Searching \ for '[EE] LTSPICE plot variables' in subject line. ()
Make payments with PayPal - it's fast, free and secure! Help us get a faster server
FAQ page: www.piclist.com/techref/microchip/ios.htm?key=spi
Search entire site for: 'LTSPICE plot variables'.

Exact match. Not showing close matches.
PICList Thread
'[EE] LTSPICE plot variables'
2012\06\05@231923 by V G

picon face
I searched the entire documentation and more but couldn't find what I'm
looking for.

How does one include schematic variables or values in plot calculations?
For example, I'm trying to plot reactance via R = 1/2*pi*frequency*C via a
small signal AC analysis. I guessed that the plot variable for frequency
would be "frequency", but I have no idea how to refer to the value for my
capacitor. For example, getting the V or I can be done with V(n001) or
I(R1) or something like that

2012\06\06@063733 by Oli Glaser

flavicon
face
On Wed, Jun 6, 2012 at 4:19 AM, V G <spam_OUTx.solarwind.xTakeThisOuTspamgmail.com> wrote:

> I searched the entire documentation and more but couldn't find what I'm
> looking for.
>
> How does one include schematic variables or values in plot calculations?
> For example, I'm trying to plot reactance via R = 1/2*pi*frequency*C via a
> small signal AC analysis. I guessed that the plot variable for frequency
> would be "frequency", but I have no idea how to refer to the value for my
> capacitor. For example, getting the V or I can be done with V(n001) or
> I(R1) or something like that.
>

2012\06\07@044959 by V G

picon face
On Wed, Jun 6, 2012 at 6:37 AM, Oli Glaser <.....oli.glaserKILLspamspam@spam@talktalk.net> wrote:

> If I understand what you are asking for:
>
> 1. Run the simulation.
> 2. Right click the graph and select "add trace".
> 3. In the box add the V/I of the relevant component - e.g. something like
> V(n001)/I(C1)
> 3. Press OK and it should plot in Ohms - to view real and imaginary parts
> left click on the y axis values (cursor changes to a ruler) and select
> "cartesian" in the drop down box (default is "bode", or nyquist is the
> other option)
>
> Hope this helps..
>

I tried all that, everything I could think of, before posting. This is what
LTSPICE is showing me for the calculated impedance graph (red) and I don't
really know why. If I punch those numbers (the red graph's equation) into a
calculator, I get expected values for the capacitor's impedance. But for
some reason, the graph looks really strange with really odd values in
LTSPICE. The green and blue graphs look fine though.

Screenshot: http://i.imgur.com/hQXwn.pn

2012\06\07@121402 by Dwayne Reid

flavicon
face
Really dumb thought - Bob Pease says that someone he knows (worked with?) said to use 50.1 Ohms instead of just 50 Ohms - somehow, that got rid of weirdness.

Might it apply to your situation - I really don't know.  But that little tidbit of info got tucked into my brain when I read it and I'm just passing it on.

dwayne


At 02:49 AM 6/7/2012, V G wrote:
>  This is what
>LTSPICE is showing me for the calculated impedance graph (red) and I don't
>really know why. If I punch those numbers (the red graph's equation) into a
>calculator, I get expected values for the capacitor's impedance. But for
>some reason, the graph looks really strange with really odd values in
>LTSPICE. The green and blue graphs look fine though.
>
>Screenshot: http://i.imgur.com/hQXwn.png


-- Dwayne Reid   <dwaynerspamKILLspamplanet.eon.net>
Trinity Electronics Systems Ltd    Edmonton, AB, CANADA
(780) 489-3199 voice          (780) 487-6397 fax
http://www.trinity-electronics.com
Custom Electronics Design and Manufacturing

2012\06\07@122025 by Oli Glaser
flavicon
face
On Thu, Jun 7, 2012 at 9:49 AM, V G <.....x.solarwind.xKILLspamspam.....gmail.com> wrote:

{Quote hidden}

I just tried that circuit and it works fine for me. Only thing I can think
of is that you are trying to plot just the real component of C1, which will
be 0 if you have not set the ESR of C1 to a realistic value (say 100mOhm or
whatever).
So this means you probably have "don't plot imaginary component" set. If
you left click on the right side axis and press ok you should get the
imaginary component plotted (the axis should show e.g. 10KiOhm, 20KiOhm,
etc, with the i being for imaginary) which should be what you expect.
Let me know how it goes..

2012\06\07@131920 by Joe Wronski

flavicon
face
Just wondering whether that's just using familiar speech patterns or did you not realize that Bob Pease died, just about 1 year ago, June 18.
http://www.ti.com/ww/en/bobpease/index.html

Joe W


On 6/7/2012 12:14 PM, Dwayne Reid wrote:
{Quote hidden}

>

2012\06\07@154215 by Dwayne Reid

flavicon
face
At 11:23 AM 6/7/2012, Joe Wronski wrote:
>Just wondering whether that's just using familiar speech patterns

Yep

>or did you not realize that Bob Pease died, just about 1 year ago, June 18..
>http://www.ti.com/ww/en/bobpease/index.html

Yeah - he died about a week after we lost one of my other heros - Jim Williams.  It was a bad week for the electronics community.

