Steve - Can't say for sure without seeing your schematic, but here is my guess.

You are using Sheet Symbols/Port Connections for your netlist scope and your top sheet has one or more GND net labels that are not attached to a GND power port. Therefor you get two GND nets. If you change your netlist scope to Net Labels & Ports Global, the two ground nets will merge to one (but this may also cause other nets to merge that you don't want merged). The quickest way to resolve the problem is to place GND net label on a short wire and also connect a GND power port to the same wire. This will essentially merge your local GND net with your global GND power port net.

As far as trace is concerned, never used it so I can't be of much help there.


At 05:49 AM 6/1/2004, you wrote:
I've seen the toggling macros that result from having two pins with the same
number, where they are alternately added and deleted from the connections with
successive netlist loads. This is similar, but slightly different.

I have built a common-mode choke schematic symbol, with 4 pins each of type
Passive. I've checked in the list panel and there are no duplicate pins.
Looking at the part in the library editor, there are no "inside-out" pins. Likewise
the corresponding PCB footprint has exactly four pads, no duplicates, and no
funny-business on any of them.

I'm still in the habit of explicitly creating the netlist from schematic, and
explicitly loading the netlist in the PCB. Each time I do so, in addition to
any macros I expect, I also get two extras: the first removes pin 3 of that
chocke from its net (Gnd), and the second adds it back to the same net. There
are no errors noted. Executing the netlist load causes no adverse effects but
works just as would be expected. But then immediately reloading the same netlist
(which should result in no changes) produces those same two stray macros.

This doesn't directly impact the board I'm laying out, as the net connections
end up correct. But I've learned the hard way not to ignore it when Protel
does oddball, unexpected things - it's trying unsuccessfully to warn me about
some glitch that, sooner or later, will rear its ugly head in a defective batch
of boards. Does anybody here have any thoughts on what I should be looking

Anticipating the first suggestion, I just tried using Schematic's <Design> - <
Update PCB>. Exactly the same result.

In moving the design forward, I added two grounded mechanical holes, by
adding two "Testpoint"s on the schematic (single pin component I've used since
antiquity) and grounding them there. Now I get three pairs of these stray macros -
a pair each for pin 3 of the choke and pin 1 (only pin) of the two new
testpoints. The only thing in common is that all three are connected to ground. But
no other grounded pins (about a hundred) show any anomalies.

Uh-oh, I may be on the track of something here. I just discovered that there
are two GND nets in my netlist. Using explicit sheet-port connectivity, but
GND power symbols should be common regardless. One GND net relates to the
top-level sheet and three subsheets; the other net seems to be all the GND
connections for the most recently-created sheet, which is properly nested under the top
sheet in the Explorer panel. In trying to turn on the trace option of the
Schematic netlist generator, it claims to generate a trace file called
filename.tng. But there's no such file on my system after running the netlist, and
indeed no recently generated files that could be the output.

I'm wandering further and further afield from getting this job out the door,
which has to happen in the next couple of days. Basic issues I need to
address, then, are:

1) The split GND net MUST be fixed somehow.
2) The stray remove / add macros might be hinting at something dangerous.
3) I can't find the netlist generator trace output.

Any and all hints welcome!! Thanks!!

Steve Hendrix

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To post a message: mailto:[EMAIL PROTECTED] * * To leave this list visit: * * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * * * Browse or Search previous postings: *[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to