Whats the best way to show output impedance with LTSpice? - diyAudio
Go Back   Home > Forums > Design & Build > Software Tools

Software Tools SPICE, PCB CAD, speaker design and measurement software, calculators

Please consider donating to help us continue to serve you.

Ads on/off / Custom Title / More PMs / More album space / Advanced printing & mass image saving
Reply
 
Thread Tools Search this Thread
Old 28th October 2011, 09:44 PM   #1
cbdb is offline cbdb  Canada
diyAudio Member
 
Join Date: Oct 2008
Location: Vancouver
Default Whats the best way to show output impedance with LTSpice?

I have searched DIY audio for a while and only found answers that aren't right.
If anyone can point me to a good solution that would be great.

Failing that:
I came up with my own method using the Delta Vout / Delta Iout technique, but its clunky. It needs 2 identical ccts, one with no load, the other with a a 1ua ac current source load. Do an AC sweep, then plot delta v/delta i or (V(vout1)-V(out2))/1ua. Seems to work well, but doubling the cct is a pain. Want to step the current load. Does anyone no how to plot the difference between the two stepped vouts (vout sep1 minus vout step2 )?? I will keep looking.
  Reply With Quote
Old 28th October 2011, 09:52 PM   #2
diyAudio Member
 
Join Date: Nov 2005
You can use a voltage controlled switch driven by a pulse train to get your step load. I don't think you can set switch resistance to Zero, but maybe really small.
  Reply With Quote
Old 28th October 2011, 09:53 PM   #3
cbdb is offline cbdb  Canada
diyAudio Member
 
Join Date: Oct 2008
Location: Vancouver
Found it. (V(vout)@2-V(vout)@1)/1ua

Cool!

Last edited by cbdb; 28th October 2011 at 09:58 PM.
  Reply With Quote
Old 28th October 2011, 09:57 PM   #4
cbdb is offline cbdb  Canada
diyAudio Member
 
Join Date: Oct 2008
Location: Vancouver
Quote:
You can use a voltage controlled switch driven by a pulse train to get your step load. I don't think you can set switch resistance to Zero, but maybe really small.
I run 2 sims (.step). First one current source =0a second time 1ua (could be anythig as long as it dosnt over load the cct.) i had trouble finding the @ sign which specifies the step.
  Reply With Quote
Old 30th October 2011, 06:07 PM   #5
jcx is offline jcx  United States
diyAudio Member
 
Join Date: Feb 2003
Location: ..
AC sources in .AC analysis never "load the circuit" - there is no "sim" going on, the cirucit is linearized around the DC operating point claclulation's output DC bias points

after that the Laplace transfer function is evaluated - you can put in Meg A and other than the scale there is no difference in the FR curves

so just use 1 A, V in AC sources to simplify reading the plots

you can also check at spot frequencies, or .step frequency of test sources in .TRAN - then you do need to pay attention to ciruit limits - but the same (sine) source can have an AC value of 1 A

Last edited by jcx; 30th October 2011 at 06:09 PM.
  Reply With Quote
Old 30th October 2011, 10:21 PM   #6
cbdb is offline cbdb  Canada
diyAudio Member
 
Join Date: Oct 2008
Location: Vancouver
Thanks I get it now. I made it more complicated than necesssary.
  Reply With Quote
Old 7th December 2011, 12:47 PM   #7
diyAudio Member
 
Join Date: Dec 2009
Location: Richmond, VA
For LTSpice newbs, the full description of my easy way is this:

Connect a current source with current flowing from ground to the node of interest . Right click on advanced for the current source and set AC amplitude to one in the box for small signal AC analysis.

Then run an AC analysis, and click on the node of interest. The default display shows a value in decibels. But go over and click on the Y axis, then select "linear". It will now show a frequency plot in volts. But because you're injecting current to the node, each volt you see here corresponds to one ohm of output impedance. Done.
  Reply With Quote
Old 9th January 2012, 04:52 AM   #8
gootee is offline gootee  United States
diyAudio Member
 
Join Date: Nov 2006
Location: Indiana
Blog Entries: 1
Quote:
Originally Posted by Wombaticus View Post
For LTSpice newbs, the full description of my easy way is this:

Connect a current source with current flowing from ground to the node of interest . Right click on advanced for the current source and set AC amplitude to one in the box for small signal AC analysis.

Then run an AC analysis, and click on the node of interest. The default display shows a value in decibels. But go over and click on the Y axis, then select "linear". It will now show a frequency plot in volts. But because you're injecting current to the node, each volt you see here corresponds to one ohm of output impedance. Done.
THEN, right-click on the voltage's heading at the top of the plot and add /I(I1) , with whatever your current source's name is in place of I1, and the vertical axis will display OHMS, with actual Ω symbols.

Cheers,

Tom
  Reply With Quote
Old 8th January 2014, 06:19 PM   #9
CSlee is offline CSlee  United Kingdom
diyAudio Member
 
CSlee's Avatar
 
Join Date: Mar 2009
Location: London
I just followed these steps, and have got some unexpected results. So obviously I have done something wrong...

1 amp current source across output,
AC analysis from 1 to 40000 Hz

Getting results in the kilovolts, kilo ohms. The plot is not actually what I expected either so has anyone got an idea as to why this might of happened?

Only just started using this software so I am sure I have missed something, but any advice would be great.

Thanks
Attached Images
File Type: jpg Output Z1.JPG (82.6 KB, 115 views)
File Type: jpg Output Z2.JPG (73.4 KB, 110 views)
File Type: jpg output Z3.JPG (26.0 KB, 110 views)
__________________
Broke solderer with delusions of grandeur
  Reply With Quote
Old 8th January 2014, 06:30 PM   #10
Mooly is offline Mooly  United Kingdom
diyAudio Moderator
 
Mooly's Avatar
 
Join Date: Sep 2007
Bob C suggests a similar technique but with the addition of a series resistor with the voltage source, the resistor being "high" in relation to the expected output impedance. Not sure how that would pan out for valve stuff.

There is an LTspice example showing this on Bobs site, the examples all accompany the book.
__________________
-------------------------------------------------------
A simulation free zone. Design it, build it, test it.
  Reply With Quote

Reply


Hide this!Advertise here!
Thread Tools Search this Thread
Search this Thread:

Advanced Search

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are Off
Refbacks are Off


Similar Threads
Thread Thread Starter Forum Replies Last Post
THD vs output power in LTspice Tekko Solid State 7 4th January 2012 01:40 PM
LTspice model for Dynaco A470 Output Transfomer Ray Waters Tubes / Valves 5 17th February 2011 03:33 PM
Measuring impedance with ltspice Telstar Software Tools 1 27th January 2011 02:50 PM
3C24 in a SE output stage - output transformer impedance recommendation !!! aldovan Tubes / Valves 15 6th September 2008 10:18 AM
Can An Output Transformer Change A Voltage Amp's Output Impedance From 0.1 To 47 Ohms kelticwizard Everything Else 11 25th March 2007 05:17 AM


New To Site? Need Help?

All times are GMT. The time now is 02:34 PM.


vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2014 DragonByte Technologies Ltd.
Copyright 1999-2014 diyAudio

Content Relevant URLs by vBSEO 3.3.2