| Submitted by: hvogt on 2005-10-02 18:46:40. | |
| Topic: | Re: Re: simulate variable resistors |
| Body: | add a little bit of structure * Voltage controlled potentiometer * vary supply and control voltage .DC Vhigh 0 1 0.01 Vcontrol 0 1 0.2 *control voltage Vcontrol control 0 DC 1 *supply to resistor Vhigh high 0 DC 1 * V(mid) is the potentiometer wiper output *upper part of resistor BResu high mid I=((V(high)-V(mid))/10k/(V(control)+1e-6)) *lower part of resistor BResd mid low I=(V(mid)-V(low))/10k/(1e-6+1-V(control)) * add 1e-6 to prevent divide by zero (adds only a small error) *measure current: Vlow low 0 DC 0 .END |
| Reply to this contribution | Write to the contributor | |
| Submitted by: hvogt on 2005-10-02 18:37:31. | |
| Topic: | Re: simulate variable resistors |
| Body: | Hi, a potentiometer with plain old Spice (as found in http://www.uni-duisburg.de/FB9/EBS/hauptteil_software_en.html: * Voltage controlled potentiometer * vary supply and control voltage .DC Vhigh 0 1 0.01 Vcontrol 0 1 0.2 *control voltage Vcontrol control 0 DC 1 *supply to resistor Vhigh high 0 DC 1 * V(mid) is the potentiometer wiper output *upper part of resistor BResu high mid I=((V(high)-V(mid))/10k/(V(control)+1e-6)) *lower part of resistor BResd mid low I=(V(mid)-V(low))/10k/(1e-6+1-V(control)) * add 1e-6 to prevent divide by zero (adds only a small error) *measure current: Vlow low 0 DC 0 .END Regards Holger |
| Reply to this contribution | Write to the contributor | |
| Submitted by: steeletraps on 2005-08-26 20:33:32. | |
| Topic: | Re: simulate variable resistors |
| Body: | Hi, I don't know anything about Opus, but have they expanded beyond the basic SPICE. With my Micro-Cap version, I can define the value of a resistor as: 1k-R(R1) and then have another resistor called R1 that is the one I sweep in DC analysis to mimic a 1kohm pot. I believe PSpice has something very similar too. |
| Reply to this contribution | Write to the contributor | |
| Submitted by: nateD on 2005-08-18 10:35:08. | |
| Topic: | simulate variable resistors |
| Body: | I need to simulate the sweep of a three pole variable resistor. I know that I can do a .DC analysis that sweeps a single parameter value, but how do I simulate one side of a variable resistor increasing and the other side decreasing? I am using Spice Opus version 2.22 on Linux, but could step back into the windows world and use pspice if I had to. Any bright ideas, or am I just too dim to see the obvious solution? Thanks for your help, Nate |
| Reply to this contribution | Write to the contributor | |
Post a new contribution | Back to the list of topics