error Message due to overwriting of Pin GND

Am 29.06.2012 12:33, schrieb Patrick Seebörger:

Hi

 

I get the following error message when I am working with EAGLE for my DC motor control.

I  need several ground connections so I took always the same symbol and changed its name and the name of its path.

Then I got this error message:

SUPPLY-Pin GND überschrieben mit mehr als einem Signal (DGND, AGND, GND_EXT, GND, GND_DRIVER)

Supply- Pin GND overwriting with more than one signal ((DGND, AGND, GND_EXT, GND, GND_DRIVER)

 

Do I have to care about it or did I everything right?

 

Thanks

 

A warning means that the user must check that item.

I don't understand your problem really. If you have just one common gnd

then why give it different names? Different names mean different gnds.

agnd and dgnd and gnd are three different gnds in this example. If you

don't find the "right" gnd then create a new one and name it for your suits.

--

Mit freundlichen Grüßen / With best regards

Joern Paschedag

I need different GNDs and VCCs which may not be connected to each other.

If I give the GND a new name EAGLE always asks if it shall connect GND with AGND ... so in the end I will not

have different Grounds because all GNDs will be connected together!?

Thanks.

On 29/06/2012 13:21, Patrick Seebörger wrote:

I need different GNDs and VCCs which may not be connected to each other.

If I give the GND a new name EAGLE always asks if it shall connect GND with AGND ... so in the end I will not

have different Grounds because all GNDs will be connected together!?

 

Thanks.

 

I second that query. I have the same problem with separate digital and

analog grounds that should only be connected at a specified single

location. Is the only way to do this, to manually add a link on the PCB

at the routing stage? (resulting in copious warnings).

    Thanks for the interest

        Andrew

On 06/29/2012 09:53 AM, Andrew Forrest wrote:

On 29/06/2012 13:21, Patrick Seebörger wrote:

>> I need different GNDs and VCCs which may not be connected to each other.

>> If I give the GND a new name EAGLE always asks if it shall connect GND

>> with AGND ... so in the end I will not

>> have different Grounds because all GNDs will be connected together!?

>>

>> Thanks.

>>

 

I second that query. I have the same problem with separate digital and

analog grounds that should only be connected at a specified single

location. Is the only way to do this, to manually add a link on the PCB

at the routing stage? (resulting in copious warnings).

 

   Thanks for the interest

       Andrew

 

The best way to solve this is to create a part in your library called

"SHORT".  The symbol should have two pins, both passive, that connect to

each other.  The layout should have two SMD pads that overlap slightly.

If you wish you can create several such packages with different SMD pad

widths.  If you wish, you can modify the SMD pads to turn the cream and

mask off.

Use the SHORT device in your schematic to connect one ground to another,

just as if it were a would a zero-ohm resistor.

In your layout, place the SHORT component close to where you wish to

connect the two separate grounds together, then route the air wires.

The SHORT serves to connect two different nets.  AGND/DGND, or

3.3A/3.3D, or whatever you want to connect.  Thus, the nets stay

separate in Eagle and are treated as such.

The only downside is that a DRC will show an overlap error.  If you

choose to approve this error, DRC won't bother you with it again until

you move the short.

I believe Olin has published a SHORTS library for this very purpose.  If

you can't find it, you should be able to create the

symbol/device/package in less time than you'd spend searching for and

downloading the library.

Attached is a library containing an example of a short.

Enjoy,

    - Chuck