At 23/05/07 17:33, Pearce, Daniel wrote: ><snip> >1. I'm a bit apprehensive about the "DDB vs. Windows File System" >decision. In the past, I've been content with having to manually >generate & load Netlists and back-annotation. I often use the PCB >editor to create sketches, etc that are never related to a >schematic, so just having a .PCB file was fine. It looks like >keeping every part of a design within a single DDB can simplify >things, but it forces a working style that packages *everything* at >a 1-DDB-per-project level. What if there is a logical >system/schematic heirarchy, but different contractors working on >different PCB designs? Also, libraries concern me - see next 2 items.
Well, as Johan Cruijff (famous dutch soccer player) put it: "ervery drawback has its advantages". I use the Windows File System exclusively since I lost three fairly large DDBs in one crash, they were beyond repair. Cost me a full week to recover to a workable point using the auto-save files and a remote tape-backup (auto-save saves open files, but it does so even if the file is not changed). Mr Jenkins is partially right in his remark that with WFS all file managment is left to the user: P99SE does keeps track of its own files by some sort of file system (.reg files in every directory), but there is no recycle bin so you have to be careful (the Windows bin is not used either). You can put stuff in directories "behind Protel's back" using Windows, but then you are the sole keeper of those files: they don't show up inside Protel. If Protel does not know about files that are there it happily deletes a complete directory *including* the files that does not know about. And without a recycle bin..... Ouch. On the upside: 1) in case of a cataclysmic systemcrash you cannot lose more than the currently open files at most, and 2) you do not have to open a project to see what's inside (reports and textfiles open directly in Notepad or whatever word processor you're using for printing or viewing, handy). >2. I want to maintain a central PCB Footprint library that contains >all of the component types we use. So far, that's only ~400 parts >and ~4Megs (I draw relatively fancy silkscreen outlines). Can I >reference one copy of one library for multiple projects? Sure. In fact libraries are always 'global'. For ease of use I have a "PCB library" project with multiple libraries (thruhole, SMT, connectors, mechanicals etc), this keeps the scroll lists manageable in size. Protel can be a bit picky when it comes to multiple .LIB files in a WFS environment (resulting in random 'invalid argument' errors when opening a file). It does not happen often (so I haven't found the cause of it yet, not annoying enough) but it can be remedied effectively by manually correcting the ADVPCB99SE.INI file and re-assigning the LIB files when it happens. > 3. A similar question applies to Schematic Libraries - Just one > central library suits me well. When I need to create a new symbol, > usually I either copy and modify an existing part, or I import from > one of the existing Mfr's libraries. There is always some editing > involved - I use different fill & outline colors based an part > types, and I *never* use hidden power pins. I have yet to encounter a problem with my schematic libraries. Again, I use multiple: discretes, passives, connectors, etc to keep manageable scroll lists. The concept of hidden pins is quite simple, but there are a lot of hidden (no pun intended) issues with them when it comes to connectivity and partlists; by not using hidden pins you can avoid most of them and need not run into the rest. I use them, but only in specific instances and even then I have to think twice about the consequences. >4. Something tells me I'll have to re-learn everything about >printing & Gerber generation - any advice/good links for some >Quick-Start info.? Using the CAM generation wizard you should be up and running pretty quickly, making previews is even simpler. There are a few minor pitfalls (different reference point for Gerber and NC files, different leading/trailing zeroes setting etc), but most good fabhouses correct those correctly on the fly. Scanning the PEDA archives for CAM and Gerber will provide you with (links to) almost everything there is to know about it within the context of P99SE ... >So, which file system, and what do I need to watch out for? >Hopefully, I can start out by importing my P98 Libraries & designs. I'd go with the WFS, you can always convert to DDB later on by creating a shadow project and importing the 'live' one. The other way around is also possible, but a lot trickier. Coming from an OrCad/Tango combo under DOS I found it very easy to get started, I was productive within three days and even found a way to import my OrCad libraries. Keep an open mind to your own routines and habits, there are always many ways to accomplish the same task (the intuitive way is not necessarily the best/quickest/most effective way, but gets the job done here and now; you can always experiment later). Best of luck, Leo Potjewijd hardware designer Integrated Engineering ____________________________________________________________ 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]
