Back to Forums
6 posts / 0 new
#1 Apr 7, 2020
jakjoud
Offline
Last seen: 1 year 3 months ago
Joined: 2020-04-07 18:46

Need of resistor controled by frequency

Dear all,

Hello,

This is my first time on your forum.

I am working on the electric equivalent circuit of acoustic and optic propagation phenomena.

I have been in need of a component (resistor for instance) whose value is a function of the supplied frequency.

I'm using a VAC source in AC sweep mode.

Thank you

Wed, 2020-04-08 15:01
retiredEE
Offline
Last seen: 1 week 17 hours ago
Joined: 2018-03-21 12:19
You can create a frequency dependent resistor using a voltage controlled current source who's value is a frequency dependent function of its terminal voltage. You can use the GLAPLACE(continuous function of f) or GFREQ(tabular function of f) to implement this.  For example, run this test circuit:

TEST R(freq)
*
* Test a frequency dependent resistor
*
V1 1 0 AC 1
R1 1 2 9
G1 2 0 LAPLACE {V(2,0)}={1/(1+0.01*s)}
.AC DEC 100 10 10K
.PROBE I(G1)
.END

G1 emulates a resistor whose value is: 1+0.01s

Refer to the PSpice REF manual and the PSpice USER guide for more information on these parts.
Fri, 2020-04-10 17:53
jakjoud
Offline
Last seen: 1 year 3 months ago
Joined: 2020-04-07 18:46

Thanks a lot

Sat, 2020-04-11 10:23
retiredEE
Offline
Last seen: 1 week 17 hours ago
Joined: 2018-03-21 12:19

Your welcome.  Also, if you substitute IMG(0.159155*s) for s you can create an expression that's a function of the real variable f rather than the complex frequency variable s.

Thu, 2021-05-06 10:47
yucj
Offline
Last seen: 3 months 18 hours ago
Joined: 2021-01-20 16:45

Hi, I also have a question related to that frequency controlled resistor.

To model a frequency-controlled resistor, I used the method including a non-linear laplace form voltage control current source "GLaplace" as your guys 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 (yellow line) change from 1 to 101 ohms when frequency changing from 1 to 100 Hz. And the voltage crossing that model is consistent with our concept. In AC sweep simulation, that model is working ok.

However when I simulate that in transient simulation with a simple 100Hz sin wave (Green line in "transient_study 2" is input 1V, 100Hz sinwave souce, red line is resistor voltage and should be a 0.5V sin wave and no phase shift compared with input source), as you could see, the resistance response of model is very inaccurate (yellow line in transient_study 1, the value should be R=1+100=101 ohms).

So I am not sure if that Glaplace model is useable in the trasient simulation.

Any suggenstions and help would be appreciated.

Thank you.

Fri, 2021-05-07 11:27
retiredEE
Offline
Last seen: 1 week 17 hours ago
Joined: 2018-03-21 12:19

Your analysis is now in the time domain and the calculation of a function of s is different.  See the section in your PSpice User Guide titled "Cautions and Recommendations for Simulation and Analysis" in the Analog Behavioral Modeling chapter.