Bug? Library part pins silently autoconnected to matching schematic net names

Tim Gipson wrote on Tue, 19 June 2012 10:50

Hi,

Ran into this strange and potentially dangerous behavior today in EAGLE

6.0.0 / 6.2.0. If a pin in a library symbol has direction 'Pwr' (possibly

others?), if a net with the same name exists in the schematic, the pin is

being automatically and silently connected in the Board editor (no

visible connection or other indication of this being the case in the

Schematic editor). No questions asked, no warnings, no way to 'undo'

(except by deleting the offending part / rolling back to a point before

the part was introduced, renaming the net, and re-importing the part). If

this has occurred, connecting the actually intended net (if any) to the

pin in the Schematic editor results in shorting the nets together in the

Board editor.

 

The fact that only certain pins (notably 'Pwr') are affected suggests

this dangerous behavior may be intentional. Is there any way to a)

disable this behavior, b) generate a loud warning whenever it is

triggered, and/or c) undo the behavior when it is triggered?

 

Some specific objections to this being a default behavior:

• Many library part authors (really, many part manufacturers, who

library part authors dutifully copy) use power pin names such as

Vin/Vcc/Vdd/V+ somewhat interchangeably; these names do not uniquely

refer to any voltage standard

• Many schematic authors (including more than one at my day-job)

sometimes use the default names for the 'supply' symbols to designate

different power nets on mixed-voltage boards (e.g. the 'Vcc' symbol for

5V and 'Vdd' symbol for 3.3V), wreaking havoc with the previous case. You

would never know your part is being overvolted by this behavior (silently

connected to wrong supply), or your supply nets are shorted together,

without careful visual inspection of the ratsnest lines.

• Likewise for ground splitting - I presume (but have not yet tested) a

Pwr pin named 'GND' will exhibit the same behavior, causing a problem

where e.g. a specific part of the circuit requires a split ground (e.g.

AGND), where elsewhere in the design, a library part that does not need,

and should not use the elsewhere AGND offers GND/AGND pins. GND/AGND will

then be shorted together at the 2nd location.

• Nets connected in the Board / design but explicitly shown as

unconnected in the schematic - this should never happen!

Hello Tim,

This is not a bug, it's a feature!  I know you've heard that before but

this is actually intended.  Now I agree with you that nothing should ever

be connected in the PCB that isn't explicitly drawn on the schematic.  But

this is how EAGLE does it.

From the help for the "PIN" command:

Quote:

If Pwr pins are used on a symbol and a corresponding Sup pin exists on

the schematic, nets are connected automatically.

My solution is to never, ever, use parts without invoking all gates on all

parts.  At least then all the pins are visible.

I would like to see a switch to disable this behaviour.  Perhaps an entry

for the SET command.  CadSoft?

Cheers,

James.

--

James Morrison  ~~~  Stratford Digital

Specializing in CadSoft EAGLE

• Online Sales to North America

• Electronic Design Services

• EAGLE Enterprise Toolkit

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

Tim Gipson wrote on Tue, 19 June 2012 10:50

Hi,

Ran into this strange and potentially dangerous behavior today in EAGLE

6.0.0 / 6.2.0. If a pin in a library symbol has direction 'Pwr' (possibly

others?), if a net with the same name exists in the schematic, the pin is

being automatically and silently connected in the Board editor (no

visible connection or other indication of this being the case in the

Schematic editor). No questions asked, no warnings, no way to 'undo'

(except by deleting the offending part / rolling back to a point before

the part was introduced, renaming the net, and re-importing the part). If

this has occurred, connecting the actually intended net (if any) to the

pin in the Schematic editor results in shorting the nets together in the

Board editor.

 

The fact that only certain pins (notably 'Pwr') are affected suggests

this dangerous behavior may be intentional. Is there any way to a)

disable this behavior, b) generate a loud warning whenever it is

triggered, and/or c) undo the behavior when it is triggered?

 

Some specific objections to this being a default behavior:

• Many library part authors (really, many part manufacturers, who

library part authors dutifully copy) use power pin names such as

Vin/Vcc/Vdd/V+ somewhat interchangeably; these names do not uniquely

refer to any voltage standard

• Many schematic authors (including more than one at my day-job)

sometimes use the default names for the 'supply' symbols to designate

different power nets on mixed-voltage boards (e.g. the 'Vcc' symbol for

5V and 'Vdd' symbol for 3.3V), wreaking havoc with the previous case. You

would never know your part is being overvolted by this behavior (silently

connected to wrong supply), or your supply nets are shorted together,

without careful visual inspection of the ratsnest lines.

• Likewise for ground splitting - I presume (but have not yet tested) a

Pwr pin named 'GND' will exhibit the same behavior, causing a problem

where e.g. a specific part of the circuit requires a split ground (e.g.

