Protel 99 sometimes seems to loose the net information on "connected copper tracks". Why it does this (or how I did this) I do not know, but it can be a little disturbing when you first come across this. (Actually, you can clear the "loaded nets", so I guess somehow ...)
Anyway, the fix, as pointed out to me on this forum several months ago, is to do the following Under "Design", select the "Netlist manager ..." >From the drop down menu on the bottom left of the dialog box that pops up, >there is a button marked as "Menu". ... click it. In the dialogs that pop up, one is "Update free primitives from component pads". Select it. Answer yes to the dialog that pops up. This will analyse the board, and re-apply the net names to the copper that connects between the pads. Of course, you really want to load the net list from the original PCB before you then try to compare with the new nets you now have after the changes. But, you might not have that anymore, so I guess you will have to tease mistakes out via the DRC, etc. The above should at least get you started down the right path Cheers Harry -----Original Message----- From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED] Behalf Of Abd ul-Rahman Lomax Sent: Friday, July 08, 2005 12:38 PM To: Protel EDA Discussion List Subject: Re: [PEDA] Protel 99SE update PCB errors. At 07:59 PM 7/7/2005, Brad Kosiance wrote: >Macro 1: New Node > >Add node CR3-2 to net NetR8_1 > >Error: Node not found Take a look at the actual footprint for the part. Quite likely you will discover that CR3 has no pin 2. Instead, perhaps, it has A or Anode (or C or K or Cathode). Likewise: >Macro 2: New Node > >Add node Q2-2,4 to net IOBUS+ > >Error: Node not found As I recall, some of the standard Protel parts showed this problem. Transistor pins can be named functionally in the schematic with names like E, B, C, or pin numbers can be used. Pin numbers, of course, are related to specific packaging, whereas names are functional and would correspond to different pin numbers. Basically, either change the schematic symbols or edit the PCB pads to have the appropriate pin names. Which one you should do depends on which one you find clearer. I do generally recommend that the PCB footprints be given numbers that correspond to actual pin layout. This can be a real mess with some parts, though, some three or four-pin discretes are numbered different ways by different manufacturers. And if the PCB footprints have numbers, the schematic symbols should also have numbers; the symbols should correspond to specific implementations of the part. Using generic symbols won't work very well when you want to translate it to PCB; if you use a generic transistor with pins named E,B,C, you have to have different PCB footprints for each variation. Better to have, for example, a single TO-92 footprint that works with all TO-92 parts, and use a specific symbol on the schematic that associates the proper pin numbers with the functions of the pins. ____________________________________________________________ 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] ____________________________________________________________ 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]
