Hello everyone ! I made a two layer pcb in which there are analog &
digital ics so , I made two gnd signals naming AGND & GND . Now I want to
connect these two signals at only at the gnd pin of power connector. When
I tried to naming these signals in Eagle I can give only one name to that
net , But don't want That ? I want separate signals.
The net lines on your schematic represent an electrical connection and once
you connect 2 nets together they are automatically merged into a single net
which can only have one name. Most, if not all, ECAD s/w works like that.
So, how do you solve the common problem of 2 or more ground nets that need
to be connected together at a single point? Well, here's how I do it, but
I'm not saying it's the best or the only solution 
- on the schematic, stick to separate nets and connect only one net to your
power pin (e.g. the GND net)
- on the schematic add a 2-pin jumper part, connect pin 1 to GND and pin 2
to AGND
- when routing the PCB, place the jumper with pin 1 as close as possible to
your power GND pin.
- route the entire board and run a DRC once finished, correct DRC errors if
any until the board is OK
- now "violate" the design rules by shorting pins 1 & 2 of the jumper. Be
aware that this will generate a DRC clearance error, but simply ignore it.
If you dont want to use the jumper principle just leave GND and AGND as 2
separate nets on the schematic and connect only GND to your power pin. When
routing the PCB, add a via with net name AGND somewhere close to the power
pin and route the AGND net, including the via. Again, when routed 100% and
DRC errors free, "violate" the design rules and connect AGND also to your
power pin by routing a trace from the via to the power pin. Alternatively,
delete the via and connect the open AGND track simply to the power pin.
If anybody here knows of a better or simplier way to solve this common
problem, I too would be very happy to hear about it
Cheers,
Robert
"Hemant" <mhamalhemant@gmail.com> wrote in message
news:g0bftc$1hj$1@cheetah.cadsoft.de...
Hello everyone ! I made a two layer pcb in which there are analog &
digital ics so , I made two gnd signals naming AGND & GND . Now I want to
connect these two signals at only at the gnd pin of power connector. When
I tried to naming these signals in Eagle I can give only one name to that
net , But don't want That ? I want separate signals.
"Hemant" <mhamalhemant@gmail.com> wrote in message
news:g0bftc$1hj$1@cheetah.cadsoft.de...
Hello everyone ! I made a two layer pcb in which there are analog &
digital ics so , I made two gnd signals naming AGND & GND . Now I
want to connect these two signals at only at the gnd pin of power
connector. When I tried to naming these signals in Eagle I can give
only one name to that net , But don't want That ? I want separate
signals.
Robert wrote:
The net lines on your schematic represent an electrical connection
and once you connect 2 nets together they are automatically merged
into a single net which can only have one name. Most, if not all,
ECAD s/w works like that.
So, how do you solve the common problem of 2 or more ground nets that
need to be connected together at a single point? Well, here's how I
do it, but I'm not saying it's the best or the only solution
- on the schematic, stick to separate nets and connect only one net
to your power pin (e.g. the GND net)
- on the schematic add a 2-pin jumper part, connect pin 1 to GND and
pin 2 to AGND
- when routing the PCB, place the jumper with pin 1 as close as
possible to your power GND pin.
- route the entire board and run a DRC once finished, correct DRC
errors if any until the board is OK
- now "violate" the design rules by shorting pins 1 & 2 of the
jumper. Be aware that this will generate a DRC clearance error, but
simply ignore it.
If you dont want to use the jumper principle just leave GND and AGND
as 2 separate nets on the schematic and connect only GND to your
power pin. When routing the PCB, add a via with net name AGND
somewhere close to the power pin and route the AGND net, including
the via. Again, when routed 100% and DRC errors free, "violate" the
design rules and connect AGND also to your power pin by routing a
trace from the via to the power pin. Alternatively, delete the via
and connect the open AGND track simply to the power pin.
If anybody here knows of a better or simplier way to solve this common
problem, I too would be very happy to hear about it
Cheers,
Robert
I've handled this by creating a library part with two pins in the schematic
symbol. For the footprint, I place two pads on top of each other (either
SMT or through-hole).
You can use this part in your schematic, connecting AGND to one pin and GND
to the other pin. In the layout, you will neatly get the pad with an air
wire to both AGND and GND, but no other air wires between AGND and GND.
Of course, DRC will complain loudly about the overlapping pads. I always
look through the list of errors, and ignore the ones relating to the
overlapping pads. WIth V5, you can now "approve" these errors so you only
have to look at them once.
Regards,
Bert Menkveld
