Re: [PEDA] [PROTEL EDA USERS]: Library Management
Re: [PEDA] [PROTEL EDA USERS]: Library Management
David, I couldn't agree with you more. With regards to library management, we have had a horrific experience with designers creating their own libraries and project libraries etc. Countless errors have been produced by this and finally I took the initiative, much to some designers dismay, to create a standard company library to include only the parts not found in the existing libraries and a much reduced DEVICE library. We have one library manager and he is responsible for any new part construction. Yes it does slow the design process somewhat, but it eliminates rework due to mistakes. I have indicated before that we have a very diverse cultural menagerie of designers and with each making their own version of the same part, well you can imagine the schematic nightmare. We have also done this to our pcb footprint library. No footprint is used without the manufacturing dept approval of the footprint first after its creation. When we use outside contractors, the same rules apply, we supply our pcb footprint library on CD. Just what we are doing. Seems to be working. Lloyd Good GE Harris Energy Control Systems Canada Inc. 2728 Hopewell Place NE Calgary, AB, Canada T1Y 7J7 (403) 214-4777 -Original Message- From: David Cary [mailto:[EMAIL PROTECTED]] Sent: Friday, February 23, 2001 1:05 PM To: Multiple recipients of list proteledausers Subject: Re: [PROTEL EDA USERS]: Library Management Dear Andy Lintz, I've been wodering about this myself. Why does everyone have to re-invent the wheel ? Andy Lintz asked for library advice: I want to set up a system to maintain orderly control over my parts and boards. Some of you seasoned pros probably have some good advice on the topic that might get me started off on the right path. There are so many library files and it seems impossible to tell where a given part originated from once it is in a design. Is it wise to make a company library of only the parts actually used, and copy individual parts to this company maintained library? I've been trying to do that. But it seems that all the other designers have their own ideas on how to organize a library, so we've ended up with an individual library for each person. When a person takes over a project (or when he wants to use a part originally used on someone elses's project), stuff gets copied into his personal library. I keep thinking there ought to be a better way. Is it correct that the libraries are only accessed when a part is first placed, when the 'update parts from cache' in Schematic Editor is executed, or when the 'Update PCB' in the PCB Footprint Editor is executed? (The libraries are not used or needed each time the design is opened, right?) Yes. If you email a .sch or .pcb file to me, I can view it, even though I don't have any of your libraries. By using Design | Make Project Library I can extract a library of symbols from your schematic, or Design | Make Library to extract a library of footprints from your layout. If I execute a 'Make Library' command from inside a schematic or pcb design, do all parts then reference that new library instead of whatever library they were originally placed from? No. Stuff inside a schematic or pcb always references the cache embedded in that same .sch or .pcb file. Those things never reference any library. Often I would like to know which library a particular item came from. But unfortunately, with Protel 99SE s.p. 6, it's impossible to find out which library it came from. What is general practice on the use of the library read-only fields and part fields? Are company part numbers usually assigned to one of the part fields, one of the library fields, or not at all in Protel? (If its the library fields, I think that means a unique library part for each value of resistor and cap) ... Andrew Lintz Good question. The designer next door to me has a unique library symbol for each value of resistor and cap on his schematics; the Lib Ref field (symbol name) contains the company part number. Another method I've seen for naming schematic symbols (which Baldwin insists on calling a ``gate decal'') and naming footprints (which Baldwin calls a ``pcb decal''): PCB Design Guidelines:Naming Conventions http://www.baldwin-tech.com/designgu.htm I keep thinking there ought to be a better way. -- David Cary * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * This message sent by: PROTEL EDA USERS MAILING LIST * * Use the reply command in your email program to * respond to this message. * * To unsubscribe from this mailing list use the form at * the Association web site. You will need to give the same * email address you originally used to subscribe (do not * give an alias unless it was used to subscribe). * * Visit http://www.techservinc.com/protelusers/subscrib.html * to unsubscribe or to subscribe a new email address. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] [PROTEL EDA USERS]: Library Management
