LTSpice variable values question

[Trileru]

Hello.
I'm trying to simulate an output stage with LTSpice and want to check what is the lowest noise I can get out of it by varying certain components.
So far so good. I need to vary one resistor but that resistor changes the bias of the output stage. It's not the bias setting resistor, but another resistor.
Now, I have to use the .step param for those two resistors so I can keep the bias at roughly the same value when varying the resistor in question. In the classical way that I know how to use this option the software will basically run through each step of the simulation like this.
Let's say res1 and res2 are the variables, and the values are from 10 to 100 in steps of 10 (ohms) for each.
The software will make 100 iterations for this setup as first it will use 10 ohms for res1 and 10 ohms for res2.
The second iterations will be with 20 ohms for the first resistor and 10 ohms for the second. and so on.
I'd like to know how to step two values at the same time. So the software will make a sim for 10/10 ohms then the second sim to be for 20/20 ohms.

 

[jcx]

you can step a numeric parameter say X

then you can calculate the value of each R based on a equation in X

{X*100} or {X + 1k} the curly braces in a component's value field makes it calculate the value

more indirectly you can make the .step param be the index into tables of values for each component
the syntax is obscure - example files in the Yahoo LTspice group

There is a very active Yahoo Group dedicated to LTspice. It's at http://groups.yahoo.com/group/LTspice. Your particular question has been discussed there several times. All posts are archived and are searchable. Also, the files section contains much useful reference material, models, and example circuits.

You can make the values of the components you wish to vary a table function of a stepped parameter. Use the ".step" command to step the controlling parameter (e.g. .step param n list 1 2 3...) to get several runs to appear in one plot. Then edit the value field of the target components to depend on this parameter (e.g. {tbl(n,1,1k,2,1p,3,1T} ). Be sure to enclose the parametrized expression in curly braces. Use extremely large values to "disconnect" the component and extremely small values to short it out.

To display only a particular step in the plot window suffix the trace expression with the step selection operator "@n", where n is the desired step number.

Most of this information is contained in the help file and is accessible via the help search function.

 

[Trileru]

Thank you very much
I must read on this on the yahoo group.

 

[Mosquito]

.step param X list 10 20 30 40 .....100
then name res1 = {X} and res2 = {X}
the same as per step varying the two halves of a PP output transformer at once
cheers
J.

 

[Trileru]

This is how I solved it:
.step param N 1 12 1
.param RES1=table(N,1,40,2,50,3,60,4,70,5,80,6,90,7,100,8,110,9,120,10,130,11,140,12,150)
.param RES2=table(N,1,317,2,322,3,327,4,332,5,337,6,342,7,347,8,351.5,9,356,10,360.5,11,364.5,12,368)

Someone over at LTSpice Yahoo group gave me the solution.