1. Home
  2. Electronics Design
  3. LTSpice: Step multiple parameters simultanious

LTSpice: Step multiple parameters simultanious

Is it possible to define the step function so that it influences multiple parameters at once?

I would for example like to increase some capacitor and decrease the stimulus volrtage source simultaniously. Something like

.step param X list 1 2.2 10 and a Capacitor with a value 10p*{X} and the voltage source with V(on) = 1/{X} would come to mind.

That way, output would for the different steps could be scaled to same height.

Thanks

--
Uwe Bonnes                bon@elektron.ikp.physik.tu-darmstadt.de

Institut fuer Kernphysik  Schlossgartenstrasse 9  64289 Darmstadt
--------- Tel. 06151 162516 -------- Fax. 06151 164321 ----------
Reply to
Uwe Bonnes
Loading thread data ...

Uwe, I believe that Mike has made LTSpice essentially compatible with PSpice, so the expressions would be...

.step param X list 1 2.2 10 and a Capacitor with a value {10p*X} and the voltage source with value {1/X}

Note the curly bracket placement.

In PSpice you need to "declare" X...

.param X = 1

I don't know if LTSpice requires that or not.

...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.
Reply to
Jim Thompson

"Jim Thompson" schrieb im Newsbeitrag news: snipped-for-privacy@4ax.com...

Hello Uwe,

this is exactly how to use it in LTspice too.

This is isn't necessary in LTspice.

I have attached an example. Just copy the attached text into a file with extension ".asc", e.g. test.asc .

Best regards, Helmut

Version 4 SHEET 1 880 680 WIRE 128 160 64 160 WIRE 240 160 208 160 WIRE 64 192 64 160 WIRE 240 208 240 160 WIRE 64 304 64 272 WIRE 240 304 240 272 WIRE 240 304 64 304 WIRE 64 336 64 304 FLAG 64 336 0 SYMBOL voltage 64 176 R0 SYMATTR InstName V1 SYMATTR Value {1/X} SYMBOL cap 224 208 R0 SYMATTR InstName C1 SYMATTR Value {10p*X} SYMBOL res 112 176 R270 WINDOW 0 32 56 VTop 0 WINDOW 3 0 56 VBottom 0 SYMATTR InstName R1 SYMATTR Value 1k TEXT 16 40 Left 0 !.step param X list 1 2.2. 10 TEXT 16 80 Left 0 !.tran 1u uic

Reply to
Helmut Sennewald

Helmut Sennewald wrote: ...

Ah,

I have to place the braces in another way I tried. A hint in scad3.pdf would be fine.

But now another problem. Scad3.exe running under a recent version of Wine under Linux, when I reopen my .app file I get the the message "Previous analysis already found: .tran 150n" and I can't run the simulation.

Any idea of what's going wrong? I short look a wine relay log doesn't give me any hint.

--
Uwe Bonnes                bon@elektron.ikp.physik.tu-darmstadt.de

Institut fuer Kernphysik  Schlossgartenstrasse 9  64289 Darmstadt
--------- Tel. 06151 162516 -------- Fax. 06151 164321 ----------
Reply to
Uwe Bonnes

Hello Uwe,

Don't use .app files.

Save your schematic as a .asc file. File -> Save As Change the end of the file name to .asc instead of .app .

Close LTspice.

Restart LTspice

Open your previously saved .asc-file File -> Open

Change the "..tran 1 steady" according to your need. Example: .tran 10m

Now run your simulation.

The .app-files are more intended for demos and for people who don't have knowledge of SPICE.

Best regards, Helmut

Reply to
Helmut Sennewald

ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.