On Mon, 26 Feb 2001 13:42:51 EST, you wrote: TIP: The Q_... name convention for symbols allows for all devices to be easily found in one area of the library without exhaustive searches. Similarly I use U_... for all IC devices, D_... for all diodes, X_... for crystals, etc. Now THERE's a convention that Protel ought to use in their libraries. If it's okay, with you, I do believe I'll steal that idea and add it to my whole personal library next time I get a little break between jobs. Am I missing something? I can only think of one case where that would be vaguely useful which is when you don't have the symbol you need and want to see a list of possibly similar symbols to copy from. It will save others from reinventing the wheel because they can't FIND the wheel, too! I would just type *wheel* in the filter box. Cheers, Terry. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * This message sent by: PROTEL EDA USERS MAILING LIST * * Use the reply command in your email program to * respond to this message. * * To unsubscribe from this mailing list use the form at * the Association web site. You will need to give the same * email address you originally used to subscribe (do not * give an alias unless it was used to subscribe). * * Visit http://www.techservinc.com/protelusers/subscrib.html * to unsubscribe or to subscribe a new email address. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To leave the EDAFORUM discussion list, send a email with 'leave edaforum' in the body to '[EMAIL PROTECTED]' More Information : http://www.dolist.net
Re: [PEDA] [PROTEL EDA USERS]: Library Management
Andy, David, Lloyd or others. Yes library management is a pain in the putoot. A good number of us have been around for long enough to see the pains first hand of not managing libraries in an acceptable manner. The problem arises from the diversity of cultures that your typical company has in it's engineering experience bank. Since there is this diversity, there are dozens of opinions about which is the best, easiest and most complete or safe way to manage this. Add to this complexity the varying limitations or restrictions found from one CAD tool to the other and you have a matrix which would make a mathematician weep. Thus there is no singular correct manner by which to handle CAD library management. Likewise there is no one globally accepted management style for any company or corporate entity, if there was all companies would be equally successful and what a boring world this would be. One rule that I follow across all my experience is that there must only be one company reference library. Every designer must have access to the reference library and use the reference parts. Even if there is a one of prototype there should not be any symbol or footprint which is not accessible to all designers and has not been designed to meet company requirements. Anything short of this overall governing rule is a one way road to disaster, or at least a few tears, gripes and complaints, throwing money away, finger pointing and lost productivity. The second rule that I follow religiously is that I will not use CAD tool vendor supplied libraries without confirming their suitability with my own reference resources. Usually none of the vendors library parts pass my inspection without revision. Thus, at best I copy the vendors libraries into my own reference library after confirming their correctness or suitability and editing them to meet our requirements. Anybody who wants to discuss particulars with me I am willing to share my views and practices further but it should be taken offline so as not to overload everyone on the listserver. Sincerely, Brad Velander Lead PCB Design Norsat International Inc. #100 - 4401 Still Creek Dr., Burnaby, B.C., Canada. V5C6G9. voice: (604) 292-9089 (direct line) fax:(604) 292-9010 email: [EMAIL PROTECTED] www: www.norsat.com -Original Message- From: TSListServer [mailto:[EMAIL PROTECTED]]On Behalf Of [EMAIL PROTECTED] Sent: Friday, February 23, 2001 12:40 PM To: Multiple recipients of list proteledausers Subject: RE: [PROTEL EDA USERS]: Library Management David, I couldn't agree with you more. With regards to library management, we have had a horrific experience with designers creating their own libraries and project libraries etc. Countless errors have been produced by this and finally I took the initiative, much to some designers dismay, to create a standard company library to include only the parts not found in the existing libraries and a much reduced DEVICE library. We have one library manager and he is responsible for any new part construction. Yes it does slow the design process somewhat, but it eliminates rework due to mistakes. I have indicated before that we have a very diverse cultural