Maker Pro
Maker Pro

PADS PCB won't length minimize GND rats

A

Andrew Holme

Jan 1, 1970
0
I want to use an old board as a starting point for a new one; but the old
one has a problem: length minimize doesn't work on the GND net. Other nets
are OK; but I'm getting lots of GND rats needlessly crisscrossing the board
after I ECO in the changes. The only way to get rid of them is to actually
route GND pins. Anyone seen this? I have other designs that are not
affected but I don't know what it is about this particular board.

TIA
 
snip


Are you routing gnds or using a plane? Lately, we use a "routing
layer" for the ground plane (not a "plane" layer) and draw in a copper
pour for GND. That seems to work better, less weird stuff, and gives
us more control over edges and cutouts and things.

Isn't it becoming more or less the standard way of diong it?
afaict the "plane" stuff is some historic leftover from using
tape where a plane was basically a inverted image of all the pads so
you didn't have to tape as much

all the layers being equal with tracks and pours seems much more
straight
forward

-Lasse
 
A

Andrew Holme

Jan 1, 1970
0
"John Larkin" wrote in message
I have seen a red-line ratsnest in PADS where all the GND runs on the
board converge on one seemingly arbitrary pin. It's very weird.

But I don't think we run the lenmin function at all. We just route.

The Brat who does our layouts turns off all the red connections, so
you can't see the unroutes at all. That entirely freaks me out, but
she does boards good and fast, so I can't complain. She just turned a
VXI crate controller into a VME crate controller in two days.

Are you routing gnds or using a plane? Lately, we use a "routing
layer" for the ground plane (not a "plane" layer) and draw in a copper
pour for GND. That seems to work better, less weird stuff, and gives
us more control over edges and cutouts and things.

Did you try

Setup / Design rules / Net / GND / Routing / Topology = minimized ?

That might do something.

Thanks. Topology was already showing as "minimized" in the GUI. And, yes,
I am using a copper pour in a routing layer for my ground plane.

After spending hours wrestling with this I may have found a fix.

I got around to playing with "Import" and "Export" and looking at the
differences between good and bad pcb files.
Just exporting connections and nothing else, good boards have:

*SIGNAL* GND 0 -2

in fact all signals, not just ground, have SIGFLAG=0 and COLOR=-2. Bad
boards have:

*SIGNAL* GND 2147483649 -2

and all other nets are 0 -2.

Exporting connections from a good file and importing into a bad file fixes
it with warnings about duplicate connections.

Editing the ASC file down to a one-liner just defining:

*SIGNAL* GND 0 -2

and importing that fixes it with no warnings.
 
N

Nico Coesel

Jan 1, 1970
0
Andrew Holme said:
I want to use an old board as a starting point for a new one; but the old
one has a problem: length minimize doesn't work on the GND net. Other nets
are OK; but I'm getting lots of GND rats needlessly crisscrossing the board
after I ECO in the changes. The only way to get rid of them is to actually
route GND pins. Anyone seen this? I have other designs that are not
affected but I don't know what it is about this particular board.

That sounds like a specific setting for the GND net in that design. I
don't know about Pads but the software I'm using allows me to use
several settings for reconnecting nets. Some result in exactly what
you are describing. So look at the properties of the GND net and
compare with other nets.
 
Top