ERC: WARNING: Sheet 1/1: SUPPLY Pin +UB overwritten with VCC

[Reed Bement]

I have two issues I'm trying to deal with. My ERC output is below:



EAGLE Version 4.11 Copyright (c) 1988-2003 CadSoft

Electrical Rule Check for C:/Program Files/EAGLE-4.11/projects/interface.sch
at 5/15/2007 06:01:15a

WARNING: Sheet 1/1: unconnected Pin: CN2-3 S
WARNING: Sheet 1/1: SUPPLY Pin +UB overwritten with VCC

Pins/Pads with different connections:

Part Gate Pin Net Pad Signal

U8 /+UB +UB VCC 16 +UB

ERROR: Inconsistency with implicit power pins (see the above list)!

1 errors
2 warnings



1. Is there an elegant way to deal with unconnected pins on a connector? The
connector is from the con-amp-mt library, perhaps there is something about
the way it was created?

2. I have power pins on IC's from two different libraries which use VCC and
+UB for the signal names of the power pin. Both are +5VDC. How can I connect
them cleanly without generating errors in ERC?

I've searched the help and FAQ's, but found nothing on these issues. Any
ideas?

Thanks,
-Reed

[futrtrubl]

On Tue, 15 May 2007 06:19:54 -0700, "Reed Bement"

Post by Reed Bement
EAGLE Version 4.11 Copyright (c) 1988-2003 CadSoft
Electrical Rule Check for C:/Program Files/EAGLE-4.11/projects/interface.sch
at 5/15/2007 06:01:15a
WARNING: Sheet 1/1: unconnected Pin: CN2-3 S
WARNING: Sheet 1/1: SUPPLY Pin +UB overwritten with VCC
Part Gate Pin Net Pad Signal
U8 /+UB +UB VCC 16 +UB
ERROR: Inconsistency with implicit power pins (see the above list)!
1 errors
2 warnings
1. Is there an elegant way to deal with unconnected pins on a connector? The
connector is from the con-amp-mt library, perhaps there is something about
the way it was created?
2. I have power pins on IC's from two different libraries which use VCC and
+UB for the signal names of the power pin. Both are +5VDC. How can I connect
them cleanly without generating errors in ERC?
I've searched the help and FAQ's, but found nothing on these issues. Any
ideas?
Thanks,
-Reed

In both of these they are warnings not errors, so they can be safely
ignored once you make sure that you did what you meant to do.

Edward

[David Moodie]

Post by Reed Bement
EAGLE Version 4.11 Copyright (c) 1988-2003 CadSoft
Electrical Rule Check for C:/Program Files/EAGLE-4.11/projects/interface.sch
at 5/15/2007 06:01:15a
WARNING: Sheet 1/1: unconnected Pin: CN2-3 S
WARNING: Sheet 1/1: SUPPLY Pin +UB overwritten with VCC
Part Gate Pin Net Pad Signal
U8 /+UB +UB VCC 16 +UB
ERROR: Inconsistency with implicit power pins (see the above list)!
1 errors
2 warnings
1. Is there an elegant way to deal with unconnected pins on a connector? The
connector is from the con-amp-mt library, perhaps there is something about
the way it was created?
2. I have power pins on IC's from two different libraries which use VCC and
+UB for the signal names of the power pin. Both are +5VDC. How can I connect
them cleanly without generating errors in ERC?
I've searched the help and FAQ's, but found nothing on these issues. Any
ideas?
Thanks,
-Reed

As has been noted the warnings are nothing to worry about. Eagle is just
checking things and reminding you about them so that you can look out for
any problems. You as the designer can choose to modify the design or ignore
the warnings.

If you really want to get rid of unconnected pins then add in a test pad
from the pin... then it is no longer unconnected.

To get rid of the supply pin warning you would need to edit the relevant
library and change the supply pin name from +UB to VCC... but it might not
be universally correct .. this is a decision for you to take. With larger
designs you will generally always have some issues with supply pin names.

What Eagle really needs to do here is have a facility to check these
warnings once you've OK'd them so they don't appear again..

Do you know what to do about your ERROR?

the classic case when inconsistencies appear is that the brd and sch files
have been edited separately. In this case it looks like you opened the sch
added vcc to the +UB pin, and then opened the brd.

THE GOLDEN RULE IS ALWAYS EDIT ENSURE SCH AND BRD FILES ARE BOTH OPEN.
(after initial sch entry and brd creation)

To correct the error rename the net in the brd window to match the sch net name.

cheers

David

[Reed Bement]

David you are quite correct. The error was due to inconsistent board and
schematic. I ended up having to abandon the board and start over because I
couldn't bring them together again. I had no problem fixing up parts
(matching names and values) but I couldn't figure out how to add nets on
the board side. This may be part of the back-anno limitation on my version
of Eagle, or it may be that I'm missing something...

Thanks,
-Reed

Post by David Moodie

Post by Reed Bement
EAGLE Version 4.11 Copyright (c) 1988-2003 CadSoft
Electrical Rule Check for C:/Program
Files/EAGLE-4.11/projects/interface.sch at 5/15/2007 06:01:15a
WARNING: Sheet 1/1: unconnected Pin: CN2-3 S
WARNING: Sheet 1/1: SUPPLY Pin +UB overwritten with VCC
Part Gate Pin Net Pad Signal
U8 /+UB +UB VCC 16 +UB
ERROR: Inconsistency with implicit power pins (see the above list)!
1 errors
2 warnings
1. Is there an elegant way to deal with unconnected pins on a connector?
The connector is from the con-amp-mt library, perhaps there is something
about the way it was created?
2. I have power pins on IC's from two different libraries which use VCC
and +UB for the signal names of the power pin. Both are +5VDC. How can I
connect them cleanly without generating errors in ERC?
I've searched the help and FAQ's, but found nothing on these issues. Any
ideas?
Thanks,
-Reed

As has been noted the warnings are nothing to worry about. Eagle is just
checking things and reminding you about them so that you can look out for
any problems. You as the designer can choose to modify the design or
ignore the warnings.
If you really want to get rid of unconnected pins then add in a test pad
from the pin... then it is no longer unconnected.
To get rid of the supply pin warning you would need to edit the relevant
library and change the supply pin name from +UB to VCC... but it might not
be universally correct .. this is a decision for you to take. With larger
designs you will generally always have some issues with supply pin names.
What Eagle really needs to do here is have a facility to check these
warnings once you've OK'd them so they don't appear again..
Do you know what to do about your ERROR?
the classic case when inconsistencies appear is that the brd and sch files
have been edited separately. In this case it looks like you opened the sch
added vcc to the +UB pin, and then opened the brd.
THE GOLDEN RULE IS ALWAYS EDIT ENSURE SCH AND BRD FILES ARE BOTH OPEN.
(after initial sch entry and brd creation)
To correct the error rename the net in the brd window to match the sch net name.
cheers
David

[David Moodie]

Post by Reed Bement
David you are quite correct. The error was due to inconsistent board and
schematic. I ended up having to abandon the board and start over because I
couldn't bring them together again. I had no problem fixing up parts
(matching names and values) but I couldn't figure out how to add nets on
the board side. This may be part of the back-anno limitation on my version
of Eagle, or it may be that I'm missing something...
Thanks,
-Reed

If forward/back annotation is broken then you can add nets in the brd window
using the signal command (from pin to pin) or you can simply draw a wire
from the relevant pad and then name it appropriately.... normally you never
need this as you NEVER work on sch or brd alone.

The other option that I forgot to mention of course is that Eagle creates
back up files and you can roll back to one of these versions. (e.g. B#1,
extension).

cheers

David