Concerning chips with more than one VCC and ground.

[corrado33]

Yes, I know they all have to be hooked up because while they ARE connected internally, the chip will not function correctly without them all hooked up.  (At least I read they're connected internally, but I'm guessing not much current could be run through the connections).

So my question is, what do you do for bypass capacitors?  Usually they're is a .1uF cap between the power leads of a microcontroller right?  If there are multiple power leads.... where do you put them?  Would you put it on the power bus that brings the 5V in?  

[Admin]

You don't always need to connect them all - see what the datasheet says. If it doesn't say anything, I connect them all to be safe.

As they would all be externally connected, you only need one set of filter capacitors. The exception is that if you have really long traces/wires, where noise can enter like if it was an antenna, than you may want some at both ends of that long trace/wire.

[corrado33]

Ahhh.  That's the situation I was thinking of.  Long leads etc.  It makes sense.  Thanks!

[waltr]

I disagree on the placement of by-pass caps Admin.

Each IC should have a by-pass cap (0.1uF to 0.01uF) on each IC and is connected as close as possible to the IC's Vdd (Vcc) and Vss (ground) pins.

On IC's with more than one Vcc or Vss pin ALWAYS connect them all to power or ground unless the data sheet say that you can leave one disconnected. IC's have multiple Vcc or Vss pins for a reason. This is for less voltage drop during high current draw and/or heat dissipation from the IC's internal circuits.

[Admin]

Each IC should have a by-pass cap (0.1uF to 0.01uF) on each IC

There are exceptions to this. Often times the IC just needs a stable supply, and if chips are close enough, you can get away with just one cap (per Farad type) shared between them all. It really depends on the IC's and the circuit layout. For products, it's ideal to have as few components as possible, and prototypes can validate the design stability.

On IC's with more than one Vcc or Vss pin ALWAYS connect them all to power or ground unless the data sheet say that you can leave one disconnected.

That's pretty much what I said (meant?), but just worded differently

IC's have multiple Vcc or Vss pins for a reason.

On rare occasion, some just give you multiple possible connections so as to make it easier for you to place them on a crowded PCB. But yea, if it's not made clear on the datasheet, I always just connect them all anyway.

[corrado33]

Each IC should have a by-pass cap (0.1uF to 0.01uF) on each IC and is connected as close as possible to the IC's Vdd (Vcc) and Vss (ground) pins.

So what you are saying is that your capacitors' leads should be placed as close to to the Vcc and Vss pins as possible.  So one lead really close to the Vss and one really close to the Vdd? 

What about chips where the Vss and Vdd pins are located opposite of each other.  The AtTiny2313/4313 for example?  The 20 pin Dip version.

 

[Admin]

What about chips where the Vss and Vdd pins are located opposite of each other.  The AtTiny2313/4313 for example?  The 20 pin Dip version.

You can always run a capacitor directly under the chip.

But unless you require ultra-stability (ADC or clock), I wouldn't worry about it for an ATmega.

[waltr]

Good question. Admin's gave a good answer and I have done that on many occasions. For many of the micro-controllers that the people on this forum use this works just fine. The circuit board for the $50 Robot is an example.

If you are building with DIP parts on say a perf board then most likely the processor or other parts are not running at high speed and the length of the cap leads is less critical. This works very well with processors running to a couple 10's of MHz.

If you are using a PCB (or designing a PCB) then there should be a ground plane (or ground copper filling the PCB space that doesn't have trace). Then a cap can be put close to the Vcc pin and connected to the ground copper.
If the processor or other parts are running at high speeds (greater than a few 10's of MHz) than having a copper ground plane or fill is required for good operation. For very high speed ( high 10's to 100's of MHz or higher) then there are other requirements for traces and ground planes to have the circuits work.

When you see profession PCBs (can be pic on the web)study the placement of the by-pass caps.

[corrado33]

Thanks admin and waltr.

