At 05:49 PM 5/3/2002 +0200, Rene Tschaggelar wrote:
>I have unassigned tracks (no net) and would like to proagate
>the connected net.
>In schematic there is a 'design/update pcb' that has a checkbox
>for 'Assign net to connected copper'. That somewho does not appear
>to work.

It should. It is possible, however, I'd think, to feed this command 
situations that it cannot digest. Most notable would be a short condition. 
Obviously, if two component pins with different nets assigned are connected 
together, Protel will not be able to determine easily which net to assign 
to connected primitives. As I recall, it will assign nets until it 
encounters the conflict and it will then abort assignments for that net, 
leaving the rest of the copper unassigned. Since it could encounter the 
conflict almost immediately, almost all the copper in the net could remain 
unassigned.

>Now ( in pcb editor )  I have do :
>-edit/select connected copper
>-read the netname from the source
>-doubleclick one new track item
>-change net to new net with global, selection same
>
>Is that all possible on one click per track ?

No. At least I don't think so. A cumbersome and complex solution has been 
outlined, and I don't even think it would work as described. I don't think 
that is the way to solve this problem, it is much simpler than that.

>Is that possible on one click for the whole board ?

Not one click, but a few, and perhaps a little detective work.

I don't know what condition the board is in, so what I will describe may be 
more involved than necessary; I have to assume that it is quite a mess....

I'd start by running, in PCB, Design/Netlist Manager/Menu/Update Free 
Primitives from Component Pads.

then run DRC with Short Circuit Constraints checked, and nothing else. Fix 
any shorts.

It may be a bit tricky; I think that the Short Circuit Constraints report 
will  include No-Net track connected to anything with a net assignment. If 
there is too much noise like this, I'd do the following:

Run PCB:Design/Netlist Manager/Menu/Create Netlist from Connected Copper. 
 From your Schematic, run SCH:Design/Create Netlist.

(Presumably you know how to set up the scope options for netlist creation....)

Then use SCH:Reports/Netlist Compare to compare the two net lists. You may 
be able to find the shorts quickly this way.

Once the shorts are removed, Update should work, whether it is run directly 
in PCB or through the Synchronizer.

If not, save the file (so that it may be possible for someone else to look 
at it, perhaps after removing proprietary information, if any) and ask us 
again.... If there is still an issue, one or more of us may volunteer to 
receive the file, please don't send it to the list!

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to