how to simulate schematic - diyAudio
Go Back   Home > Forums > Amplifiers > Power Supplies

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 8th June 2012, 07:45 AM   #1
diyAudio Member
 
Join Date: Jun 2006
Default how to simulate schematic

Hi

I have found interesting discrete voltage regulators Discrete Voltage Regulator - John Swenson - Computer Audio Asylum and would like to view how they are simulated
I have draw schematic but don't know what to do to get simulated results like noise vs freq and output impedance vs freq
Attached Files
File Type: zip js5.zip (2.7 KB, 33 views)

Last edited by samoloko; 8th June 2012 at 07:53 AM.
  Reply With Quote
Old 8th June 2012, 08:04 AM   #2
diyAudio Member
 
Join Date: Nov 2009
Location: Wellington
Draw this circuit in any spice simulator. There are many free ones available such as Tina-TI or LTspice. Circuitmaker 2000 is also very good for this sort of thing.
  Reply With Quote
Old 8th June 2012, 08:15 AM   #3
diyAudio Member
 
Join Date: Jun 2006
It Is drawn In LTSpice but when I run simulation I got error logs
have you seen attachment
  Reply With Quote
Old 8th June 2012, 08:53 AM   #4
Elvee is offline Elvee  Belgium
diyAudio Member
 
Elvee's Avatar
 
Join Date: Sep 2006
Quote:
Originally Posted by samoloko View Post
have you seen attachment
Why do you zip your files? It is a PIA, and with the new forum capabilities, you have no excuse to stick to it.
__________________
. .Circlophone your life !!!! . .
♫♪ My little cheap Circlophone© ♫♪
  Reply With Quote
Old 8th June 2012, 08:55 AM   #5
jcx is offline jcx  United States
diyAudio Member
 
Join Date: Feb 2003
Location: ..
I1 is at least 10x too high

do a .TRAN type analysis for debugging a Spice sim - save the .NOISE for after the .TRAN shows proper cirucit operation

you can cruise the schematic following a successful .TRAN with the cursor and the DC operating point I, V will be displayed in the lower left corner as the cursor moves over wires, device terminals
  Reply With Quote
Old 8th June 2012, 09:48 AM   #6
diyAudio Member
 
Join Date: Jun 2006
I have corrected I1 to 0,005A and also output cap to 100uF and program run simulating output voltage at 5V but I would like to know what settings to set to get noise of regulator and output impedance
  Reply With Quote
Old 8th June 2012, 10:54 AM   #7
euro21 is offline euro21  Hungary
diyAudio Member
 
Join Date: Sep 2004
Location: Budapest
Proper Noise syntact:
.noise V(out) V1 oct 5 2 25000
  Reply With Quote
Old 8th June 2012, 01:11 PM   #8
diyAudio Member
 
Join Date: Jun 2006
thank you euro21

would you please tell me how can I view output impedance vs freq

regards
  Reply With Quote
Old 8th June 2012, 06:53 PM   #9
euro21 is offline euro21  Hungary
diyAudio Member
 
Join Date: Sep 2004
Location: Budapest
Quote:
Originally Posted by samoloko View Post
would you please tell me how can I view output impedance vs freq
Add signal generator to output. Signal AC=1V.
Run 'AC Analysis'. 1Hz-1MHz, 10 point/octave.
Click on 'out' node.
Edit 'AC Analysis' window title -right mouse click on title- (now V(out) ) to V(out)/I(V2).
Change 'AC Analysis' window left (vertical) menu (now decibel) -left mouse click- to 'Linear'. Thereafter it is Ohm.
Attached Images
File Type: jpg Rout.jpg (63.1 KB, 128 views)
Attached Files
File Type: zip JohnSwenson_Rout.zip (30.4 KB, 11 views)
  Reply With Quote
Old 8th June 2012, 08:10 PM   #10
jcx is offline jcx  United States
diyAudio Member
 
Join Date: Feb 2003
Location: ..
a Current Source is more commonly used for testing Voltage Output node impedance - like the Output of Voltage Regulator circuit

and the I1 bais current is still totally unrealisitic - the LED would be a DED at 1/4 A

the .Noise and .AC analysis can be misleading - they only operate on the small signal linearized model derived from the DC operating point analysis on start up

they don't show any nonlinear, saturation, reverse bias conditions that your test signals could cause in a "real sim"

really the only "safe" way to use the .AC based sims is after you have tested with .TRAN, simmed with realistic load, test sources with sine, or pulse/ramp waveforms

Last edited by jcx; 8th June 2012 at 08:15 PM.
  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
Anybody willing to simulate ? east electronics Solid State 28 24th January 2012 11:51 AM
Need some help to simulate Aleph 5 guitvinny Pass Labs 7 1st January 2008 04:11 PM
Someone willing to simulate a TL for me? tubee Multi-Way 21 27th November 2007 03:25 PM
Paid to simulate steve_mak Solid State 3 8th July 2007 06:34 AM
Can anyone simulate these Vifa's for me please. K-amps Multi-Way 9 31st May 2005 04:17 PM


New To Site? Need Help?

All times are GMT. The time now is 12:40 AM.


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