LTSpice plot voltage vs step param

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

Il 23/01/2013 15:52, Jim Thompson ha scritto:

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

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...

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

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. ...Jim Thompson

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

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

Yes. I know you're looking for a "continuous" plot of behavior versus the resistance.

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

Marco, You're in luck.

Just as I suspected, Mike Engelhardt 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! ...Jim Thompson