--- In LTspice@..., "ks_bilder" <transients@> wrote:

Hello,

just started using LTspice and I don't know how to do the
following: In electrochemistry it is common practice to use
a so called constant phase element (CPE) in impedance analysis
of electrodes. The CPE is defined as follows:

Z = 1/( C * (j*w)^alpha )

where Z is the impedance, C equivalent capacitance, j imaginary
unit, w=2*pi*freq and 0 < alpha <= 1. For alpha=1 the CPE is
identical to an ideal capacitor.

What is the best way to define such an element in LTspice?
I would like to use the element in AC as well as in time
dependent modeling.

any help is appreciated!

Klaus

Hello Klaus,

Do you have some literature how other people have simulated it?

I think only a Laplace function can do the job.

There is absolutely no problem with any Laplace function in the
frequency domain simulation in (LT-)SPICE (.AC simulation).

The transient simulation (.TRAN) can make a lot of trouble with
these functions. The most important rule for transient simulation
is at least with LTspice that the value of a Laplace function
should fall to zero for high frequencies.
This means function with 1/s, 1/s**2 are good functions.

Now to some examples.

The value of the parameter alpha can be defined with a "param"-
statement. The character for exponent is ** and not ^ in LTspice.

.param alpha=1


CPE with G-source: OK in .AC but bad in .TRAN

Laplace=1e-6*s**{alpha}


CPE with E-source: OK in .AC, useful in .TRAN
The E-source circuit requires an additional current meter.
It's also necessary to add a small real value of 1u(1e-6)
to get useful results.

LAPLACE {I(V2)} = {1/(s**{alpha}*1e-6+1u)}


I have uploaded a test circuit to the Files section.

Files > Temp > Constant_phase_element1.asc


Best regards,
Helmut

?