menagerie of designers and with each making their own version of the same part, well you can imagine the schematic nightmare. We have also done this to our pcb footprint library. No footprint is used without the manufacturing dept approval of the footprint first after its creation. When we use outside contractors, the same rules apply, we supply our pcb footprint library on CD. Just what we are doing. Seems to be working. Lloyd Good GE Harris Energy Control Systems Canada Inc. 2728 Hopewell Place NE Calgary, AB, Canada T1Y 7J7 (403) 214-4777 -Original Message- From: David Cary [mailto:[EMAIL PROTECTED]] Sent: Friday, February 23, 2001 1:05 PM To: Multiple recipients of list proteledausers Subject: Re: [PROTEL EDA USERS]: Library Management Dear Andy Lintz, I've been wodering about this myself. Why does everyone have to re-invent the wheel ? Andy Lintz asked for library advice: I want to set up a system to maintain orderly control over my parts and boards. Some of you seasoned pros probably have some good advice on the topic that might get me started off on the right path. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * This message sent by: PROTEL EDA USERS MAILING LIST * * Use the reply command in your email program to * respond to this message. * * To unsubscribe from this mailing list use the form at * the Association web site. You will need to give the same * email address you originally used to subscribe (do not * give an alias unless it was used to subscribe). * * Visit http://www.techservinc.com/protelusers/subscrib.html * to unsubscribe or to subscribe a new email address. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] [PROTEL EDA USERS]: Library Management
On Mon, 26 Feb 2001, Brad Velander wrote: Steve, can't help you with your routing problem, routers are a big mystery to me. Nobody I have worked for has ever had boards that they would trust to, would work with, nor would they shell out for, an autorouter. It depends what you expect from them. The board I'm currently running is 7*3.3, with 3300 pads, very few of which are on a conventional bus - no memory arrays. It's also blessed with 12 supply voltages, many of which have local planes. Even at an incredibly optmistic 20 seconds per pad, that's 18 hours - more realistically, it's about 5 times that. (Specctra would be done in about 4-6 hours). I'm better than Specctra on any given net, and I don't paint myself into a corner as often as it does, but it's far, far faster. For nets I care passionately about, I'll always check its output, but for run-of-the mill stuff, even if I can see a way to do a net better, I'll leave the specctra output alone - twiddling with a board for weeks isn't normally profitable, especially for prototype boards, where the first prototype run may or may not work at all, let alone subtle EMC issues... Getting the softies something to work with while I work on rev 2 seems to be much more efficient. (This is all for short timescale stuff. People with relaxed timescales obviously have different options) One thing that autorouters also help with is placement - if the autorouter can't make a good start very quickly, odds on the placement or ruleset needs a tweak. Are you aware that Protel 'suggests' that they only support 12 characters in the footprint name? Yeah. Don't know it it still applies, but that's my uniqueness limit. Steve * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * This message sent by: PROTEL EDA USERS MAILING LIST * * Use the reply command in your email program to * respond to this message. * * To unsubscribe from this mailing list use the form at * the Association web site. You will need to give the same * email address you originally used to subscribe (do not * give an alias unless it was used to subscribe). * * Visit http://www.techservinc.com/protelusers/subscrib.html * to unsubscribe or to subscribe a new email address. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To leave the EDAFORUM discussion list, send a email with 'leave edaforum' in the body to '[EMAIL PROTECTED]' More Information : http://www.dolist.net
Re: [PEDA] [PROTEL EDA USERS]: Library Management
