At 02:36 PM 12/21/2001 +1100, Thomas wrote: >I have a 5 sheet project that I was planning to put on one PCB. >However It has become clear that there is no way all the parts are going to >fit in the space available. > >To solve this I will have to stack 2 PCBs (there are mounting slots provided >for two PCBs in the enclosure). > >The problem is that the most efficient way to do this requires all the >display parts on one PCB - the rest on the other. Unfortunately this is not >the way the schematic sheets are arranged. So it will be impossible to get a >netlist for individual PCBs.
What you want here is one schematic and 2 PCBs. Not necessarily a great idea unless the boards are truly conjoined twins, which is not the case if I understand the description (two "mounting slots") >What I was planning to do was draw the two pcbs in one file connected >together and have a perforation or groove for splitting the two pcbs. You could do this. In this case, you have not two pcbs but one. Only they get cut apart and the tracks cut replaced by ribbon. If you like, the interconnection tracks could be on a non-fabricated inner layer, so you won't even have the embarrassment of cut copper at the board edge. > Placing correctly sized vias on a 2.54mm pitch for PCB interconnections on >both PCBs should allow me to use a ribbon cable from another one of our >standard products. Don't do it that way. Instead, add connectors to the schematic, two of them, matching the ribbon, even if the "connectors" are only a hole pattern for flat flexible cable or the like. A pattern of "correctly sized vias" I would call a "footprint," and you can control this from the schematic if you place connector symbols.... Plus you probably already have the footprint from your other standard product. >I plan to annotate the schematics showing which parts are on the second PCB. > >All this should still be quicker than redrawing the project. You are going to have to decide what parts go on what PCB, and then ensure that the relevant signals communicate on the ribbon. That takes time. You might as well split the design into two parts. Seriously, that is probably the easiest way to do this. I recommend this: take your existing schematic, and save it with a different name. Then split the original design into two schematics, you can use select, cut and paste to move parts and interconnection information from one to the other. Be careful about multipart ICs, if you have any! Be sure to place the interboard connectors, one on each schematic; it may be best to assign nets to the pins with net labels. When you are done, add the two connectors with their net labels to the original schematic and generate a net list, I'll call it original.net. You will probably want to use net labels and ports global. If you have used some other scope for your original schematic, things get more complicated, I won't address that here. Take your individual schematics and link them through a top-level project schematic. Make a project netlist, I'll call it split.net. Once again, net labels and ports global. Use the Protel netlist comparison tool (It's under Reports in Schematic) to prove to yourself that both netlists are identical. If they are not, you have something to fix.... Then design each PCB, one from each of the individual, non-linked schematics. At this point you can choose to fab them separately or together. (If you fab them together, you may want to add the dummy interconnections on an unused inner layer I mentioned above, that way the whole design will DRC properly). If later you change one of them, you can just fab one instead of being forced to fab both at higher cost. Also, with the individual sheets, you will be able to generate a BOM for each board, pick and place, etc. [EMAIL PROTECTED] Abdulrahman Lomax Easthampton, Massachusetts USA * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
