Go Back   Home > Forums > >
Home Forums Rules Articles diyAudio Store Blogs Gallery Wiki Register Donations FAQ Calendar Search Today's Posts Mark Forums Read

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

My circuit is too good!
My circuit is too good!
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 30th August 2017, 03:28 PM   #1
bugbear is offline bugbear  United Kingdom
diyAudio Member
 
Join Date: Jul 2016
Location: Norfolk/Suffolk border
Default My circuit is too good!

I've been trying to design a PSU for a HifiBerry DAC+.

Since the feed point is (in fact) a decent regulator, I'm just trying to get the high frequency trash cleaned up, so I'm using a CRCRC circuit.

I was going OK with a simple SINE voltage source. Noise was down at -120Db at 1KHz. Voltage had minor ripple, but at low freq - that's what regulators handle really well.

But since I was concerned about the nasty wave forms that diodes can (I'm told) generate, I changed the input side of my circuit to have a SINE source representing the secondary of a transformer, and a bridge rectifier.

This simulates fine and reasonably under .tran, but under .ac the noise is now down at -540Db. Which is a little too good to be credible. Something's wrong.

I upgrade my LTSpice-under-Wine-Under-Ubuntu from IV to XVII (oops, version drift) with the same result.

I've attached my crazy sim run, and the asc file. Can anyone see what dumb-*** newb mistake I've made?

BugBear
Attached Images
File Type: png aa.png (57.7 KB, 317 views)
Attached Files
File Type: asc psu_crcrc_filt.asc (2.8 KB, 4 views)
  Reply With Quote
Old 30th August 2017, 03:41 PM   #2
Osvaldo de Banfield is offline Osvaldo de Banfield  Argentina
diyAudio Member
 
Osvaldo de Banfield's Avatar
 
Join Date: Dec 2011
Location: Barrio Garay,Almirante Brown, Buenos Aires, Argentina
The simulation is only this, a simulation. Capacitors have certain amount of internal inductance, which resonates parallel at some well defined frequency. Above this frequency, the cap no longer behaves as a cap, more over it is inductive. Did you take this into account?
__________________
Osvaldo F. Zappacosta. Electronic Engineer UTN FRA from 2001.
Argentine Ham Radio LW1DSE since 1987.
  Reply With Quote
Old 30th August 2017, 03:58 PM   #3
KSTR is offline KSTR  Germany
diyAudio Member
 
KSTR's Avatar
 
Join Date: Jul 2007
Location: Central Berlin, Germany
Classic sim user error.
.AC analysis is based on infinitely small signal exitation (read: linear behaviour everywhere) at the operation point established by initial DC conditions.

Also, you mus always use .opt plotwinsize=0 to avoid data compression.

Last edited by KSTR; 30th August 2017 at 04:03 PM.
  Reply With Quote
Old 30th August 2017, 04:13 PM   #4
bugbear is offline bugbear  United Kingdom
diyAudio Member
 
Join Date: Jul 2016
Location: Norfolk/Suffolk border
Quote:
Originally Posted by KSTR View Post
Classic sim user error.
.AC analysis is based on infinitely small signal exitation (read: linear behaviour everywhere) at the operation point established by initial DC conditions.
Does that mean that (in effect) the signal isn't getting past the rectifier at all, and all I'm seeing on the output is noise?

I could understand that.

Quote:
Also, you mus always use .opt plotwinsize=0 to avoid data compression.
I shall go and look up what that means (since I don't know)

Thank you!

BugBear
  Reply With Quote
Old 30th August 2017, 04:26 PM   #5
KSTR is offline KSTR  Germany
diyAudio Member
 
KSTR's Avatar
 
Join Date: Jul 2007
Location: Central Berlin, Germany
Quote:
Originally Posted by bugbear View Post
Does that mean that (in effect) the signal isn't getting past the rectifier at all, and all I'm seeing on the output is noise?
Yes, actually you are only seeing calculation artifacts / resolution limits, not any type of noise (.AC analysis is noise-free). Your DC operation point is 0V, the diodes don't conduct at all. The scale value for an AC source is just that, a scale value. You can use 1uV or 100MegaV, it just scales the display. No actual voltage is presented to the circuit.

.opt plotwinsize=0 switches off the file size compression of the output data used for display. Think sort of MP3 vs WAV.
For the new LTspice version it might not be needed to locate this statement in the sim file directly, I don't know, and I will never upgrade from IV...

