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

I just wanted to illustrate the havoc it causes me.. This is just a tiny

part of my very long ERC list (8  pages long, and I have 1600 pixel high

screen). At least it could have merged alot of these warnings into one.

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

parts.  At least then all the pins are visible.

This is good advice. Unfortunately the "feature" also appears to strike PWR pins which are on the part (don't need to be invoked).

The specific case where I noticed it was adding a battery charger IC which has two PWR pins - "VDD", a generic power source (charge current set by resistor), and "VUSB" for USB port power (charge current 100mA/500mA selectable). One or the other may be left unconnected. Since my application charges from USB port power but the battery requires a custom charge current, I had USB power (appropriately enough named 'VUSB' in the schematic) tied to the VDD pin and the VUSB pin intentionally unconnected. This resulted in the VDD and VUSB pins of the IC being shorted together on the board, with the only indication being the teeny, tiny ratsnest wire between the adjacent pads. It was an extremely lucky catch!

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

Even not invoked Pwr pins will be connected.

I did a quick test today that seems to suggest (n=1 observations) that a PWR pin's auto-connected net will be disconnected again if a different-named net is subsequently wired to the PWR pin. Can you confirm wither the silently auto-connected pins will be (always, sometimes or never) disconnected again if a net with a different name is explicitly connected? Or will the two nets ever both remain connected and become shorted at that pin? (I.e. does the behavior I observed depend on what order the nets/part/connection were created, phase of the moon, etc.?)

Thanks!

Count me in! Again!

This stuff only makes my ERC more painful.

James Morrison wrote on Wed, 20 June 2012 11:37

And having connections done in the PCB that aren't shown in the

schematic is VERY BAD PRACTICE.  When I'm debugging a board I need to be

able to tell all of the exact connections.  The possibility of implicit

and hidden connections is enough for some companies to not even consider

EAGLE since it breaks internal design process requirements.  Having a SET

command that could turn this off would be a great compromise.

I totally agree.  It's really about time Cadsoft fixes this.  This has been

brought up by many people many times before.

--

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

Am 21.06.2012 07:24, schrieb Lorenz:

Andrew Sterian wrote:

>> On 6/20/12 11:37 AM, James Morrison wrote:

>>> CadSoft Support wrote on Wed, 20 June 2012 03:02

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

>>>> Even not invoked Pwr pins will be connected.

>>

>> Please do update EAGLE's approach for 2012: recognize that boards have

>> multiple voltages, there is no such thing as "VCC" anymore, and NOTHING

>> should be connected that is not visible on the schematic.

 

as it is best practice to create you own libraries, just don't use PWR

pins (only on power symbols).

 

I agree with Lorenz in creating/modifying my own libraries. I also use

the same names given in the data sheets incl. VDD,VSS etc. BUT I don't

use these names as supply in drawings and so there is no automatic

connection. And even if there is a fancy supply voltage like 2.347861

then there will be a new supply connected to the device VCC. I get a

warning and that is OK and accepted.

--

Mit freundlichen Grüßen / With best regards

Joern Paschedag

Andrew Sterian wrote:

>On 6/20/12 11:37 AM, James Morrison wrote:

>> CadSoft Support wrote on Wed, 20 June 2012 03:02

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

>>> Even not invoked Pwr pins will be connected.

>[...]

>Please do update EAGLE's approach for 2012: recognize that boards have

>multiple voltages, there is no such thing as "VCC" anymore, and NOTHING

>should be connected that is not visible on the schematic.

as it is best practice to create you own libraries, just don't use PWR

pins (only on power symbols).

--

Lorenz

On 6/20/12 11:37 AM, James Morrison wrote:

CadSoft Support wrote on Wed, 20 June 2012 03:02

>> 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......

>

I understand all of that Richard.  But electronics have evolved a bit in 20

years--maybe EAGLE should too!  20 years ago you might have had an entire

board powered by 5V so one rail called VCC was very useful.  Most boards I

do today have 5+ different power voltages so this is no longer the case.

 

And having connections done in the PCB that aren't shown in the schematic

is VERY BAD PRACTICE.  When I'm debugging a board I need to be able to tell

all of the exact connections.  The possibility of implicit and hidden

connections is enough for some companies to not even consider EAGLE since

it breaks internal design process requirements.  Having a SET command that

could turn this off would be a great compromise.

 

James.

Fully agree. Every one of my designs has numerous ERC errors that say

"Warning: Power pin VDD connected to +3.3V" or something like that

because I don't know what the voltage will be on the "VDD" pin: it could

be 2.5V, 3.3V, sometimes, 5V, etc. So many frivolous errors hides the

real errors.

And James is completely right: "having connections done in the PCB that

aren't shown in the schematic is VERY BAD PRACTICE".

Please do update EAGLE's approach for 2012: recognize that boards have

multiple voltages, there is no such thing as "VCC" anymore, and NOTHING

should be connected that is not visible on the schematic.

Andrew.

CadSoft Support wrote on Wed, 20 June 2012 03:02

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......

I understand all of that Richard.  But electronics have evolved a bit in 20

years--maybe EAGLE should too!  20 years ago you might have had an entire

board powered by 5V so one rail called VCC was very useful.  Most boards I

do today have 5+ different power voltages so this is no longer the case.

And having connections done in the PCB that aren't shown in the schematic

is VERY BAD PRACTICE.  When I'm debugging a board I need to be able to tell

all of the exact connections.  The possibility of implicit and hidden

connections is enough for some companies to not even consider EAGLE since

it breaks internal design process requirements.  Having a SET command that

could turn this off would be a great compromise.

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/

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.