Third manner/variation (still a manual edit) but a bit more manual for us
control freaks.
Use the (right-click) Select Connected Copper for each trace
individually and globally assign the netname to the selected traces. This gives
you the control over which traces are net renamed and you can appropriately
deal with connections that may no longer be needed or don't connect where they
should.
Where you have a net connection where some trace segments still have
the netname assigned (traces that continue past a previous pin), you can use
that trace segment to do the global net assignment to the selected segments and
not even have to enter the netname manually, just check the netname box while
doing the global edit.
Sincerely,
Brad Velander
Senior PCB Designer
Northern Airborne Technology
#14 - 1925 Kirschner Road,
Kelowna, BC, V1Y 4N7.
tel (250) 763-2329 ext. 225
fax (250) 762-3374
-----Original Message-----
From: Abd ul-Rahman Lomax [mailto:[EMAIL PROTECTED]
Sent: Friday, May 12, 2006 8:06 AM
To: Protel EDA Discussion List
Subject: Re: [PEDA] after Update ---> net-names lost
At 08:53 AM 5/12/2006, Jim McGrath wrote:
>It appears you need to "update free primitives from compomemt pads".
>Go To Design, Netlist Manager, Menu and select "update free primitives
>from compomemt pads".
Just to make it explicit, there are only two ways designed into
Protel 99SE (and, I think, later versions as well) to assign nets to
primitives.
One is directly, through edits, individual or global or similar.
This, obviously, will not be satisfactory.
The other is Update Free Primitives from Component Pads, as described
by Mr. McGrath. This command essentially clears out all Free
Primitive nets (as I recall) and then analyzes the pcb for
connectivity, assigning nets as it goes, until all nets have either
been assigned or have been found to be in conflict.
The component pads can get their nets, again, in two ways: by
individual edits or by load from schematic. The latter is highly
recommended, ordinarily component pad nets should be left alone and
all such changes made in the schematic. That way the net assignments
won't disappear next time a netlist is loaded from the schematic.
____________________________________________________________
You are subscribed to the PEDA discussion forum
To Post messages:
mailto:[email protected]
Unsubscribe and Other Options:
http://techservinc.com/mailman/listinfo/peda_techservinc.com
Browse or Search Old Archives (2001-2004):
http://www.mail-archive.com/[email protected]
Browse or Search Current Archives (2004-Current):
http://www.mail-archive.com/[email protected]
