> Tell a friend
This site matches your expectations, send a note to a friend about it.
|
> Previous contributions to the AboutSpice.com mailing-list
| 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
|
|
Copyright © 2001-2008
CIW.
All rights reserved. For any comment, update or feedback, please
use the contact us form. All registered
and unregistered trademarks referenced herein are the property of
their respective owners and no trademark rights to the same is claimed.
Read our privacy
statement.
The material on this web site is provided "as-is" without
warranty of any kind, expressed or implied, including without limitation
any warranty concerning the accuracy, adequacy, or completeness
of the material or the results obtained using same. CIW will not
be responsible for any claims attributed to errors, omissions, or
other inaccuracies in the material presented on this web site. In
no event shall CIW be liable for direct, indirect, special, incidental,
or consequential damages of any nature in connection with, or arising
out of, any use or application of the materials herein.
Links: KoffeeWare
- photo
backup - Send
photos - Send
pictures
|
