Used Power instead of Supply on parts

John Bachman wrote on Fri, 18 December 2009 12:54

I have my schematic all done and have discovered that I should have

used

Supply for ground connections to some of the ICS.

I don't understand what you mean by "using Supply for ground connections".

You need to connect the ground pins to whatever net you want them connected

to.

Quote:

ERC comes up with an

error in places where I connected Vss to GND.

Eagle complains when the net name connected to a power pin doesn't match

the pin name.  Even worse, it will automatically connect a unconnected

power pin to a net of the same name.  Argh!!

Make sure all power pins are explicitly connected in the schematic, then

"approve" the ERC errors complaining about a name mismatch between the pin

and the net.  Unfortunately you have to pay attention because there could

be a real error lurking in the pile of nuisance warnings.

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

John Bachman schrieb:

I have my schematic all done and have discovered that I should have used

Supply for ground connections to some of the ICS.  ERC comes up with an

error in places where I connected Vss to GND.  Do I need to go back and

correct every part or can I just ignore the ERC warnings?

Pin direction "supply" is for those pins that provide power, like within

the GND and VCC symbols. The name of a net connected to that pin will

implicitly taken from the pin name (if possible).

Pin direction "power" is for those pins that need to be connected to a

power source, like the power supply pins of ICs.

ERC will warn you if you connect different supply pins to one net (which

can only have one name, so that's a conflict). ERC will also warn you if

you don't connect the correctly named net to a power pin of any device.

Besides that, only the net names and their connections are really

relevant. You might as well remove all power supply symbols and just

name your nets correctly (take care of implicit power gates!).

If you use different IC families with the same supplies, ERC will always

report many warnings, since the power pins of the devices are named

differently (i.e. GND, VSS or V-) but are connected to a single net.

You can safely ignore these warnings as long as you know that these

connections are really wanted in your design.

Tilmann

On 12/18/2009 2:41 PM, Olin Lathrop wrote:

John Bachman wrote on Fri, 18 December 2009 12:54

I have my schematic all done and have discovered that I should have

used Supply for ground connections to some of the ICS.

 

I don't understand what you mean by "using Supply for ground

connections". You need to connect the ground pins to whatever net you

want them connected

to.

 

Quote:

ERC comes up with an error in places where I connected Vss to GND.

 

Eagle complains when the net name connected to a power pin doesn't match

the pin name. Even worse, it will automatically connect a unconnected

power pin to a net of the same name. Argh!!

 

Make sure all power pins are explicitly connected in the schematic, then

"approve" the ERC errors complaining about a name mismatch between the pin

and the net. Unfortunately you have to pay attention because there could

be a real error lurking in the pile of nuisance warnings.

To clarify: When creating new components one can choose the type of pin.

  For all pins that are power supply or ground I chose "Power".  It

appears that Eagle would be happier if I chose "Supply" for the pins

that I will connect to a ground.  Hence my question which I think that

another poster has answered.

--

John Bachman, W1JGB

AnaTek Corporation

John Bachman wrote on Sat, 19 December 2009 07:17

To clarify: When creating new components one can choose the type of

pin.

Actually it's called the pin "direction".  Apparently when you said "used

Supply for ground connections" you really meant "set the pin direction of

ground pins to Supply".  This was not clear.

Quote:

For all pins that are power supply or ground I chose "Power".

Here's a heretical thought: Use the pin directions as intended and clearly

documented.  The Supply pin direction is for pins that produce supply

rails, like the output of a voltage regulator or a ground symbol.  Power is

for pins that are expected to be connected to a supply rail, like Vdd and

Vss pins of a CMOS chip.

Quote:

It appears that Eagle would be happier if I chose "Supply" for the pins

that I will connect to a ground.

No, you should use Supply for the single ground symbol and Power for the

ground pins of the various parts connected to the ground net.

Again, this is all clearly documented.  Try HELP PIN.  It may correct a few

more unfortunate guesses.

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca