Re: [PEDA] Project woes
At 11:44 AM 12/28/2001 +1100, Thomas wrote: Someone recently posted a question to this list, asking weather a schematic should represent the electrical or physical layout, I was of the firm opinion - electrical, now I'm not so sure. A schematic is intended to represent the electrical layout of a single subassembly. The project in question involves two subassemblies, so it is not an exception. Each PCB should have its own schematic, *that* schematic is a representation of the electrical layout of that PCB. One might possibly want to represent a higher-level assembly with a single schematic on a single sheet, but this is not useful for design of the individual subassemblies; further, a prime use of a schematic is for field service or other technical work with the PCB, and the technician will want to know the circuit partitioning. I don't recommend it. So, do I scrap the easy to interpret logical electrical layout in favour of a physical one? The easy to interpret quality of the integrated schematic is illusory. It is easy to interpret for the purpose of understanding the assembly function, but not for understanding the function of each individual PCB and for identifying which specific components are involved. Normally, if your partitioning of the circuitry into the two PCBs is rational (typically one minimizes interconnects, and/or functional blocks are grouped to minimize noise and other signal integrity problems), each schematic will make sense by itself, especially if the interconnecting signals are given functional names. However, it is possible to have it both ways. I'm still not sure. They both have their merits. Electrical layout with annotations pointing to the physical layout is the easiest to use when trying to understand the design, but physical layout would be easier to generate the netlists for layout and thus manufacturing. Remember, the annotations would be a chore to create and a nightmare to maintain, plus netlisting would require additional time-consuming work. And the result will not be any more useful, even for the purpose of transmitting understanding of the design, than another approach. I'm having another look at the design to see If I can come to a better compromise, perhaps by adding another sheet, for the distributed display components, but then how do I represent this on the master sheet (if I stay with schematic = electrical design) if the master sheet is only to be used for generating the netlst for the other ccts? A rectangle object instead of a sheet symbol for the display cct perhaps? First of all, if you use port only connectivity, the master sheet only calls out the two subsheets, it would not actually implement the connections. Its only function, really, would be to tell the netlister to look at both subsheets. In fact, the project sheet is not really necessary at all, since one of the subsheets could contain the reference (sheet symbol) to the other subsheet. One would use ports only to make sheet interconnection completely clear. But, in fact, the only purpose of the ports is to cause the creation of a complete netlist for the combination of the two sheets, which can be compared with the original project to make sure that every connection is the same. Once the new set of schematics matches the original single schematic, the ports would be replaced with connectors. I'd put net labels on the connector pins. (Using net labels and ports global later one would still produce a complete net list.) The reference to the second sheet from the first could also be deleted, at least for the purpose of generating a net list from the first sheet alone. Yes, replacing that sheet symbol with a rectangle and perhaps arranging the connectors around that rectangle might make things easier for a technician later on. What I would really like is to be able to select a list of sheets to be netlisted instead of all or only one. This has the potential to create more problems than it would solve though (how could I be sure the whole design was netlisted?). No, this is how it works now, if you use a project sheet. The list of sheets is a project schematic with sheet symbols for all the sheets to be included. [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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Project woes
Thanks everyone for all the suggestions. I think I understand the basic problem I have with this design. Abdulrahman said it best, as usual :) , with this; What you want here is one schematic and 2 PCBs. This is because I am using the master sheet as a block diagram of the electrical design, not the physical layout. Someone recently posted a question to this list, asking weather a schematic should represent the electrical or physical layout, I was of the firm opinion - electrical, now I'm not so sure. In the past this has been ok as each electrical 'block' or sheet was associated closely with the physical layout (i.e. one sheet = one pcb). However due to the distributed nature of the display in this particular design it will not work (one sheet = two pcbs). So, do I scrap the easy to interpret logical electrical layout in favour of a physical one? I'm still not sure. They both have their merits. Electrical layout with annotations pointing to the physical layout is the easiest to use when trying to understand the design, but physical layout would be easier to generate the netlists for layout and thus manufacturing. I'm having another look at the design to see If I can come to a better compromise, perhaps by adding another sheet, for the distributed display components, but then how do I represent this on the master sheet (if I stay with schematic = electrical design) if the master sheet is only to be used for generating the netlst for the other ccts? A rectangle object instead of a sheet symbol for the display cct perhaps? What I would really like is to be able to select a list of sheets to be netlisted instead of all or only one. This has the potential to create more problems than it would solve though (how could I be sure the whole design was netlisted?). I'm sure I'll sort something out. Happy new year, Tom. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Project woes
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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
[PEDA] Project woes
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 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. 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. I plan to annotate the schematics showing which parts are on the second PCB. All this should still be quicker than redrawing the project. Any one see any problems with this idea? Or a better way of proceeding? Thanks, Tom. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Project woes
At 02:36 PM 21/12/01 +1100, you 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 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. 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. I plan to annotate the schematics showing which parts are on the second PCB. All this should still be quicker than redrawing the project. Any one see any problems with this idea? Or a better way of proceeding? Thanks, Tom. I am firmly in the one sch = one PCB camp myself. So if it was me I would copy and paste the schematics until I had the division correct, then I would have to manage two sets of manufacturing docs and test docs etc etc but I would still do it. The additional overhead over what the combined assy would have taken is not great - there is the same number of components (or close to it) and the overall complexity is not much greater. But that is just the way I would do it - maybe a smart panelization and clever layout will work for you. Ian Wilson * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Project woes
Dwight Harm wrote: I'd tend to agree with Ian. Me too! But what comes to my mind is an alternative method (though I actually never did it myself): What's about a mixed rigid/flex PCB? That could keep the single project while offering a dual slot mounting. Don't know if the costs for rigid/flex increase over the additional connector/cable/test/assembly costs in your project. Regards, Emanuel -- MPL AG www.mpl.ch Emanuel Zimmermann [EMAIL PROTECTED] Manager RD Phone: +41 (0)56 483 34 34 Taefernstrasse 20 Fax: +41 (0)56 493 30 20 CH-5405 Daettwil * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
