Decoupling Capacitor value on a dc supply

[ameachin]

Please can you tell me if I am correct on both the choice and value of capacitors I am using on a 5v DC power line to an RF circuit.

I have decided to use a Tantalum 10uF for the low frequency, a .1uF Ceramic for the high frequencies and a 0.001uF Ceramic for the very high frequencies. All capacitors are mounted in parellel close to the vcc pin of the RF circuit.

 

[BrianG]

As a general rule, yes, that's the best way to do h.f. decoupling, however it all depends on what the "r.f. circuit" actually is. Are you trying to stop the r.f. circuit from causing interference with other parts of the circuit, or are you trying to stop some other power supply noise from modulating the r.f. circuit?

You may find with some circuits it's better to isolate it by putting some inductance between the r.f circuit and the capacitors. Feed the power supply to the circuit via a ferrite bead around the wire, or if it's a circuit board, break the track and add a small U-loop of wire through the ferrite bead. You can also get surface-mount ferrites beads too.

 

[ameachin]

Many thanks Brian for your reply. Well, I am trying to reduce noise from other parts of the circuit sharing the same power supply.

The RF side is a self contained SIL board (incorporating both the RF & Decoder) this then plugs into the main circuit board.

If I use an Inductor in the power line to the RF circuit do I still need to use the decoupling capacitors before the inductor?

One more area you may be able to help with Ground Plane: Currently I have flooded the bottom of the double sided circuit board with copper with small islands for top mounted components and kept all signal / power tracks on the top also. My circuit incorporates both analogue and digital how important is it to have a seperate ground planes for each or is it ok to utilse the one ground plane for both?

Hope you can help, many thanks

 

[ameachin]

Forgot to ask since you mentioned Inductors I have found the following;

RF inductors with a ferrite core encapsulated with ratings from 1 millihenry up and standard axial ferrite bead inductors. Which would you recommend for a 5v RF circuit using 50ma (frequency 433mhz)?

Hope you can advise, many thanks

 

[BrianG]

Hi, sorry for the delay - I have been on leave.

Ground planes: this is a slightly tricky one to answer because like most things in electronics the answer is "it all depends..." Without seeing all of your circuit and its layout, correct performance can't be guaranteed; generally a ground plane will improve things if it's done correctly - but can make things worse if done badly! One ground plane can be OK for both, but if you have things like high-power clock signals with fast edges in the digital bit, it can help to "bury" these in a layer between two ground planes.

Filter inductor/capacitor networks: you will have to work out how much voltage drop your d.c. component will cause in the inductor winding. It is usually the resistance of the wire which determines which inductor you can use, together with its self-resonant frequency. You can usually never have too much decoupling capacitance, but make sure you know where the capacitor h.f. by-pass currents flow in ground planes, etc!

 

[ameachin]

Hi Brian

Many thanks for writting back hope your leave went well, sorry to throw all of these questions at you, I did not realise how hard the field of electronics was!

Is there a way of attaching an image to the Forum so that I can show you what I have designed?

 

[IRstuff]

In general, bypass capacitors are supposed to be placed closest to the source of the displacement current that the capacitor must supply. This means that the capacitors, particularly the higher frequency ones, must be placed as close to the component directly connected to the power rail.

That's why you usually see bypass capacitors by each IC on a computer board.



TTFN

 

[47gandalf]

One additional input. If your RF frequency is high, you might make the last capactitor a dipped silver-mica type. They remain capacitive at very high frequencies, but the maximum C value is not very high.

 

[Comcokid]

I thought you were suppose to avoid use of silver-mica capacitors where there would be a DC bias, because time, temperature, and moisture would result in silver migration and eventual conduction. Is this correct?

 

[jtsamuels]

My two cents. With a double sided board a single ground plane is preferable to a split plane AS LONG AS THE high speed digital is routed away from the analog and is over contiguous copper that allows the return current to flow undisturbed back to its source (check those vias, only find one for the return current is a sure noise source. Add multiple parallel vias to reduce the inductance). A good source for an overview of using ground planes the better way is:

http://www.hottconsultants.com/papers.html

I have taken over a half dozen in plant courses from Henry and consider them some of the easiest understood quidelines for board layout/noise reduction. Split planes can work but under NO Circumstances should digital run over the analog return plane or vice versa. Any signals that need to be shared between these sections require some type of isolated coupling (optical, magnetic, etc.).

THE OVERRIDING DETAIL IS THAT ANY CURRENT SOURCED MUST HAVE ITS RETURN PATH BE AS LOW AN INDUCTANCE AS POSSIBLE. ANY DEVIATIONS FROM THIS RESULTS IN A GRADIENT BEING DEVELOPED WHICH WILL GENERATE A DIFFERENTIAL SIGNAL LEADING TO NOISE OR EMI EMISSIONS. THAT MEANS THE GROUND PLANE MUST BE UNIFORM WITHOUT SLOTS, REMOVED AREAS, OR ANYTHING THAT WILL FORCE A RETURN CURRENT TO HAVE TO DETOUR FROM FOLLWING BACK, ITS OUTGOING SIGNAL TRACE. Please check Henry's site, he explains it so much better.

For the capacitors, once again it is the inductance that causes the capacitors to stop working at elevated frequencies. Need more capacitance? Parallel them in an ARRAY about your point to both lower the ESR of the caps as well as the ESL (equivalent series inductance) which is the critical aspect.


However, for RF power distribution, consider using the combination of a pi input, L section output filter configuration, where each section of your RF design has its own unique L section to deliver the 5v.
Pi Filter L Section
L1 L2
----00000------- ---00000---
| | | |
_ _ _ _
-C1 -C2 -C3 - C4
| | | |
V V V V

Typical values for
C1=100 - 1000 uF (Load current/ripple voltage dependent)
C2=1-10 uf Tantalum (doesn't tolerate negative voltages well)
C3=1000 - 5000 pF (Silver Mica)
C4=100 - 1000 pF (Silver Mica) (noise related)
L1= 10 - 100 mH (Ripple voltage/load current dependent)
L2= 50-500 uH (noise related).


Thus you have ONE Pi section and as many L sections as you have RF points to apply 5v to. Check out the ARRL site for more in depth and better information

Good Luck,
Jim

 

[ameachin]

Many thanks for all of your input, I am really starting to feel out of my depth when it comes to RF PCB design is there any recommendations to who I could go to, to over look what I have designed?

 

[ameachin]

One more question I am using a 2N3904 NPN to switch an LED on momentary. The LED is 2.2v / 20ma.

The supply voltage to the Transistor is between 3.8 normal to 5v max with 10ma.

A. What value in-line resistor should I use before the transistor

B. What value resistor should I use between the base and gnd

Should I be using any decoupling capacitors to help illiminate noise?

Hope you guys can help! many thanks :0)