Loaded Tank circuit lossess -- PSPICE Simulation - Page 2 - diyAudio
Go Back   Home > Forums > Source & Line > Analog Line Level

Analog Line Level Preamplifiers , Passive Pre-amps, Crossovers, etc.

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 29th May 2006, 05:44 PM   #11
diyAudio Member
 
Join Date: May 2005
Location: Mumbai
Quote:
Originally posted by xitronics


Even with R = 1K, the observed Q in case A is 54, whereas theorotically it comes out to be 10000..!!
Oh a mistake by my calci , therotical value of Q with R = 1K is 100. Anyways, its still deviant.

______________
Prasanna Rao.
  Reply With Quote
Old 30th May 2006, 01:03 AM   #12
lndm is offline lndm  Australia
diyAudio Member
 
Join Date: Mar 2006
Location: nsw
In order to obtain a high Q, your source impedance needs to be as high as possible. Maybe you could try using a voltage source instead of the current source and using a large value of discreet resistance in series with this. At least then you would have this control.
  Reply With Quote
Old 31st May 2006, 01:13 PM   #13
diyAudio Member
 
Join Date: Sep 2004
Location: virginia
The formula for the resonant Q of that parallel RLC circuit is given by Q=R*sqrt(C/L). The Q changes when you change the ratio of C and L.
Regards,
Ray
  Reply With Quote
Old 1st June 2006, 02:38 PM   #14
jcx is offline jcx  United States
diyAudio Member
 
Join Date: Feb 2003
Location: ..
you might need to dig into spice settings that control the accuracy and defaults of the simulation, in LtSpice a default R damps inductors without explicit Rser declarations, you have to turn it off in the control panel

in .ac sim you need to use a very fine frequency grid to hit the 1/(2*pi) * 10e6 resonance exactly, or change component values to match a even frequency

with LtSpice I get ~ 1% amplitude difference even with 10000 points/oct freq resolution
  Reply With Quote
Old 1st June 2006, 05:43 PM   #15
jcx is offline jcx  United States
diyAudio Member
 
Join Date: Feb 2003
Location: ..
still had a default inductor Rser= 1 mOhm to clear in the control panel>hacks menu

normalized freq - works pretty near perfectly:

Click the image to open in full size.

them's femto dB and pico degrees!
  Reply With Quote
Old 2nd June 2006, 08:44 AM   #16
diyAudio Member
 
Join Date: May 2005
Location: Mumbai
Quote:
Originally posted by jcx


you might need to dig into spice settings that control the accuracy and defaults of the simulation.


That's right. But i havent found any data in the model of L in PSPICE; which represents its series DC resistance. Surely, Rseries is the only reason for the non-ideal voltage response in my experiment.

I am trying to go deep into PSPICE and seek that Rseries data for L. If anyone knows regarding it then kindly present them in this thread.

Regards Prasanna.
_______________
  Reply With Quote
Old 2nd June 2006, 12:37 PM   #17
diyAudio Member
 
Join Date: May 2005
Location: Mumbai
Default Now problem in Transient Analysis

Oh great..! The problem for AC sweep is solved. I increased the points/octave value to 10000 and the response is almost perfect.

But the transient reponse is absurd. Its showing amplitude of Vr = 10V at resonance, where should actually be 100V. Whats this problem for..?


I have attached the transient response with this post.


Kindly reply if anyone has any answer.

_________________
Regards Prasanna.
Attached Images
File Type: gif rlc.gif (31.4 KB, 50 views)
  Reply With Quote
Old 2nd June 2006, 12:42 PM   #18
lndm is offline lndm  Australia
diyAudio Member
 
Join Date: Mar 2006
Location: nsw
Just a thought, your time stepping seems a little coarse.
  Reply With Quote
Old 2nd June 2006, 12:45 PM   #19
diyAudio Member
 
Join Date: May 2005
Location: Mumbai
Quote:


Just a thought, your time stepping seems a little coarse.


Didnt get it.. .. Could you pls elaborate more on that..



Regds Prasanna
_________
  Reply With Quote
Old 2nd June 2006, 01:19 PM   #20
lndm is offline lndm  Australia
diyAudio Member
 
Join Date: Mar 2006
Location: nsw
As spice samples in transient mode, it takes samples at intervals of time. These intervals are referred to as the time step. Your plot looks a little low res (pointy )
  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
How big difference of noise between the realistic circuit and pspice simulation? goodnight521 Parts 1 20th June 2008 12:58 PM
How big difference of noise between the realistic circuit and pspice simulation? goodnight521 Analog Line Level 4 19th June 2008 06:22 PM
PSPICE simulation sunknu Everything Else 0 21st September 2006 10:30 AM
PSpice Simulation annex666 Everything Else 1 25th November 2005 04:56 PM


New To Site? Need Help?

All times are GMT. The time now is 08:11 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