Last edited by KSTR; 30th August 2017 at 04:29 PM.
  Reply With Quote
Old 30th August 2017, 04:50 PM   #6
Mark Johnson is offline Mark Johnson  United States
diyAudio Member
 
Mark Johnson's Avatar
 
Join Date: May 2011
Location: Silicon Valley
My circuit is too good!
Looks like you made a couple of rookie mistakes.
1. Forgot to select a diode model. Your simulation schematic shows that you used a diode called "D" ... which is an ideal diode and decidedly not available in the real world. I suggest you choose diode 1N4004 for simulation studies

2. Connected AC stimulus incorrectly. To get the answer you want, replace the input by two voltage sources connected in series. The first one is (7.5V DC, 0V AC) and the second one is (0V DC, 1V AC). This will let you get the answer you want in .AC analysis
  Reply With Quote
Old 30th August 2017, 11:30 PM   #7
djoffe is offline djoffe  United States
diyAudio Member
 
Join Date: Oct 2008
I tweaked your sim a bit...ran it in the time domain...picked some real diodes...you can see the resultant ripple.
Attached Images
File Type: png PSUScreenShot.png (44.6 KB, 251 views)
__________________
www.akitika.com Featuring the GT-102 Power Amp and PR-101 Preamp kits
www.updatemydynaco.com Featuring upgrades for classic Dynaco Solid State Equipment
  Reply With Quote
Old 31st August 2017, 08:30 AM   #8
bugbear is offline bugbear  United Kingdom
diyAudio Member
 
Join Date: Jul 2016
Location: Norfolk/Suffolk border
Quote:
Originally Posted by Mark Johnson View Post
Looks like you made a couple of rookie mistakes.
1. Forgot to select a diode model. Your simulation schematic shows that you used a diode called "D" ... which is an ideal diode and decidedly not available in the real world. I suggest you choose diode 1N4004 for simulation studies

2. Connected AC stimulus incorrectly. To get the answer you want, replace the input by two voltage sources connected in series. The first one is (7.5V DC, 0V AC) and the second one is (0V DC, 1V AC). This will let you get the answer you want in .AC analysis
Thank you. Does this mean I (in fact) need slightly different models for different simulations?

Is there an easy way to manage this, other then (re)editing the model for the two sims?

(I've changed the diodes as recommended; I wasn't planning to worry about component selection until I had the sims running OK; there seemed little point).

BugBear
  Reply With Quote
Old 31st August 2017, 09:23 AM   #9
bugbear is offline bugbear  United Kingdom
diyAudio Member
 
Join Date: Jul 2016
Location: Norfolk/Suffolk border
Does LTSpice (version XVII) have any means of searching/filtering its component lists?

When I attempt to "Pick New Diode" I simply get an enormous unsorted scrolling list.

I don't think 1N4004 is there, but it's hard to tell.

BugBear
  Reply With Quote
Old 31st August 2017, 11:37 AM   #10
djoffe is offline djoffe  United States
diyAudio Member
 
Join Date: Oct 2008
1N4004 is not in the standard list. You'd have to add a model for it.
__________________
www.akitika.com Featuring the GT-102 Power Amp and PR-101 Preamp kits
www.updatemydynaco.com Featuring upgrades for classic Dynaco Solid State Equipment
  Reply With Quote

Reply


My circuit is too good!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

Forum Jump

Similar Threads
Thread Thread Starter Forum Replies Last Post
Good Phono preamp circuit? PeterMoreton Solid State 46 6th September 2016 07:45 AM
Can anyone recommend a good buffer circuit primalsea Tubes / Valves 9 23rd November 2004 09:58 PM
Very good tutorial on circuit design markp Solid State 13 26th September 2004 03:07 AM
Good bridge circuit soundNERD Chip Amps 0 16th September 2004 09:03 PM
Whats a Good 6L6 circuit? hacknet Tubes / Valves 34 25th April 2004 07:31 PM


New To Site? Need Help?

All times are GMT. The time now is 08:12 AM.


Search Engine Optimisation provided by DragonByte SEO (Pro) - vBulletin Mods & Addons Copyright © 2018 DragonByte Technologies Ltd.
Resources saved on this page: MySQL 14.29%
vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2018 DragonByte Technologies Ltd.
Copyright ©1999-2018 diyAudio
Wiki