Steve, can't help you with your routing problem, routers are a big mystery to me. Nobody I have worked for has ever had boards that they would trust to, would work with, nor would they shell out for, an autorouter. And in trying to play with them, they confound me and constantly do not respond in the manner one might expect when trying to make one work in a reasonable fashion. This last comment is undoubtedly because I have never received any training in how to configure or use one. You do mention something that I believe I had problems with a while ago after first starting with Protel. You mention a footprint naming convention that appears it could easily violate Protel's footprint name limitations. Are you aware that Protel 'suggests' that they only support 12 characters in the footprint name? I had some problems a while back with various operations not working correctly (like Update from the footprint library). Several people on this list as well as Protel suggested several issues with my footprint names, one of these was the length limitation. I am not sure which naming issue had bit me but I changed several and my problems went away. Now I restrict the name to the 12 character limit. FYI: the limitation is mentioned in only one location that I have been able to find. It is hidden in the section explaining netlist formats and limitations (pg 648 in my acrobat version of the Protel P99SE manual). Sincerely, Brad Velander Lead PCB Design Norsat International Inc. #100 - 4401 Still Creek Dr., Burnaby, B.C., Canada. V5C6G9. voice: (604) 292-9089 (direct line) fax:(604) 292-9010 email: [EMAIL PROTECTED] www: www.norsat.com -Original Message- From: Steve Wiseman [mailto:[EMAIL PROTECTED]] Sent: Monday, February 26, 2001 11:22 AM To: Multiple recipients of list proteledausers Subject: RE: [PROTEL EDA USERS]: Library Management TIP: The Q_... name convention for symbols allows for all devices to be easily found in one area of the library without exhaustive searches. Similarly I use U_... for all IC devices, D_... for all diodes, X_... for crystals, etc. I extend this, with, f'rinstance, IC_TSSOP_whatever in the PCB libraries. Makes for slightly longer footprint names, but it's not as if I have to type them in very often, and not having dozens of slightly different SOP8, SO8, S08, S0P8 variants, the world's a better place. SNIP Steve * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * This message sent by: PROTEL EDA USERS MAILING LIST * * Use the reply command in your email program to * respond to this message. * * To unsubscribe from this mailing list use the form at * the Association web site. You will need to give the same * email address you originally used to subscribe (do not * give an alias unless it was used to subscribe). * * Visit http://www.techservinc.com/protelusers/subscrib.html * to unsubscribe or to subscribe a new email address. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To leave the EDAFORUM discussion list, send a email with 'leave edaforum' in the body to '[EMAIL PROTECTED]' More Information : http://www.dolist.net
Re: [PEDA] [PROTEL EDA USERS]: Library Management
Brian And everyone, I was just about to post a very similar message. I'm currently very irritated because I just found a library problem in a production run of boards Please let me know if I did something really stupid or if Prtoel did something stupid and I was too naive to catch it. The problem is: I made a schematic and converted it to a PCB. Gripe 1: There are no matching (default) PCB footprints for the schematic symbols. This stikes me as really dumb. There should be a set... Gripe 2: The schematic symbol for a pot has pin 3 as the tap/wiper. I never saw this because my pin names were off... I converted from sch to PCB and applied the generic footprint VRn - to avoid wiring problems (hah!). That what the whole point of this technology is for isn't it! I checked my transistors for pin problems and found some (but I guess I had kind of expected a transistor problem. I didn't expect a problem in something so basic as a VR and time was short). The PCB component was correct - pad 2 is (and as far as I know is ALWAYS) the wiper. So as far as I'm concerned the schematic library component is wrong in a dangerous and dumb way. I can see that it is an extension of resistor but surely everyone would get caught by this. Question: Take the RETSISTOR TAPPED sch library part for eg. It does not have any hidden pins (according to library params) yet I have to use display hidden pins to see the pin nums etc... Why is this so ? Question: What is the correct way of assiging schematic pins so they match PCB pins (how do I make the change and ensure correctness) Question: Do I have to create my own compatible sch and PCB libs which seems really stupid in as professional a product as PCB. I seem to remember that others have had to make libs too. Do we have a shared library pool (schematic compatible). I currently don't feel like trusting protel libs. ISA9000 or not. Ok so am I being really stupid/naive or is it a serious problem ? regards Kim On Sunday, February 25, 2001 10:05 AM, Brian Guralnick [SMTP:[EMAIL PROTECTED]] wrote: I know it's a waste of space, but I wish that each schematic library component had it's own dedicated footprint as a default, or the option of an external footprint, or copy an external footprint to the schematic component's default. OK, I realize that this is exactly how you currently define any current component, but all I want is for the schematic component to be connected, or part of the same single library name file for any component. _ Brian Guralnick File: ATT2.htm * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * This message sent by: PROTEL EDA USERS MAILING LIST * * Use the reply command in your email program to * respond to this message. * * To unsubscribe from this mailing list use the form at * the Association web site. You will need to give the same * email address you originally used to subscribe (do not * give an alias unless it was used to subscribe). * * Visit http://www.techservinc.com/protelusers/subscrib.html * to unsubscribe or to subscribe a new email address. