Take the 2-minute tour ×
Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. It's 100% free, no registration required.

I have a design where I have some high speed ICs and need to put a capacitor on the input voltage line to stabilize the voltage and protect from spikes or dips. I am operating at 5v and between 300 and 500 mA. My research indicates that I need an electrolytic capacitor for this application but I have no idea how to select the appropriate capacitance value. Also, why couldn't I just use a regulator for this purpose? The datasheet for my IC indicates that I should use a capacitor but wouldn't a VR do a better job?

share|improve this question
1  
First of all, I'm too low on reputation to comment. All whining aside, could you post your design IC name and links to the datasheets you're using? I've seen often that the IC design recommends components (some go as specific as the component maker). Did your datasheet not include this? If you could post a few additional details, such as part number, PCB layout/schematic, components you would like to use, I think you could get more specific answers. –  Shabab Sep 30 '13 at 19:18
    
Those capacitors are called decoupling/bypass capacitors. Decoupling = isolate from noise, bypass = provide local energy for when fast switching digital signals require it. –  dext0rb Sep 30 '13 at 19:27
    
The voltage regulator cannot respond instantaneously to changes in power requirements, resulting in a momentary dip in voltage when current demands increase. The capacitors charge to the output voltage level of the regulator, and then supply localized current while the regulator adjusts to meet the demands on the power rail. The capacitors are placed as near as possible to the current sink to minimize the resistive effects of the trace (or wire) connecting the IC to the supply. –  Scott Winder Sep 30 '13 at 19:36
    
@Dabloons - Listen to the man –  Andy aka Sep 30 '13 at 20:04
    

1 Answer 1

up vote 7 down vote accepted

Why couldn't I just use a regulator for this purpose?

Mainly, because every chip can't be right next to the regulator. The further your chip is from the regulator that's supplying it, the more resistance and inductance there is in the connection from the regulator to the Vcc pin (and from the ground pin on the way back).

If the current draw of your chip changes, this resistance and inductance will result in a change in the voltage at the Vcc pin.

I have no idea how to select the appropriate capacitance value.

There's two ways to look at this.

  1. When your chip changes its current draw, that di/dt will create a voltage drop across the inductance back to the voltage source. You want a capacitor that can supply (or sink) the current delta until the current from the source can respond.

    Unfortunately choosing a capacitor this way requires knowing two things that you often don't know: What will be the di/dt generated by the chip (this one you might actually know in some cases), and what's the inductance of the connection to the source (this you could simulate with a good power integrity tool, but that's expensive).

  2. You can design your bypass capacitors to provide a low-impedance connection to ground at all frequencies you're interested in.

    A low valued capacitor will have a high impedance at low frequencies because \$Z=\dfrac{1}{j\omega{}C}\$.

    A high-valued capacitor will require a larger package and have a high impedance at high frequencies because of its equivalent series inductance (ESL), for which \$Z=j\omega{}L\$.

    The solution is to put several values of capacitor in parallel, so that all frequencies are covered. A good capacitor vendor will provide ESL and ESR characteristics so that you can simulate your combination of capacitors and find a combination that works.

My research indicates that I need an electrolytic capacitor for this application

A common set-up is a 0.1 uF ceramic capacitor at the Vcc pin of each chip, and a few large-valued electrolytics spread around the board (not necessarily one per chip). Whether this is appropriate for your design isn't clear from what you've shared.

Generally the high values (in bigger packages and often electrolytics) don't need to be as close to the chip as the small-value (small package) capacitors, because they are useful at lower frequencies where inductance separating them from the load (chip) has less effect. Maybe one 10 uF capacitor can be shared between 4 or more loads. And a few 47 or 100 uF capacitors can be sprinkled around the board.

share|improve this answer
    
This is a really great response! Thorough and educational! Its exactly what I needed! Thanks! –  Dabloons Oct 1 '13 at 4:32
    
Excellent explanation!!! –  AKR Oct 2 '13 at 17:03

Your Answer

 
discard

By posting your answer, you agree to the privacy policy and terms of service.

Not the answer you're looking for? Browse other questions tagged or ask your own question.