Back to Forums
6 posts / 0 new
Last post
#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.

Can you help please?

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. 

AC_SWEEP.png

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). 

Transient study_1.pngTransient study_2.png

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.

Download PSpice and try it for free! Download Free Trial
Cadence