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To leave the EDAFORUM discussion list, send a email with 'leave edaforum' in the body to '[EMAIL PROTECTED]' More Information : http://www.dolist.net
Re: [PEDA] [PROTEL EDA USERS]: Library Management
Kim, from the sounds of your enquiry, you are not overly experienced in the use of CAD tools. If you were you would realize that this falls under the concept of not trusting vendor supplied libraries (canned libraries). It is almost a cardinal rule in EDA that you cannot trust canned libraries. This is not a Protel issue, it is an issue with most every CAD library supplied by a Vendor. This would fall under the requirement that one must verify and ensure the suitability of any vendor supplied library part/component/symbol. As for the original comment from Brian, with the profusion of part footprints from varied manufactures do you think it is possible to supply a library with a default footprint that would cover all possibilities in a suitable fashion. A word of warning might point out an issue for further study on your part. Would all SOT23 devices fit one standard/global SOT23 footprint? Not a chance, in the professionally designed footprint standard that our company uses there are over one dozen variations of a SOT23 footprint to cover all manufacturers and devices that they have encountered over the life of their footprint design standard. Need a SOT23 footprint? You had better pull out the manufacturers datasheets and ensure that you have got exactly the right footprint for that manufacture and that manufacturers particular part type (this does not even include the fact that some manufacturers alter the pin numbering scheme around on SOT23s). In some cases, a standard SOT23 footprint is not even a reality across one manufacturers part offerings, depends on the packaging facility that packaged the dies. As for your POT symbol/footprint problem, I have seen manufacturer's parts specs that would have fit your symbol pin numbering (pin #3 is wiper). So is the symbol you used wrong? No it was simply not the symbol which you wanted to use. Assume nothing when it comes to vendor supplied libraries! When you make a library part document it in a way that think is suitable to ensure others don't make similar mistakes using your library. Your issue with the hidden pins on the tapped resistor, the pin numbers obviously are defined as hidden. If they were not defined as hidden you would not need to check the hidden pins checkbox in order to make them visible. The checkbox may seem slightly confusing because the pin is possibly not the portion of the information which is hidden, as you found out the pin number can be hidden as well. As for being stupid or naive, no, I doubt that you are either. Inexperienced, sounds more like it. Sincerely, Brad Velander Lead PCB Design Norsat International Inc. #100 - 4401 Still Creek Dr., Burnaby, B.C., Canada. V5C6G9. voice: (604) 292-9089 (direct line) fax:(604) 292-9010 email: [EMAIL PROTECTED] www: www.norsat.com -Original Message- From: Kim Lester [mailto:[EMAIL PROTECTED]] Sent: Saturday, February 24, 2001 8:15 PM To: Multiple recipients of list proteledausers Subject: RE: [PROTEL EDA USERS]: Library Management Brian And everyone, I was just about to post a very similar message. I'm currently very irritated because I just found a library problem in a production run of boards Please let me know if I did something really stupid or if Prtoel did something stupid and I was too naive to catch it. The problem is: I made a schematic and converted it to a PCB. Gripe 1: There are no matching (default) PCB footprints for the schematic symbols. This stikes me as really dumb. There should be a set... Gripe 2: The schematic symbol for a pot has pin 3 as the tap/wiper. I never saw this because my pin names were off... I converted from sch to PCB and applied the generic footprint VRn - to avoid wiring problems (hah!). That what the whole point of this technology is for isn't it! snip Question: Take the RETSISTOR TAPPED sch library part for eg. It does not have any hidden pins (according to library params) yet I have to use display hidden pins to see the pin nums etc... Why is this so ? Question: What is the correct way of assiging schematic pins so they match PCB pins (how do I make the change and ensure correctness) Question: Do I have to create my own compatible sch and PCB libs which seems really stupid in as professional a product as PCB. snip Ok so am I being really stupid/naive or is it a serious problem ? regards Kim * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * This message sent by: PROTEL EDA USERS MAILING
