Google Groups no longer supports new Usenet posts or subscriptions. Historical content remains viewable.
Dismiss

LTSpice plot voltage vs step param

2,315 views
Skip to first unread message

Marco Trapanese

unread,
Jan 23, 2013, 3:33:40 AM1/23/13
to
Hello,

I can't figure out how to plot a voltage versus a step parameter.
I defined:

.step param R 100 150

but now I don't know what's the right simulation directive.
I tried the tran command, and it actually plots several curves for each
step. They are super-imposed of course.
Instead the goal is to put my {R} variable into the horizontal axis -
changing the plotted quantity field leads to error (undefined symbol).

I searched in the help without find anything useful.
Thanks in advance
Marco

Jim Thompson

unread,
Jan 23, 2013, 9:52:29 AM1/23/13
to
In PSpice, it would be done in a .DC analysis. I think it's the same
in LTspice.

...Jim Thompson
--
| James E.Thompson, CTO | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona 85048 Skype: Contacts Only | |
| Voice:(480)460-2350 Fax: Available upon request | Brass Rat |
| E-mail Icon at http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.

Marco Trapanese

unread,
Jan 23, 2013, 10:22:37 AM1/23/13
to
Il 23/01/2013 15:52, Jim Thompson ha scritto:

> In PSpice, it would be done in a .DC analysis. I think it's the same
> in LTspice.


If I understand correctly the guide the .dc directive requires either a
voltage or current source to sweep.

Marco


Jim Thompson

unread,
Jan 23, 2013, 10:50:15 AM1/23/13
to
Hi Marco,

In PSpice it would be like this...

.DC PARAM R <start value> <end value> <increment>

I couldn't find an equivalent in the LTspice manual.

Though it wouldn't surprise me if it didn't work. Mike included in
LTspice many of the features of PSpice.

I'm a member of the LTspice forum, so I'll post your question, or you
can join in...

http://tech.groups.yahoo.com/group/LTspice/

Jim Thompson

unread,
Jan 23, 2013, 12:23:57 PM1/23/13
to
On Wed, 23 Jan 2013 08:50:15 -0700, Jim Thompson
<To-Email-Use-Th...@On-My-Web-Site.com> wrote:

>On Wed, 23 Jan 2013 16:22:37 +0100, Marco Trapanese
><marcotrapa...@gmail.com> wrote:
>
>>Il 23/01/2013 15:52, Jim Thompson ha scritto:
>>
>>> In PSpice, it would be done in a .DC analysis. I think it's the same
>>> in LTspice.
>>
>>
>>If I understand correctly the guide the .dc directive requires either a
>>voltage or current source to sweep.
>>
>>Marco
>>
>
>Hi Marco,
>
>In PSpice it would be like this...
>
> .DC PARAM R <start value> <end value> <increment>
>
>I couldn't find an equivalent in the LTspice manual.
>
>Though it wouldn't surprise me if it didn't work. Mike included in
>LTspice many of the features of PSpice.
>
>I'm a member of the LTspice forum, so I'll post your question, or you
>can join in...
>
> http://tech.groups.yahoo.com/group/LTspice/
>
> ...Jim Thompson

Hi Marco, I posted your question to the LTspice List...

>
> A question has come up on S.E.D...
>
> Can LTspice do this PSpice-style sweep...
>
> .DC PARAM R 35 100 1
>
> -Jim Thompson
>

and got this answer...

"Hello Jim,

Please use this syntax below without .DC .

.step param R 35 100 1
.op

If R is the value of a resistor, use {R} for its value.

Best regards,
Helmut"

I haven't tried it, but I don't think its the same effect.

Marco Trapanese

unread,
Jan 23, 2013, 12:30:35 PM1/23/13
to


Il 23/01/2013 18:23, Jim Thompson ha scritto:


> Hi Marco, I posted your question to the LTspice List...
>
>>
>> A question has come up on S.E.D...
>>
>> Can LTspice do this PSpice-style sweep...
>>
>> .DC PARAM R 35 100 1
>>
>> -Jim Thompson
>>
>
> and got this answer...
>
> "Hello Jim,
>
> Please use this syntax below without .DC .
>
> .step param R 35 100 1
> .op
>
> If R is the value of a resistor, use {R} for its value.
>
> Best regards,
> Helmut"
>
> I haven't tried it, but I don't think its the same effect.


Thank you very much Jim.
Tomorrow I will try the solution proposed - anyway I'm afraid it's not
what I'm looking for.

I'll join the list too.

Marco


Jim Thompson

unread,
Jan 23, 2013, 12:52:46 PM1/23/13
to
Yes. I know you're looking for a "continuous" plot of behavior versus
the resistance.

>
>I'll join the list too.
>
>Marco
>

Great! You'll like it. Technical discussion without bizarre claims
of "I want it to work this way, don't bother me with the facts" >:-}

Jim Thompson

unread,
Jan 23, 2013, 5:29:29 PM1/23/13
to
Marco, You're in luck.

Just as I suspected, Mike Engelhardt included PSpice features in
LTspice.

So it'll be like I said:

Declare parameter...

.PARAM R=1K

Then Spice "Directive"...

.DC LIN PARAM R 1K 2K 100 ; For Example

I tested it simply by doing it in PSpice, then running the .CIR file
in LTspice... worked great!
0 new messages