If you want to see the 1/f the model has to have it. Very few models
do. I do mine like that, all of my models allow you to see the 1/f
given that you plot the noise on log log scale of course
 
first of all you have to "enable" the noise analysis of your simulator,
then simply put a voltage marker at the output of your buffer (while
it's grounded) and look at the input referred noise by simply using the
insert on your keyboard. Make sure you use the log log scale and bingo,
you should have your noise including the 1/f. As I said very few models
have that so don't expect to see it match the datasheet it ain't there.
if you want a good one to use as a guidance take a look at the OP27 or
AD8616 spice models.
 
Yes noise will vary with current but in this case it shouldn't if
you're running a constant Vsy and not sweeping any sort of DC.
But i don't know anything about LTspice I just know Pspice or Orcad
from cadence I guess.
 
Helmut Sennewald wrote:

"Genome" <ilike_spam@yahoo.co.uk> schrieb im Newsbeitrag
news:8Nv3e.3240$vv2.1350@newsfe2-gui.ntli.net...

"Helmut Sennewald" <helmutsennewald@t-online.de> wrote in message
news:d2lp8h$lta$01$1@news.t-online.com...

Hello Robert,
your .noise command controls the input source.

Example in LTspice: The voltage source V1 is the input source.
.noise V(out1) V1 dec 100 1 1MEG

From your netlist: V2 is used as input source which is wrong
if you want simulate a voltage follower in your circuit.


.AC oct 8 0.1 10K
.noise V(P002) V2

Best Regards,
Helmut



It may be that my install has got corrupted but when I try to
edit the simulation card for noise silly things go on and the
entered data gets corrupted.

Before

Output V(vout)
Input V(vset)
Type decade
N.points 20
Start F 1
Stop F 100K

After

Output V(vout)
Input V
Type octave
N.points dec
Start F 20
Stop F 1

Gives Error 'Missing number of points per octave'

DNA


Hello Genome,
there seems to be a different syntax between the SPICE programs.


LTspice:
.noise V(out1) V1 dec 100 1 1MEG

Other SPICE programs may require two lines:
.noise V(out1) V1
.ac dec 100 1 1MEG

Best Regards,
Helmut




True; does not address the problem, which appears to be a bug.
Click to expand...
 
Genome wrote:

"Helmut Sennewald" <helmutsennewald@t-online.de> wrote in message
news:d2m55g$ksc$02$1@news.t-online.com...

"Genome" <ilike_spam@yahoo.co.uk> schrieb im Newsbeitrag
news:8Nv3e.3240$vv2.1350@newsfe2-gui.ntli.net...

"Helmut Sennewald" <helmutsennewald@t-online.de> wrote in message
news:d2lp8h$lta$01$1@news.t-online.com...

Hello Robert,
your .noise command controls the input source.

Example in LTspice: The voltage source V1 is the input source.
.noise V(out1) V1 dec 100 1 1MEG

From your netlist: V2 is used as input source which is wrong
if you want simulate a voltage follower in your circuit.


.AC oct 8 0.1 10K
.noise V(P002) V2

Best Regards,
Helmut



It may be that my install has got corrupted but when I try to
edit the simulation card for noise silly things go on and the
entered data gets corrupted.

Before

Output V(vout)
Input V(vset)
Type decade
N.points 20
Start F 1
Stop F 100K

After

Output V(vout)
Input V
Type octave
N.points dec
Start F 20
Stop F 1

Gives Error 'Missing number of points per octave'

DNA

Hello Genome,
there seems to be a different syntax between the SPICE programs.


LTspice:
.noise V(out1) V1 dec 100 1 1MEG

Other SPICE programs may require two lines:
.noise V(out1) V1
.ac dec 100 1 1MEG

Best Regards,
Helmut






I am running LTspice.

If I click on Simulate, Edit Simulation Cmd and then click
on the Noise tab then when I set up the analysis and click
on OK the data gets corrupted and the error message is
generated.

If I explicitly place a spice directive on the circuit in
the correct format then when I run the simulation it comes
up with the same error. The spice directive remains correct
but the data in the Noise tab gets corrupted.

I did do a web update but the problem remains.

HTH

DNA


Yes, i have seen the corruption created when one wants to change
Click to expand...
inoise or onoise specifications.
It happens every time.
Just manually correct the last 3 lines, click OK on the pop-up and
the noise card should follow what you entered.
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top