Bob Pease *hated* SPICE because, he said, that it always lied to him.  But he did recognize that many people do actually get good results from it and he passed on that tip.  I have NO idea if it applies to LTspice.

dwayne


{Quote hidden}

2012\06\10@210532 by V G

picon face
On Thu, Jun 7, 2012 at 12:20 PM, Oli Glaser <oli.glaserspamspam_OUTtalktalk.net> wrote:

>  I just tried that circuit and it works fine for me. Only thing I can
> think
> of is that you are trying to plot just the real component of C1, which will
> be 0 if you have not set the ESR of C1 to a realistic value (say 100mOhm or
> whatever).
> So this means you probably have "don't plot imaginary component" set. If
> you left click on the right side axis and press ok you should get the
> imaginary component plotted (the axis should show e.g. 10KiOhm, 20KiOhm,
> etc, with the i being for imaginary) which should be what you expect.
> Let me know how it goes...
>

I'm still getting a strange graph output. Can you please send me your
LTspice circuit file and plot settings file? I want to see if there's
something I'm missing

2012\06\11@005835 by Oli Glaser

flavicon
face
part 1 1256 bytes content-type:text/plain; charset="iso-8859-1" (decoded quoted-printable)

On Mon, Jun 11, 2012 at 2:05 AM, V G <@spam@x.solarwind.xKILLspamspamgmail.com> wrote:

{Quote hidden}

Okay, here's the files. I started the sweep from 1kHz to make the imaginary
(dotted) curve more obvious. The 1mOhm real part is just the cap ESR.


part 2 678 bytes content-type:text/plain; name="VG.asc"
(decoded base64)

Version 4
SHEET 1 880 680
WIRE -448 96 -496 96
WIRE -144 96 -384 96
WIRE -496 176 -496 96
WIRE -144 176 -144 96
WIRE -496 320 -496 256
WIRE -144 320 -144 256
WIRE -144 320 -496 320
FLAG -144 320 0
FLAG -144 96 Vout
SYMBOL voltage -496 160 R0
WINDOW 123 24 124 Left 2
WINDOW 39 -147 33 Left 2
SYMATTR Value2 AC 1
SYMATTR SpiceLine Rser=0
SYMATTR InstName V1
SYMATTR Value 5
SYMBOL res -160 160 R0
SYMATTR InstName R1
SYMATTR Value 50
SYMBOL cap -384 80 R90
WINDOW 0 0 32 VBottom 2
WINDOW 3 32 32 VTop 2
SYMATTR InstName C1
SYMATTR Value 1F
SYMATTR SpiceLine Rser=1m
TEXT -856 32 Left 2 !.ac lin 100000 1000 100e3

part 3 401 bytes content-type:application/octet-stream; name="VG.log" (decode)

part 4 224 bytes content-type:application/octet-stream; name="VG.net" (decode)

part 5 354 bytes content-type:application/octet-stream; name="VG.plt" (decode)

part 6 181 bytes content-type:text/plain; name="ATT00001.txt" (decode)

2012\06\16@102225 by V G

picon face
On Mon, Jun 11, 2012 at 12:58 AM, Oli Glaser <RemoveMEoli.glaserTakeThisOuTspamtalktalk.net>wrote:

> Okay, here's the files. I started the sweep from 1kHz to make the imaginary
> (dotted) curve more obvious. The 1mOhm real part is just the cap ESR.
>

Thanks a lot! That worked! I don't understand where the imaginary part is
coming from though (what law/equation, etc...)

2012\06\16@113128 by V G

picon face
On Sat, Jun 16, 2012 at 10:22 AM, V G <spamBeGonex.solarwind.xspamBeGonespamgmail.com> wrote:

> On Mon, Jun 11, 2012 at 12:58 AM, Oli Glaser <TakeThisOuToli.glaserEraseMEspamspam_OUTtalktalk.net>wrote:
>
>> Okay, here's the files. I started the sweep from 1kHz to make the
>> imaginary
>> (dotted) curve more obvious. The 1mOhm real part is just the cap ESR.
>>
>
> Thanks a lot! That worked! I don't understand where the imaginary part is
> coming from though (what law/equation, etc...).
>

Oh I think I can guess... Is it because of the two solutions to the
equation involving a square root (for calculation of the RMS voltage at the
two nodes)

2012\06\17@214248 by Oli Glaser

flavicon
face
On Sat, Jun 16, 2012 at 4:31 PM, V G <RemoveMEx.solarwind.xspamTakeThisOuTgmail.com> wrote:

> On Sat, Jun 16, 2012 at 10:22 AM, V G <x.solarwind.xEraseMEspam.....gmail.com> wrote:
>
> > On Mon, Jun 11, 2012 at 12:58 AM, Oli Glaser <EraseMEoli.glaserspamtalktalk.net
> >wrote:
> >
> >> Okay, here's the files. I started the sweep from 1kHz to make the
> >> imaginary
> >> (dotted) curve more obvious. The 1mOhm real part is just the cap ESR.
> >>
> >
> > Thanks a lot! That worked! I don't understand where the imaginary part is
> > coming from though (what law/equation, etc...).
> >
>
> Oh I think I can guess... Is it because of the two solutions to the
> equation involving a square root (for calculation of the RMS voltage at the
> two nodes)?
>
>
I think you are on the right track. The imaginary part is simply 1/2pi * F
* C. To work out the overall impedance you take the square root of the
(squared) imaginary and real impedances. So if you have 50 ohms imaginary
and 50 ohms real you have a total impedance of sqrt(50^2 + 50^2) = 70.7
ohms.
You can check this in the simulation if you plot V(n001)/I(C1) and look at
the bode and cartesian displays. 1uF is 50 ohms around 3.18 kHz. At this
frequency on the bode you should read 70.7 ohms on the plot, if you change
to the cartesian you should see both real and imaginary at 50 ohms

More... (looser matching)
- Last day of these posts
- In 2012 , 2013 only
- Today
- New search...