Power and Supply Pin Use on Schematics

Question

I've created a schematic design for a digital circuit with an isolated RS422 section. I'm using an isolating power supply for the transceivers and bringing the data lines onto the main board using an optoisolator. From that point, the rest of the board has common power and grounds. I'm using polygons with different names for GND on each section.

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)

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.

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?

Slight mess! Yes, VDD has no net as it will generate more errors if I connect it to +5v.

I appreciate your time and suggestions!

Warm regards.

dukepro · Accepted Answer

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

dukepro · Answer

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

autodeskguest · Answer

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