Go Back   Home > Forums > Source & Line > Digital Source

Digital Source Digital Players and Recorders: CD , SACD , Tape, Memory Card, 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 31st October 2002, 01:04 AM   #1
diyAudio Member
 
Join Date: Jan 2002
Default Inductors before the power pins vs ground bounce

From one of the sources:

http://www.dde-eda.com/ecadman/guide...iesTermination

"Ground bounce is caused by the voltage drop appearing across the chip power connections, due to the inductance of the power pins and the trace leading to the pins."

Although we like to add inductors on the power supply lines to clean up the power, it may also introduce/enlarge the problem of ground bounce. Am I correct or am I missing something here?

Normally, what size of inductor is best? 100uF? 250uF? 500uF?

Thanks

  Reply With Quote
Old 3rd November 2002, 02:58 PM   #2
diyAudio Member
 
Join Date: Dec 2001
Location: Eindhoven
Default Re: Inductors before the power pins vs ground bounce

Quote:
Originally posted by patwen
"Ground bounce is caused by the voltage drop appearing across the chip power connections, due to the inductance of the power pins and the trace leading to the pins."

Although we like to add inductors on the power supply lines to clean up the power, it may also introduce/enlarge the problem of ground bounce. Am I correct or am I missing something here?

Normally, what size of inductor is best? 100uF? 250uF? 500uF?
[/B]
I assume you mean uH rather then uF

Anyway, the drop in a supply loop is unavoidable, best you can do is keep it as small as possible, and shift the drop towards the supply rather then to ground, as most circuitry refers its' signals to groun.

By doing so the drop across the ground is minimised. Use ferrite beads, they absorb RF as well.

Typical values are 1 uH. The choice depends on the application, the used frequencies. Surf around at

http://www.murata.com/catalog/blm.pdf

Inn addition, my article may help

http://members.chello.nl/~m.heijlige...decoupling.pdf

all the best

Guido
__________________
Guido Tent
www.Tentlabs.com
  Reply With Quote
Old 4th November 2002, 01:57 AM   #3
diyAudio Member
 
Join Date: Jan 2002
Talking uH ... not uF

Thanks for the reply.

"and shift the drop towards the supply rather then to ground"

How does one actually do this?

Although a few uH is usually seen in the design, what's the problem if one uses something like 200uH or 500 uH, but keep the current rating of inductors proper (like using 0.5A or 1A inductors)?

Do so, will give a much cleaner DC supply free of HF noises, but at the expense of "responsiveness" of the regulator? Am I correct?
  Reply With Quote
Old 4th November 2002, 07:01 AM   #4
hifiZen is offline hifiZen  Canada
diyAudio Member
 
hifiZen's Avatar
 
Join Date: May 2001
Location: Mountain View, CA
Actually, the inductance referred to in the article is that which is in the short traces and pins between the decoupling caps and the IC. Therefore, the closer you mount your decoupling caps to the chip, the shorter these traces will be, and the less series inductance will be present to cause "ground bounce". I actually prefer to think of it as "rail bounce", since the voltage fluctuations can take place on either the supply voltage or ground. This type of noise is in fact more common on the voltage rail, not ground, especially if you've been careful to avoid large ground return current paths, and have made good use of ground planes.

It is often desireable to have some inductance between the power regulator and the decoupling cap, but <i>not</i> between the decoupling caps and the IC. Inductance and/or resistance between the regulators and the decoupling caps will tend to block high-frequency electrical noise from going either way through it... that is, it will isolate your IC supply voltage from high frequency noises on the regulator side, and likewise, the high frequency noise generated by the digital logic switching in the IC will be prevented from getting back to the regulator side. This is important because if this switching noise does leak all the way back to the regulator, there is a current associated with that voltage noise, and this current will have to return through the ground. This ground return current will thus run through other areas of the circuit board, causing small ground voltage fluctuations as a ground plane is not free from resistance or inductance itself. So, the more we can restrict high frequency ground currents to a small section of a board, the less they will affect the operation of other areas of the circuit. The ideal is to keep all ground currents (except DC currents) restricted to the tiny loop formed by the IC power pins, it's internal circuitry, the decoupling caps for <i>that</i> IC (and not another IC's decoupling caps), and the short lengths of trace or ground plane which connect the decoupling cap to the IC pins.
__________________
- Chad.
  Reply With Quote
Old 4th November 2002, 07:34 PM   #5
diyAudio Member
 
Join Date: Dec 2001
Location: Eindhoven
Thumbs up Groundbounce

Quote:
Originally posted by hifiZen
Actually, the inductance referred to in the article is that which is in the short traces and pins between the decoupling caps and the IC. Therefore, the closer you mount your decoupling caps to the chip, the shorter these traces will be, and the less series inductance will be present to cause "ground bounce".

This is partly true. If you place the decoupling capacitor close to the ground pin, the groundbounce will be lower than the supply bounce

I actually prefer to think of it as "rail bounce", since the voltage fluctuations can take place on either the supply voltage or ground.

Yes, exactly

This type of noise is in fact more common on the voltage rail, not ground, especially if you've been careful to avoid large ground return current paths, and have made good use of ground planes.

Yes and no (logically spoken that would be a no)

Consider RF currents run in loops of lowest inductance. If you run a (supply) trace above a groundplane, its return current will run exactly underneath that trace. As a result, the inductance of the "grounplane" is equal to that of the trace !!!

It is often desireable to have some inductance between the power regulator and the decoupling cap, but <i>not</i> between the decoupling caps and the IC.

Yes, fully agree

Inductance and/or resistance between the regulators and the decoupling caps will tend to block high-frequency electrical noise from going either way through it... that is, it will isolate your IC supply voltage from high frequency noises on the regulator side, and likewise, the high frequency noise generated by the digital logic switching in the IC will be prevented from getting back to the regulator side. This is important because if this switching noise does leak all the way back to the regulator, there is a current associated with that voltage noise, and this current will have to return through the ground. This ground return current will thus run through other areas of the circuit board, causing small ground voltage fluctuations as a ground plane is not free from resistance or inductance itself.

I wholeheartedly agree here

So, the more we can restrict high frequency ground currents to a small section of a board, the less they will affect the operation of other areas of the circuit. The ideal is to keep all ground currents (except DC currents) restricted to the tiny loop formed by the IC power pins, it's internal circuitry, the decoupling caps for <i>that</i> IC (and not another IC's decoupling caps), and the short lengths of trace or ground plane which connect the decoupling cap to the IC pins.
What can I add ?

Final words (gush, this sounds like Jerry Springer, yuck): Inside the IC still some inductance is present. The internal reference (often the substrate) bounce wrt the groundplane. Voltages of 200 mV has been observed........


best regards
-
__________________
Guido Tent
www.Tentlabs.com
  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
Parallel LM3886, input ground, power ground, safety resistor and oscillations. markiemrboo Chip Amps 5 9th August 2007 03:50 PM
Help with TP2050 Power Input Pins HolyGhostFire20 Class D 1 28th July 2005 04:36 PM
Contact bounce rho Solid State 6 10th March 2005 08:31 PM
Ground Bounce/ Oscillations in SPDIF fmak Digital Source 24 6th March 2004 07:52 PM
does connecting mains ground with circuit ground create a ground loop? jarthel Everything Else 0 25th June 2003 12:55 PM


New To Site? Need Help?

All times are GMT. The time now is 11:30 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