At 11:30 AM 4/23/2002 -0700, JaMi Smith wrote: >Most of these boards are built in house, but the error rate on stuffing >components (the wrong ones in the wrong locations) is very high and the >trouble-shooting time to find these assembly errors is exhorbinate, so I >really do need the silkscreen every place I can get it.
No, you don't. You need good process for assembly. Good assemblers don't even look at the silkscreen. It's too time-consuming. Instead, efficient hand assemblers would, in my experience, prefer to have a golden board, i.e., a board which has been correctly assembled. It's not essential, but if they have a flicker viewer, so much the better (i.e., a viewer which switches quickly from a view of one pcb to the other, with the images positioned identically. Very efficient for detecting differences, first used, I think, in the search for what was later named Pluto. I think I have heard of such a device being used for assembly, but I'm not sure. Similar would be a device which superimposed an image of an assembly drawing over a view of the physical PCB. Presumably, however, if assembly has been making lots of errors, they don't have tools like this. One reason, by the way, to send difficult assembly out. You really can't compete with them, when all is said and done. >Herein lies the problem. I have 4 duplicate channels, with ref >designators currently numbered as R1_1, R1_2, R1_3, R1_4, R2_1, etc. in >the 4 parallel and identical channels. That's a problem in itself, perhaps, though it is one possible configuration. Other posts have often described ways to do duplicate channels in PCB. The default naming that Protel uses when you simply copy a block of components is *not* intended for serious use in duplicating blocks. You could consider these names as placeholders. Their meaning is obvious. But if you like those names, it is obviously easy to obtain them. The solution starts with a good renumbering in the schematic. The use of channel postfixes (like A, B, C etc), assigned number sequences (like channel A contains all refdes numbers between 100-199, B contains 200-299, etc) should be done at the schematic level. It is possible to use match on selection status to rename parts block by block, or if each section has its own page on the schematic, Protel's annotation tool can handle some kinds of channel numbering. Global edits with appropriate match criteria can be used to add distinctive characteristics to each block. As I recall, there are some irritating limitations in replacement criteria which has led me in the past to use the spreadsheet to add channel designators; one should realize that complex manipulations of refdes and comment text can be done in the spreadsheet, and one would have all the tools available in, say, Excel. I've not had good luck with the Protel spreadsheet editor, but perhaps I did not correctly intone the incantations. I use the Protel spreadsheet tool just for exporting the data and taking it back into the Schematic or PCB. If one wants to use the spreadsheet, I advise looking back into the archives for posts about how to Update from Spreadsheet. It can be quite persnickity, if you look cross-eyed at it, it can fail. > My ref designators are already as >small as our fab house will go for which is .025" high and .005" thick >lines, and I am also tenting all of my vias so that they will not >interfere with the silkscreen. Good. Though, as was implied in what I wrote before, I would not let silkscreen requirements override fab and assembly quality requirements. If you want tented vias, perhaps to reduce solder bridging, or you can at least tolerate them -- some assemblers, as I recall, don't like them, perhaps because of outgassing during soldering -- fine. Otherwise I would not go very far to make a complete silkscreen. But if you want a complete silkscreen for 0402 parts, there is lots of room between the parts if you cut out some of the outline, especially if you can handle 5 mil text. I've never gone that small. I'd make some custom footprints with the outline designed for this use. You could, of course, unlock primitives for a footprint and edit the outlines, but I would only do this if there were just a few places where it were necessary. > I could however get a lot more >designators placed in the limited room that I have if I could eliminate >the channel designator part of the ref designator, i.e.: reduce the R1_1 >to simply R1, which is much shorter, and which due to the layout is >acceptable since the channels are physically very clear and already >labeled as CH_1, CH2, etc. Sure. And this is not at all difficult to do. See below. >However, if I shorten the actual designator, it makes for >synchronization problems with the schematic, as well as hell to pay in >the DRC department. Right. Don't do that. Instead use the Comment field, which is otherwise a bicycle for a fish. To make the comment fields correspond to the reference designator minus the channel indicator, I'd use Excel as indicated above. Some combination of Excel and a word processor can accomplish almost anything needed to solve a problem like this. >I want to keep the ref designators the same for the same component in >the different channels for the sake of circuit / schematic / >troubleshooting clarity, etc. Renumbering them to 100 series for channel >1, 200 series for channel 2, etc, is not only very time consuming but >doesn't really get me much shorter designators anyway. Right. The use of A, B, C could be a little better, depending on the number of parts in the channels. >Hiding the original designators, and replacing them with "loose" text is >not only very time consuming, but prone to error, not only now, bur >especially in the future if someone else has to modify the board and >move components, since the "loose" text is not related to the component. Yes, very bad idea, boo, boo.... :-) >I have thought of copying off the final database and modifying all of >the designators and then generating a new gerbers from the modified file >and substituting those overlay gerbers in the final set for fab, but >that is a massive amount of work that will have to be done all over >again if there is any substantial change to the board. Yes, also bad idea and to be avoided. There are, quite simply, better ways. >I do in fact own an Official Mickey Mouse Club Tee Shirt and Hat, which >I am about to pull out and put on, but there has got to be a better way >of handling duplicate circuits in Protel, or should I just throw up my >hands and look for another product all together (PADs, Mentor, Verybest, >etc.). It appears that Protel truly has no provision to handle any kind >of duplicate circuits, especially of the Step and Repeat variety, >whatsoever. It would have been more accurate to say, "I haven't been able to figure out how to use Protel with duplicate circuits." I'd not conlude that there is "no provision" for something until I've asked about it here. You'll notice that when someone asks a question like "Is there any way to do XXX in Protel," I won't answer, if I am awake that day, with "No." Instead I might say, "Not that I have been able to find." Sometimes, indeed, someone else has popped in with something I had never noticed. >Anyone out there got any useful ideas? How I would solve this problem might depend on the complexity involved, but if there were more than a few minutes necessary to renumber parts by hand, I'd use one of the more sophisticated techniques, probably involving the spreadsheet. I would definitely want to end up with a PCB and Schematic that fully synchronize, normally, without any fiddling, and I would seriously avoid making a special file for silkscreen use. Too much work, which must be repeated every time one edits the board. Lots of room for error. And I'll add one piece of advice, hard-earned from many times I did not follow it: Design the first repeated section in the schematic very carefully (or ask the engineer, if it isn't you, do be very careful) to reduce necessary changes other than changes that can easily be handled with global edits (such as value changes). If you wait until after you have multiplied up the section, you will also have multiplied the work involved in any changes. Then, likewise, with the PCB, place and wire one section and plan very carefully how you are going to multiply it up. Make sure you have it right. (I'd send the section to the engineer before proceeding.) Once again, every corrective action will be multiplied if you wait until later. 4 sections is not so many. I did a board for SETI that had 32 channels, each with perhaps 40 or 50 parts. Yes, I had to make some changes.... [Protel, give us easy-to-record and easy-to-use macros.....) I would seriously try to avoid needing to manipulate the designators. This would mean designing the part so that the autopositioned designators were correct, or at least could be massaged into the correct positions en masse (such as with a spreadsheet). If it is necessary to move the designators, it should be done with the first section *before* it is multiplied up, and if later sections will have longer designators, that should be considered. If a block of parts have centered, autopositioned designators, an offset can be added to move those designators in a particular direction by a set amount; I'd do this in Excel. Good planning is essential for easy and easily maintainable multi-channel design. It is well worth thinking the whole process out, and perhaps testing some aspects of it, before plowing into the work. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *