2
\$\begingroup\$

I'm working with a schematic in Eagle and I use IC's with different types of power pins. I connect VDD to VCC to +5V and I connect GND to VSS to zero volts.

When I look at the ERC, I receive warnings as follows:

WARNING: Sheet 1/1: POWER Pin IC1 VCC connected to VDD
WARNING: Sheet 1/1: POWER Pin IC1 GND connected to VSS
WARNING: Sheet 1/1: POWER Pin IC5 V+ connected to VDD
WARNING: Sheet 1/1: POWER Pin IC5 GND connected to VSS

When I switch over to PCB manufacturing mode, it seems that not all the pins are connected.

My schematic has a microcontroller, CMOS IC's and a 555 timer.

Do I need to add resistors between each of the different power supply designations? I'm trying to be legal so that no electrical software complains.

\$\endgroup\$
5
  • 1
    \$\begingroup\$ I think by "legal" you mean you're trying to eliminate all design rule check warnings. No regulatory body will worry about this. \$\endgroup\$
    – jbarlow
    Jul 15, 2016 at 6:25
  • \$\begingroup\$ Try renaming VDD rail to VCC and VSS to GND. Though such behaviour looks strange - you should be able to name your netnames the way you want to \$\endgroup\$
    – Artūras Jonkus
    Jul 15, 2016 at 6:28
  • \$\begingroup\$ Warnings are just that, warnings, not errors. \$\endgroup\$
    – Passerby
    Jul 15, 2016 at 6:28
  • \$\begingroup\$ related (possibly): How to attach a pin not shown on schematic symbol? \$\endgroup\$
    – Nick Alexeev
    Jul 15, 2016 at 6:38
  • \$\begingroup\$ See electronics.stackexchange.com/questions/56005/… \$\endgroup\$
    – Peter Smith
    Jul 15, 2016 at 10:41

1 Answer 1

Reset to default
3
\$\begingroup\$

In schematic editors, a 'net', that is a set of nodes connected together, has a name, and is identified by that name. Therefore the 'VCC' and 'VDD' nets are distinct. If a wire is used to connect them, this will cause a logical problem for the editor. Different editors have different behaviour in these circumstances. Some will automatically rename one net, some will leave the nets unconnected.

There are several solutions

a) Connect them by a component, such as a 0-ohm resistor. This is wasteful if the only reason is to get round net naming issues, though the odd 0-ohm link in power supplies can be handy for debugging, allowing various bits of the circuit to be isolated

b) Choose a unified net name as one of the comments suggests. Rename everything to 'VCC' or the like. I don't like this as labels like 'VCC' and 'VDD' already have semantic meaning, and can cause confusion with the data sheet, at least, they confuse me.

c) Name the nets on the board for what they are. I tend to filter supplies, so end up with nets called '+5v_in', '+4.8v_fil', '+4.5v_fil2' etc, so I know where I am.

\$\endgroup\$
2
  • 1
    \$\begingroup\$ VCC and VCC have no special meaning in Eagle. If net contains a pin of direction supply (like the little arrow or ground symbols have), it becomes a supply net. The only reason these warnings appear is that the symbol itself has pins that have a direction of power which is then connected to a supply net with a different name. You could give a pin named bob the direction of power if you wanted and it would then give warnings that bob is connected to supply net (hope it's not mains, otherwise poor Bob). If the supply net has the same name as the power pin, no warning is generated. \$\endgroup\$
    – Tom Carpenter
    Aug 3, 2016 at 21:52
  • \$\begingroup\$ Check the warnings to make sure the connection is correct, and if so click the Approve button. \$\endgroup\$
    – Tom Carpenter
    Aug 3, 2016 at 21:53

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge that you have read and understand our privacy policy and code of conduct.