Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Question about capacitors

Status
Not open for further replies.

overflow

Advanced Member level 4
Joined
Jul 20, 2001
Messages
1,347
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,316
Activity points
142
Hi all,

I am designing a digital circuit and I need to put some capacitors between the power supply VCC and the ground GND.

Could someone explain me the difference on using a multilayers capacitor instead of a polyesther one ?


Thanks a lot...........
 

flatulent

Advanced Member level 5
Joined
Jul 19, 2002
Messages
4,629
Helped
489
Reputation
980
Reaction score
150
Trophy points
1,343
Location
Middle Earth
Activity points
46,689
multilayer

Multilayer is a type of chip capacitor made with a hard dielectric like ceramic matherials. These are good for power filtering and decoupling. This same material is used in one layer capacitors.

The capacitors made with several types of plastic dielectrics are more expensive for a give capacitance and are used for low loss and accuate applications like signal filters and low distortion amplifiers.
 

overflow

Advanced Member level 4
Joined
Jul 20, 2001
Messages
1,347
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,316
Activity points
142
Hi,

thanks for your reply. I want to give you more information. I am designing a reader/writer for smartcard. Now I have to put a capacitor between the VCC and GND pin of the smartcard. Now the question is : what kind of capacitor to use ? Multilayers or poliester ? And for what reason I need to choose one instead the other ?


Thanks a lot.............
 

flatulent

Advanced Member level 5
Joined
Jul 19, 2002
Messages
4,629
Helped
489
Reputation
980
Reaction score
150
Trophy points
1,343
Location
Middle Earth
Activity points
46,689
size

In your application size and cost is important. Since this is just filtering the power, accuracy and linearity are not important. Use the smallest surface mount capacitor for the capacitane you need. This will be the multilayer type.
 

wolf69

Advanced Member level 4
Joined
Sep 20, 2002
Messages
105
Helped
2
Reputation
4
Reaction score
0
Trophy points
1,296
Activity points
785
Multilayer may be a good choice since you don't need precision and low loss.
Anyway, usually to filter power lines I use a multilayer and an electrolityc capacitor in parallel. The electrolityc (since the high capacity) gives you good filtering and stability at low frequency. The multilayer at higher. But this can vary from application to application.
Bye!
 

falling_stone

Member level 1
Joined
Jul 19, 2002
Messages
40
Helped
1
Reputation
2
Reaction score
1
Trophy points
1,288
Activity points
503
Hi,
In power decoupling applications capacitor should provide lowest impedance at the desired frequencies.

What are the desired frequencies? The best way to know this is to measure noise spectrum on Your power supply rail. But before the device is created You may roughly find out this range of frequencies by:

knowing spectrum of Your analog circuit signal (audio/speech, video, etc.)

In digital circuit by knowing the rise/fall time of the chips You use (You will have peaks at F=1/((1..4)*Tr)
AND knowing Your clock frequencies
AND knowing access rates (if you have for example one access per 1024 clock cycles).

The lowest impedance means that capacitor(s) should have the least possible parasitic inductunce and resistance:
leads (so use SMD part),
construction (thats why You may see on the motherboards strange looking wide capacitors, this is one of the measures to decrease parasitic inductance in multilayer capacitors),
quantity (10 0.01uF capacitors are better than 1 0.1uF, but from the other point of view the cost in the decision argument))

The layout of PCB is one of the most critical things for good decoupling: locate decoupling capacitor as close to component as possible (but dont forget about assembly issues) and connect it to the component with the trace as wide as possible (but dont forget about thermal relief). The lowest capacitance should be situated closer to the component (see explanation below). Connect power supply "trough" the capacitor (I mean trace geometry, power supply should first reach capacitor and than the component). Connect the capacitor's ground terminal to the GND terminal of the component (with the trace as wide as possible) or to the ground plane (power and ground planes act as good capacitors by themselves, so if You have multilayer board, connect everything trough plane).

Different capacitors have their own resonance frequencies (they form LC tank with parasitic inductance) and this frequency lowers when capacity increases. At the frequencies higher than the resonant capacitor begins to perform as inductor, increasing its impedance with the frequency, so the best decoupling may be achieved in the area around the resonant frequency. Thats why if You want to cover wide frequency range You should use few different value capacitors connected in parallel (once I saw, for example, 1000pF, 10nF, 0.1uF and (after all :) - tantallum 10uF)

FINALLY: film capacitors (like polyesther) are usully much more accurate (which does not matter for decoupling applications) and produce less noise and no piezoelectric noise comparing from ceramic capacitors, but more expecsive and have higher inductance, thats why as far as I know they are mostly not in use in decoupling.

Do not forget "big" tantallum or aluminium oxide capacitor ("big" ceramic (~10uF) capacitors may be used only togehter with bigger tantallum or aluminium, because of the resonance and piezoeffect).

Sorry for such an amount of words :)
Best Regards,
F.S.
 

Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top