Power and Supply Pin Use on Schematics

On 09/30/2013 11:27 AM, David Kanazawa wrote:

When I run ERC, I get warnings of interconnected nets. I believe I'm

using Power and Supply pins incorrectly. Simple case - how do I properly

connect +5v to VCC and to VDD on the same net?

It is a warning. Either ignore it or fix the component to match your

power and ground names. This is a check that helps simple circuits of

beginners and a nuance with complex circuits.

Paul

On 09/30/2013 11:27 AM, David Kanazawa wrote:

...

I'm running into 2 distinct problems.

1) I need to keep the isolated VCC and GND nets separated on the

schematic. I'm having some sucess with this as I am using different net

names (i.e. GND and -VOUT)

Use the supply symbols in supply.lbr or supply2.lbr for each of your

different nets.  i.e. GND, GND1, GND2, etc.

Eagle will treat these, as it should, as separate nets.  To tie them

together, use the SHORT device in the attached shorts.lbr.  This is

merely two pads that overlap each other.  This will produce a DRC error,

but it can be approved to prevent from being a nuisance.

2) Power and Supply pins are more challenging. Some IC's have VCC,

others VDD. The isolated section I've given the net name of +VOUT. All

are at +5v.

You can use the supply symbol +5V from the supply2 library to name the

net (it conveys more information to the reader).

When I run ERC, I get warnings of interconnected nets. I believe I'm

using Power and Supply pins incorrectly. Simple case - how do I properly

connect +5v to VCC and to VDD on the same net?

ERC warnings of the type "VCC connected to +5V" can be approved.  All it

means is that the name of the power pin does not match the name of the

net to which it's connected.

If you want to connect separate nets, use the SHORT device.

I do this quite often to separate different grounds such as analog

ground, a noisy high-power ground, and a logic ground.  I want to tie

them all together eventually, but keep them separate as long as

possible.  So all the shorts are placed close to the battery connector.

Since it's an on-board component, I take all shorts out of the BOM.

HTH,

    - Chuck

Paul and Chuck,

Thanks very much for taking the time to help (re)explain this issue. It's very helpful to have the concrete examples of devices, the error messages and result of "approving" errors. It would not have occurred to me to search for the SHORT device, so that was particularly useful. I'll give this a go and hopefully it will allow me to complete this section of schematic layout. Nice touch on removing the SHORT from the BOM.

One side note - I'm not clear on why it's necessary to even have the supply and power connections laid out. Is it for clarity of which voltage is being applied to a particular net such as defining the VCC voltage?

And on to the next topic - "Polygons May Have Fallen Apart".

Thank you for helping me understand how to use these tools!

David K.

On 10/01/2013 01:29 PM, David Kanazawa wrote:

One side note - I'm not clear on why it's necessary to even have the

supply and power connections laid out. Is it for clarity of which

voltage is being applied to a particular net such as defining the VCC

voltage?

VCC, of course, stems from the collector voltage, just as VDD refers to

a drain voltage.  Consider the case where a SUPPLY device called VDD is

attached to a POWER pin on an IC named VDD.  This certainly avoids the

DRC warning.

Putting on my philosopher's hat for a moment, the purpose of a schematic

is to convey the design of a circuit to a reader.  Some may call it art,

and other may call it the essence of the circuit.  Whatever one chooses

to call it, a schematic should convey what the circuit is about, and not

necessarily how the design is manifested on a PCB.

Back to engineering...  So, when a reader sees that a VDD supply is

connected to VDD pin, it's a real "duh" moment.  The next question is

"what is VDD?".  So, instead of using a SUPPLY device called VDD,

consider using a SUPPLY device that conveys what the voltage on that net

should be.  Something like "5V", "3.3V", or "+15V".  This serves a

dual purpose in that it immediately conveys to the reader what VDD

should be, and it produces a DRC warning allowing the designer to verify

(by approving the error) that the proper voltage supply should indeed be

connected to VDD of that particular IC.

As far as leaving the power pins off of a schematic, I would recommend

against it for the simple reason that it hides information from the

reader.  Many IC's have power and ground pins on the corner (7 and 14,

or 8 and 16); others have power and ground midway down the sides; and

QFP's have multiple power pins scattered wherever they're needed.  In

cases where the power pins are a separate gate from the main schematic

symbol, I usually stuff them down in a corner of my schematic along with

a bypass capacitor.  But keep them on the schematic

I would recommend using SHORT devices sparingly in that it, in part,

defeats the purpose of the DRC.  For example, if one were to connect a

+5V supply to a GND supply through a SHORT, Eagle would not complain one

bit.  But as soon as you applied power, your board would certainly

complain with a puff of smoke.

HTH,

    - Chuck

David Kanazawa wrote:

Paul and Chuck,

 

 

One side note - I'm not clear on why it's necessary to even have the

supply and power connections laid out. Is it for clarity of which

voltage is being applied to a particular net such as defining the VCC

voltage?

 

One thing to watch out for is that VCC and VDD, for example, are used

interchangeably in the standard libraries to mark power on both +5V parts

and +3.3V parts. If you bring in a part that uses VDD for +5V, and hook that

power pin up to the 'VDD' supply symbol from the SUPPLY2 library, and

connect that to a 5V source, everything is well. That is, until you bring in

another library part that runs on +3.3V but also uses 'VDD' as the power pin

label. Eagle will nicely and quietly hook that pin up to your +5V VDD net

automatically. If this is a normally-hidden invokable power symbol, you may

never realize the problem until you power the board for the first time. If

you invoke this power symbol, not only is it easier for someone else to read

your schematic, but you might also spot the issue (ERC certainly will) when

you attempt to connect your +3.3V supply symbol to the VDD pin.

This is why I always invoke and hook up the power symbols. It's also another

good reason to never use library components directly, but to copy them to

personal libraries and modify them if necessary, for example, to use a

consistent power rail naming scheme.

Bob

All,

Thanks very much for the detailed explanations and suggestions. These responses go well beyond what Eagle has written up in the manual as to "What needs to be done and this is how to do it" approach. The "Why" and history are very insightful as to the need for this Power and Supply definition. I hope others will benefit from what you've taken the time to explain.

Thank you so much,

David