Re: [PEDA] [PROTEL EDA USERS]: Library Management
On Mon, 26 Feb 2001, Brad Velander wrote: As for your POT symbol/footprint problem, I have seen manufacturer's parts specs that would have fit your symbol pin numbering (pin #3 is wiper). So is the symbol you used wrong? No it was simply not the symbol which you wanted to use. Assume nothing when it comes to vendor supplied libraries! When you make a library part document it in a way that think is suitable to ensure others don't make similar mistakes using your library. Also, there's no need to use dull pin numbers like 1, 2 and 3. For a pot, I'd go for CW, CCW and WIP , just to hammer it home. Same goes for my big collection of SOT23 footprints, given that I can't trust any manufacturer for pin names, I'll do it myself, and it's dead handy while debugging boards T3.E means more to me than T3.3 (assuming I got it right at schematic time). Steve * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * This message sent by: PROTEL EDA USERS MAILING LIST * * Use the reply command in your email program to * respond to this message. * * To unsubscribe from this mailing list use the form at * the Association web site. You will need to give the same * email address you originally used to subscribe (do not * give an alias unless it was used to subscribe). * * Visit http://www.techservinc.com/protelusers/subscrib.html * to unsubscribe or to subscribe a new email address. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To leave the EDAFORUM discussion list, send a email with 'leave edaforum' in the body to '[EMAIL PROTECTED]' More Information : http://www.dolist.net
Re: [PEDA] [PROTEL EDA USERS]: Library Management -relevant?, yes!
Re: [PEDA] [PROTEL EDA USERS]: Library Management
Steve, I take a different approach to transistor devices. 'Most' follow a normal standard for pins 1,2,3,(4?) so I use this method and over-ride any manufacturers which do not follow the same standard. I stick to the 1,2,3,(4?) based upon the most common occurrence of SOT23, TO92, TO220 numbering. To hell with the rogue manufacturers. I do make custom symbols for each transistor device configuration that I come across, naming them by the manufacturers part number and assigning a matching footprint. There are just too many combinations of transistors to try and standardize a symbol and footprint for all transistor devices. I have also seen too many board errors over the years from trying to standardize transistor symbol/part management down to standard symbols and footprints to cover all cases. For example my symbol library would contain transistors named Q_2N2201, Q_2N4401, Q_MMBT3904, Q_IRFR5305, etc. Each would be pin numbered to match a standard footprint pin numbering. This way any tech or engineer does not have to find each and every manufacturer's datasheet to know where pin 3 is on a particular device, or to know here the emitter is on a particular device, as long as he has the schematic in front of him and knows the standard pin numbering for the particular package rather then the custom (non-standard) pin numbering from 'ABC' manufacturer. Yeah I know, somebody is going to say that someone using the manufacturers datasheet is going to get confused but likewise in the opposite case someone is going to get confused and that confusion can too easily cause scrap PCBs. The engineer should always have the schematic as well as the manufacturers datasheet and the schematic will set him straight. TIP: The Q_... name convention for symbols allows for all devices to be easily found in one area of the library without exhaustive searches. Similarly I use U_... for all IC devices, D_... for all diodes, X_... for crystals, etc. Sincerely, Brad Velander Lead PCB Design Norsat International Inc. #100 - 4401 Still Creek Dr., Burnaby, B.C., Canada. V5C6G9. voice: (604) 292-9089 (direct line) fax:(604) 292-9010 email: [EMAIL PROTECTED] www: www.norsat.com -Original Message- From: Steve Wiseman [mailto:[EMAIL PROTECTED]] Sent: Monday, February 26, 2001 9:50 AM To: Multiple recipients of list proteledausers Subject: RE: [PROTEL EDA USERS]: Library Management On Mon, 26 Feb 2001, Brad Velander wrote: As for your POT symbol/footprint problem, I have seen manufacturer's parts specs that would have fit your symbol pin numbering (pin #3 is wiper). So is the symbol you used wrong? No it was simply not the symbol which you wanted to use. Assume nothing when it comes to vendor supplied libraries! When you make a library part document it in a way that think is