rmf@bpdsun1.uucp (Rob Finley) (11/17/89)
> Well, Tango PC w/ autoroute costs around $1000, so I'm looking for > something between $500-$1500. The cheaper the better. Doesn't have to > have a whole lot of features, I just need it to get the job done. I > would like it to output to a plotter _or_ printer though. Considerations for Computer Aided Board Design (I design PCB's for a living) For auto routing to be practical and to keep wiring errors controlled (trust me, you will make them and they won't be fun to find!) I cannot recommend strongly enough to do your schematic with a Schematic-Capture program. You will not find a better package for less than $600 than ORCAD schematic. It is simply a dream to use. I use it at home but not at work. After you get the schematic entered, Orcad can run a utility called a NETLISTER. A net list is a database of the wiring. One file will have a list of parts and which kind of packages they are using (whether it be a 14pin IC chip, a small bypass cap, or a large Electrolytic). Another file will have a list of pins and which wires are connected to them. I use the netlist when I have to wirewrap things. Which isn't very often :). Orcad does have a nice PCB design package available as well as a logic simulator(that we would like to get at work as our present Schematic package won't design programmable logic chips). A less expensive but high quality package would be Tango PCB II. It is complex enough to support normal through-the-hole technology and be able to correctly handle surface mounts up to 160 pins with 0.0250" spacing! Both packages will run on at least a 640K PC with acceptable speed (especially Orcad |8-) ) and don't require an 8087. Boards are a bear to make on a monochrome system. Tell me you have at least a color EGA! The beauty about having a net list is that it will show DEFEREDs (sp?) when you are using the board design package. Tango does a nice job of this. In our system, a Deferred is a connection that has not been made yet. It is shown as a thin line of bright colors (we have many to chose from) that runs between two pins. When you place the connection between them, the Deferred disappears. Neat? I can do a medium sized board in a day. WARNINGS and PITFALLS TO LOOK OUT FOR. Each board has a set of design rules. Design rules are specifications such as the sizes of the pads for "via's" or feedthru connections, line widths, and the clearance distance between two pieces of metal foil. If your clearances are not wide enough, you will end up with a "blob" when you get your board plotted. If the clearances are too large, then the program won't (shouldn't :< ) let you put in lines wide enough to carry the current. For final plots on the boards: For boards of any complexity, you will get the best results if you generate a plot file in the GERBER photoplotter format. You will need to find a service bureau that does photoplotting and either modem or send them floppies, or 9 track magnetic tape. Finding a bureau should be done FIRST. If they use an older photoplotter where the patterns are actually masks that it shines a light through ("arpeture"), you will need to get a list of the apeture specs or send a list with your plot files. Otherwise you might end up with line specifications that the plotter won't support. I can't recommend doing it any other way unless you can send it out on a piece of transparency plastic processed with a standard laser printer. If you are using a fabricator to make the board, you might want to chose your own plotting bureau as a lot of them have in-house Gerber laser plotters that they paid millions for and they can charge you hundreds if they do your board on their machine. Drilling holes: All fab houses have drilling machines that read paper tape lists of the holes and the sizes of the drill bits. The industry standard was defined by the EXCELLON company and almost everyone uses it. For some bizarre reason, our company doesn't send it with the plot files and the fabricators have to "bomb site" each hole location with a digitizer tablet and MANUALLY create the drill tape. UUUUGGGGHHHH!!! By the way, if your PCB package makes the file, a floppy version of the file should suffice. They usually have the equipment on hand to make the tape. Check your work before you send it. You migh even hold on to it for a day or two after you are done to make absolutely sure that it is right. We have missed things in the heat of the race and had to do it over. A replot of our projects costs us more than $100! and that is if they catch it before they start making the boards!! Before I got this job, I tried to do a board quickly with no experience on my IBM PC with monochrome cga video. It was impossible. There is a lot to do before you can create a board simply in setting up the "libraries". I spend a lot of time "creating" schematic symbols and physical package information for each new part that we add to the system. Fortunately, they are reuseable. But, be sure to allow for setup time in your project plans. Last but not least. A larger board size is always a cheaper alternative to using four layer boards. You cannot do a 3 layer board without having it warp severely. Try your hardest to get it onto just two layers. The cost difference between two and four is phenomenal. And, if you have a wiring error on one of the inner traces, you are sunk. You can't get to it to even test the changes and will have to do it all over again. ugh! EMAIL me if you have any problems. ------- "Don't you try to play God! You aren't very good at it and besides, the position is already taken!" --- Fat Man and Little Boy. We make Television and Radio Transmittors. If your station doesn't have one, call them up and complain. Rob quintro!bpdsun1!rmf@lll-winken.llnl.gov uunet!tiamat!quintro!bpdsun1!rmf
malcolm@Apple.COM (Malcolm Slaney) (11/29/89)
In article <054911.339@bpdsun1.uucp> rmf@bpdsun2.UUCP (Rob Finley) writes: >For final plots on the boards: >For boards of any complexity, you will get the best results if you generate >a plot file in the GERBER photoplotter format. You will need to find a >service bureau that does photoplotting and either modem or send them >floppies, or 9 track magnetic tape. Mosis provides a service where they will accept CIF over the Internet and turn it into a photoplot or even a completed PCB. Its pretty neat to send some EMAIL and get back a PCB in a few weeks. Mosis was the DARPA chip making organization. I think it has since been spun off and is now administered by ISI in Southern California. A couple of years ago they started adding a few more services based on their successes with chip building. The PCB making service was done to support the chips they made. They will now do business with anybody so there is no longer a need to get funny money from the US Government. It's pretty easy to translate back and forth between CIF (the standard academic/research standard for chip designs) and Gerger (the PCB standard). I don't have the code anymore but both directions were only a couple pages of code. When they first started this service they took the CIF and plotted it onto a quartz photomask, photographically expanded it and then made the PCB's from this. Since quartz photomasks are a bit expensive they were working on doing it the right way (use software to convert to convert the CIF to Gerber.) Still a couple of years ago it was pretty neat to do a design on a Cadnetix system, convert the Gerber to CIF and use EMAIL to submit the design. I'm sure the procedure is much less complicated now. For more information send a note to mosis@mosis.edu and you should get back some information on how to request the PCB stuff. Malcolm