AGND), where elsewhere in the design, a library part that does not need,

and should not use the elsewhere AGND offers GND/AGND pins. GND/AGND will

then be shorted together at the 2nd location.

• Nets connected in the Board / design but explicitly shown as

unconnected in the schematic - this should never happen!

Hello Tim,

This is not a bug, it's a feature!  I know you've heard that before but

this is actually intended.  Now I agree with you that nothing should ever

be connected in the PCB that isn't explicitly drawn on the schematic.  But

this is how EAGLE does it.

From the help for the "PIN" command:

Quote:

If Pwr pins are used on a symbol and a corresponding Sup pin exists on

the schematic, nets are connected automatically.

My solution is to never, ever, use parts without invoking all gates on all

parts.  At least then all the pins are visible.

I would like to see a switch to disable this behaviour.  Perhaps an entry

for the SET command.  CadSoft?

Cheers,

James.

--

James Morrison  ~~~  Stratford Digital

Specializing in CadSoft EAGLE

• Online Sales to North America

• Electronic Design Services

• EAGLE Enterprise Toolkit

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

On 19.06.2012 17:13, James Morrison wrote:

Tim Gipson wrote on Tue, 19 June 2012 10:50

>> Hi,

>> Ran into this strange and potentially dangerous behavior today in EAGLE

>> 6.0.0 / 6.2.0. If a pin in a library symbol has direction 'Pwr' (possibly

>> others?), if a net with the same name exists in the schematic, the pin is

>> being automatically and silently connected in the Board editor (no

>> visible connection or other indication of this being the case in the

>> Schematic editor). No questions asked, no warnings, no way to 'undo'

>> (except by deleting the offending part / rolling back to a point before

>> the part was introduced, renaming the net, and re-importing the part). If

>> this has occurred, connecting the actually intended net (if any) to the

>> pin in the Schematic editor results in shorting the nets together in the

>> Board editor.

>>

>> The fact that only certain pins (notably 'Pwr') are affected suggests

>> this dangerous behavior may be intentional. Is there any way to a)

>> disable this behavior, b) generate a loud warning whenever it is

>> triggered, and/or c) undo the behavior when it is triggered?

>>

>> Some specific objections to this being a default behavior:

>> * Many library part authors (really, many part manufacturers, who

>> library part authors dutifully copy) use power pin names such as

>> Vin/Vcc/Vdd/V+ somewhat interchangeably; these names do not uniquely

>> refer to any voltage standard

>> * Many schematic authors (including more than one at my day-job)

>> sometimes use the default names for the 'supply' symbols to designate

>> different power nets on mixed-voltage boards (e.g. the 'Vcc' symbol for

>> 5V and 'Vdd' symbol for 3.3V), wreaking havoc with the previous case. You

>> would never know your part is being overvolted by this behavior (silently

>> connected to wrong supply), or your supply nets are shorted together,

>> without careful visual inspection of the ratsnest lines.

>> * Likewise for ground splitting - I presume (but have not yet tested) a

>> Pwr pin named 'GND' will exhibit the same behavior, causing a problem

>> where e.g. a specific part of the circuit requires a split ground (e.g.

>> AGND), where elsewhere in the design, a library part that does not need,

>> and should not use the elsewhere AGND offers GND/AGND pins. GND/AGND will

>> then be shorted together at the 2nd location.

>> * Nets connected in the Board / design but explicitly shown as

>> unconnected in the schematic - this should never happen!

>

Hello Tim,

 

This is not a bug, it's a feature!  I know you've heard that before but

this is actually intended.  Now I agree with you that nothing should ever

be connected in the PCB that isn't explicitly drawn on the schematic.  But

this is how EAGLE does it.

 

From the help for the "PIN" command:

 

Quote:

>> If Pwr pins are used on a symbol and a corresponding Sup pin exists on

>> the schematic, nets are connected automatically.

>

My solution is to never, ever, use parts without invoking all gates on all

parts.  At least then all the pins are visible.

 

I would like to see a switch to disable this behaviour.  Perhaps an entry

for the SET command.  CadSoft?

 

Cheers,

 

James.

Hello Tim, James,

EAGLE connects Pwr pins with same names automatically, that's true.

Even not invoked Pwr pins will be connected.

To have this all under control EAGLE runs several checks (ERC).

For each Pwr signal in the schematic EAGLE wants you to place a

supply pin on every sheet.

ERC message: "No supply for power pin xxxxx" helps in identifying

pwr signals. And there are additional checks on Pwr signals.

That's the way EAGLE works for about 20 years now......

--

Mit freundlichen Gruessen / Best regards

Richard Hammerl

  CadSoft Support -- hotline@cadsoft.de

  FAQ: http://www.cadsoft.de/training/faq/