Using Glaplace component in PSPICE for frequency controlled resistor

Skip to first unread message

Chengju Yu

May 6, 2021, 10:56:24 AM5/6/21
Hello everyone,
To model a frequency-controlled resistor, I used the method including a non-linear laplace form voltage control current source "GLaplace", that some websites and engineerings suggested.
I tried with a simple equation, R=1+f, when I do the AC sweep study in the PSPICE, the model works fine as I attached figure as AC sweep, the resistance changes from 1 to 101 ohms when frequency changing from 1 to 100 Hz. And the voltage crossing that model is consistent with concept. In AC sweep simulation, that model is working ok.
However when I simulate that in transient simulation with a simple 100Hz sin wave, the resistance response of model is very inaccurate (the value is far away from R=1+100=101 ohms).
So I am not sure if those Glaplace model could be used in the transient simulation.
Did anyone know any information related to that?
Any suggestions and comments would be appreciated.
Thank you.

Kevin Aylward

Oct 17, 2023, 3:21:10 PMOct 17
>"Chengju Yu" wrote in message
What are you trying to achieve?

Typically, the point of a frequency dependant resistance is to simulate skin
effect resistance for inductors.
This can be achieved by an LR ladder network.

If this is your goal, a better option is to use a model that gives the
correct 45 degs, 10db/dec characteristic. Pure frequency dependant resistors
produce responses that are non real.


.SUBCKT SkinEffectResistance_XN !0_A !1_B FMAX=110M K=0.49
* _SS_Symbol [<System>Functional.ssm] [SkinEffectResister]
V!1 !1_B B 0
V!0 !0_A A 0
* skin effect impedance variation with sqrt(F)
* set F0 to > max fequency of operation
.param FX={FMAX/100}
.param L={0.1*K/sqrt(FX)}
.param R={10*K*sqrt(FX)}
R8 Node8 A {R/128}
L8 Node8 B {L*128}
L1 Node1 B {L}
R1 Node1 A {R}
R6 Node6 A {R/32}
R5 Node5 A {R/16}
R4 Node4 A {R/8}
R3 Node3 A {R/4}
R2 Node2 A {R/2}
R0 B A {R}
R7 Node7 A {R/64}
L2 Node2 B {L*2}
L3 Node3 B {L*4}
L4 Node4 B {L*8}
L5 Node5 B {L*16}
L6 Node6 B {L*32}
L7 Node7 B {L*64}

There is an example in my freebee SuperSpice


That demonstrates this.

Furthermore, there are sets of CoilCraft inductor models that fully
implement their inductors using that technique. The Model files should also
run directly in LTSpice.

-- Kevin Aylward SuperSpice

Reply all
Reply to author
0 new messages