I was also wondering about the ground plane.  But you answered my question.  It's good to know that connecting to the ground plane is almost as good as connecting right next to the ground pin.  And it's good to know that you still put the cap as close to Vcc as possible.  (Yes I'm making broad assumptions based on your statements  )

And admin, are you talking about under as in on a double sided PCB, or literally... under it.  I guess if it was in a socket you could do that (or just buy a socket with bypass caps included). 

[Admin]

Well, you said DIP version, so I assumed you were making a hand-soldered through-hole board.

If it was SMD, I'd use a ground plane.

Remember that with a ground plane, electricity still flows in a path that takes the shortest distance - possibly under noise-sensitive chips/traces. So be careful about high-current/noisy stuff on your ground plane.

Also, it's very very important that the crystal and capacitors (for the crystal) are as close as possible to your mcu. The caps for your power supply, not so much (by comparison).

On my Axon Mote, there are several grounds. Some grounds only for digital stuff, other grounds only for analog signals. It's important how these two ground types are connected, as analog noise doesn't hurt digital signals, but digital noise can hurt analog signals.

[Soeren]

Hi,

I was also wondering about the ground plane.  But you answered my question.  It's good to know that connecting to the ground plane is almost as good as connecting right next to the ground pin.

It is, as long as you make sure that the trace/plane from Vss to the other end of the cap is really low impedance.

And admin, are you talking about under as in on a double sided PCB, or literally... under it.  I guess if it was in a socket you could do that (or just buy a socket with bypass caps included). 

On a single sided PCB, with a (low impedance) copper pour connected to Vss, it's very easy to mount an SMD cap from a Vdd pin to the pour (on the solder side).

And if there's more than one Vdd pin and they're there out of need, a cap on each is a very good idea.
The need for caps as close as physically possible is not really due to the clock frequency. You could run a fast controller at 10kHz and still get problems, as it's the very fast level shifts that generates lots of harmonics (into the GHz range) and the more current you draw, eg. from an I/O, the stronger the transients.
As the harmonics are able to rech such high frequencies, 10mm of trace is a huge influence, and it will radiate, if not filtered (at both ends in some instances)

[Soeren]

Hi,

Also, it's very very important that the crystal and capacitors (for the crystal) are as close as possible to your mcu. The caps for your power supply, not so much (by comparison).

The x-tal should be close, but that's because it has got a fairly weak signal, so any noise may influence it.
But... The supply bypass is not less important, the x-tal does not produce any overtones, as it's output is fairly sinusoid, while the nanosecond level shifts will hammer through at lots of different overtones to even the best supply, and as a consequence, will spread to anything powered from the same supply.

[corrado33]

Thanks soeren. 

On my Axon Mote, there are several grounds. Some grounds only for digital stuff, other grounds only for analog signals. It's important how these two ground types are connected, as analog noise doesn't hurt digital signals, but digital noise can hurt analog signals.

I read about doing it this way.  Separating high noise items (fast switching transistors) from noise sensitive items (microcontroller) into different ground planes.  But I was confused because I knew they had to be connected.  But if they're connected they're not separated.  I'm going to take a look at your mote now, but would you implement some kind of filter between the ground planes?  The place I was reading about it said that there would definitely be filtering of the "positive" at each separate ground plane.  I gotta go find that site again...

What IS the proper way to connect them?

[Admin]

Electricity follows the shortest route. Image electricity flowing between the pins, as if the ground plane was just straight wires connecting everything to a single point (the ground pin of your battery).

Now try to make sure the analog and digital imaginary wires don't cross, and stay far from each other. On the Axon Mote, I planned out traces that I needed for other stuff to strategically divide up my ground plane to separate signals. And I kept my digital traces away from my analog traces.

You don't need to worry about this too much for your board, it's just good design in case you wanted it to be 'perfect'.

I didn't know this stuff when I designed the original Axon, and it still worked out fine.