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://firstname.lastname@example.org * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *