In this schematic how are the caps such as C5, C6, and C9 connected? They are just going between my power source and ground?
Bypass or "de-coupling" capacitors which is their other name, do connect between a power rail and ground. As such, as you have already figured out, all those pins are electrically connected together.

That brings up an interesting situation when it comes to drawing them on the schematic.

You would think that the best way would be to draw them attached to the pin of the device you want them to be connected to so it is obvious what the capacitor is associated with. 

That IS one approach, however many component symbols have hidden power and ground pins, as such, showing them attached to a particular IC is not always  possible. It also makes for a very cluttered schematic. You can, if you wish, place them at the side instead, as you have shown, which visually implies that cap is associated with the thing it is nearest to.

However, even if you do a really good job of that, the PCB designer may or may not follow the schematic when placing the parts. The schematic after all is only a visual representation of the component and nets list.

In reality, the schematic design contains no actual positional information. The data passed to the PCB tool is merely a component list and a nets list. In the latter there will be a line like this..


  3.3V, U1-14, U4-1, U4-6, X1-8, C5-1, C9-1, C6-1, R10-1, R12-1, R13-1,...


That defines what the net 3.3V is connected to. Note it does not say explicitly C5 is connected to U1-14, even if you drew it that way, just that all those pins are connected to 3.3V.

Most PCB layout tools, and designers, use what is called "rubber-banding" on a "rats-nest" layout to place components in locations that minimize the trace length and avoid too many crossovers and twisting. 



Normally, the schematic designer only details the size of the board and where important things must be, like connectors, switches, LEDs etc. The PCB designer is trusted to place the rest, all be it with some review and approval by the schematic designer.

Unfortunately, since all those caps are attached to rails, depending on the software, they do not rubber-band well or, if you have power and ground planes, may not rubber-band at all. 

If you draw your schematic with connections to the devices and the PCB designer is not informed about that and does not follow your schematic manually, the caps can end up in entirely different locations because the PCB designer knows to place them close to chip power pins all on their own. 

That does not mean the PCB will have bad decoupling, but rather the C numbers on the schematic will no longer look like what is happening on the board. C5 may be in the position of C9 etc. As such, it is important to chat with the designer on this matter to ensure you both understand what is going to happen.

In some cases, if you trust the PCB designer to do his job, you can allow them to add or place all the capacitors on his own and use a "de-couplers" page in the schematic where all the caps are shown en-mass just for reference. A good PCB designer can even be trusted to add and maintain that page for you.







simulate this circuit &ndash; Schematic created using CircuitLab

Personally, I prefer the last method by far. It makes for much cleaner schematics and saves the PCB designer a lot of time not having to thumb through pages of schematics to identify hidden de-couplers before placing each one. 

Whatever method you choose, good communication between designers is critical. It really is a team effort. 

If you are doing both the schematic and the PCB design on your own you can use either method, though you will still find the common page, or schematic block,  easier. Count how many you need in total and make a first stab at the de-coupler page then place them after you decide where the ICs are going to go. Then adjust the schematic to add or remove caps as required.

If you ARE using a PCB designer you should realize, in all likely-hood, he has probably designed far more boards than you will ever design in your lifetime. Listen to what he says and learn from his experience moderated by your own.

As always, ultimately it is the responsibility of you, the schematic designer, to review the PCB layout before production to ensure that sufficient de-couplers have been used and that they are placed correctly.