suitable to ensure others don't make similar mistakes using your library. Also, there's no need to use dull pin numbers like 1, 2 and 3. For a pot, I'd go for CW, CCW and WIP , just to hammer it home. Same goes for my big collection of SOT23 footprints, given that I can't trust any manufacturer for pin names, I'll do it myself, and it's dead handy while debugging boards T3.E means more to me than T3.3 (assuming I got it right at schematic time). Steve * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * This message sent by: PROTEL EDA USERS MAILING LIST * * Use the reply command in your email program to * respond to this message. * * To unsubscribe from this mailing list use the form at * the Association web site. You will need to give the same * email address you originally used to subscribe (do not * give an alias unless it was used to subscribe). * * Visit http://www.techservinc.com/protelusers/subscrib.html * to unsubscribe or to subscribe a new email address. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To leave the EDAFORUM discussion list, send a email with 'leave edaforum' in the body to '[EMAIL PROTECTED]' More Information : http://www.dolist.net
Re: [PEDA] [PROTEL EDA USERS]: Library Management
Re: [PEDA] [PROTEL EDA USERS]: Library Management
Dear Andy Lintz, I've been wodering about this myself. Why does everyone have to re-invent the wheel ? Andy Lintz asked for library advice: I want to set up a system to maintain orderly control over my parts and boards. Some of you seasoned pros probably have some good advice on the topic that might get me started off on the right path. There are so many library files and it seems impossible to tell where a given part originated from once it is in a design. Is it wise to make a company library of only the parts actually used, and copy individual parts to this company maintained library? I've been trying to do that. But it seems that all the other designers have their own ideas on how to organize a library, so we've ended up with an individual library for each person. When a person takes over a project (or when he wants to use a part originally used on someone elses's project), stuff gets copied into his personal library. I keep thinking there ought to be a better way. Is it correct that the libraries are only accessed when a part is first placed, when the 'update parts from cache' in Schematic Editor is executed, or when the 'Update PCB' in the PCB Footprint Editor is executed? (The libraries are not used or needed each time the design is opened, right?) Yes. If you email a .sch or .pcb file to me, I can view it, even though I don't have any of your libraries. By using Design | Make Project Library I can extract a library of symbols from your schematic, or Design | Make Library to extract a library of footprints from your layout. If I execute a 'Make Library' command from inside a schematic or pcb design, do all parts then reference that new library instead of whatever library they were originally placed from? No. Stuff inside a schematic or pcb always references the cache embedded in that same .sch or .pcb file. Those things never reference any library. Often I would like to know which library a particular item came from. But unfortunately, with Protel 99SE s.p. 6, it's impossible to find out which library it came from. What is general practice on the use of the library read-only fields and part fields? Are company part numbers usually assigned to one of the part fields, one of the library fields, or not at all in Protel? (If its the library fields, I think that means a unique library part for each value of resistor and cap) ... Andrew Lintz Good question. The designer next door to me has a unique library symbol for each value of resistor and cap on his schematics; the Lib Ref field (symbol name) contains the company part number. Another method I've seen for naming schematic symbols (which Baldwin insists on calling a ``gate decal'') and naming footprints (which Baldwin calls a ``pcb decal''): PCB Design Guidelines:Naming Conventions http://www.baldwin-tech.com/designgu.htm I keep thinking there ought to be a better way. -- David Cary * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * This message sent by: PROTEL EDA USERS MAILING LIST * * Use the reply command in your email program to * respond to this message. * * To unsubscribe from this mailing list use the form at * the Association web site. You will need to give the same * email address you originally used to subscribe (do not * give an alias unless it was used to subscribe). * * Visit http://www.techservinc.com/protelusers/subscrib.html * to unsubscribe or to subscribe a new email address. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To leave the EDAFORUM discussion list, send a email with 'leave edaforum' in the body to '[EMAIL PROTECTED]' More Information : http://www.dolist.net
