PADS PCB won't length minimize GND rats

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.

snip

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

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:

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

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:

and importing that fixes it with no warnings.

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.

That's good to know.

PADS can be a little strange, but I expect that all PCB software has quirks. One good thing about PADS is that an entire design can be exported/imported in ASCII, which means you can text-edit or run scripts on those files. Sometimes just doing ASCII OUT then ASCII IN can clean things up. Overall, PADS is very good.

If anyone's interested, I wrote two PowerBasic programs for PADS.

PINK.EXE compares two netlists, PCB or SCH in any combination, better than PADS does.

BLUE.EXE compares our parts database against a schematic. It checks package types, values, and stock number against the PADS part attributes. Our stock listing is itself an ascii file, so it wouldn't be hard to adapt to other systems. We fill in all part attributes on a schematic and then use PADS Logic to make our BOMs, so BLUE is a good consistancy check.

That seems like the net has a flag active. That flag got enabled somewhere in the software.