Re: [PEDA] [PROTEL EDA USERS]: Library Management
Terry, I can feel for your pain brother, what a ridiculous bureaucratic nightmare. Obviously this one engineer caused you endless grief and pain, did any of the other engineers ever do a study on the Component Authority and show how he was costing the company L40,000 per component approval? One must remember to use the same tools that management uses against us to show where your problems are crimping development and especially delaying development schedules. You know, use the old product cycle curve to show that two weeks delay will result in a loss of 1+ million pounds over the life of the product? Possibly you could obsolete your Component Authority shortly after he had got himself set-up in the position and you had time to gather a few real examples to demonstrate your beef against the process. You will note that in my explanation I did not specify a singular librarian or component CAD designer. Where possible this should be a shared responsibility, possibly with a senior designer acting as a quick check point before the components are released upon the world. The senior designer would also act to determine who was qualified/unqualified to create new components in the first place. The tertiary function of the this senior designer would be to see that all of the staff received suitable training on the creation of CAD library components so that the individuals are qualified to create their own component requirements within the company guidelines or requirements. I am a firm believer in empowerment, not officious management. Sincerely, Brad Velander Lead PCB Design Norsat International Inc. #100 - 4401 Still Creek Dr., Burnaby, B.C., Canada. V5C6G9. voice: (604) 292-9089 (direct line) fax:(604) 292-9010 email: [EMAIL PROTECTED] www: www.norsat.com -Original Message- From: Terry Harris [mailto:[EMAIL PROTECTED]] Sent: Friday, February 23, 2001 5:12 PM To: Multiple recipients of list proteledausers Subject: Re: [PROTEL EDA USERS]: Library Management On Fri, 23 Feb 2001 13:48:18 -0800, you wrote: Sounds great and how can any engineer regardless of diversity of cultures complain about finding all parts in one library ready checked and approved? Let me tell you my experience as a contract (circuit/software) design engineer in a company that took your rule a little further. Working on a large project (and I mean large) some young aspiring engineer come up with statistics showing that each different component used in the project was going to cost the company around L20,000 in overheads associated with buying stocking and maintaining spares. Compared to a previous project if engineers just used a little more commonality the company would save millions. That engineer was appointed the project component authority and a project part database and CAD libraries were set up. To use a component in your design which was not already in the approved database required you to fill out a request form with written justification of your need to use that component and proof that no other existing component could be substituted. The request was passed on to the project component engineer who checked and reported on availability and obtained data sheets for the project library. The request was then passed on to the component authority who had to approve the request. This often resulted in a simple NO and you try again or eventually have a meeting where you had to verbally argue your request and were sometimes asked to go talk to other project engineers to see if an approved component they were using could be replaced by something else which both of you could use. Approved components then got passed on to the CAD library manager to be added to his list awaiting symbol and footprint creation. I don't think this process ever happened in less than a week and if anyone in the chain was sick or on holiday or off site the process stalled till they got back. The component authority maintained an overall project component type count which was obviously calibrated in management brownie points he would get for saving the company all this notional money. snip Cheers, Terry. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * This message sent by: PROTEL EDA USERS MAILING LIST * * Use the reply command in your email program to * respond to this message. * * To unsubscribe from this mailing list use the form at * the Association web site. You will need to give the same * email address you originally used to subscribe (do not * give an alias unless it was used to subscribe). * * Visit http://www.techservinc.com/protelusers/subscrib.html * to unsubscribe or to subscribe a new email address. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * To leave the EDAFORUM discussion list, send a email with 'leave edaforum' in the body to '[EMAIL PROTECTED]' More Information : http://www.dolist.net
