Re: [PEDA] Shortened Designator on Silkscreen
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
Re: [PEDA] Shortened Designator on Silkscreen
Solution 1. Use different numbering R1, R101, R201... for the different channels. Solution 2. Provide a separate drawing of the silk screen (in PDF format for example) to your assembly house. You can place the text inside the part outlines. There won't be mistakes. Mira --- JaMi Smith [EMAIL PROTECTED] wrote: I have a small problem with small parts in a small area on a small board (so what else is new?). I have 4 parallel channels of a Quad Transimpedance Amplifier circuit, which is very high gain and requires good isolation. The circuit is all descrete analog components, mostly 0402, except for the S0-8 op-amps, and is packaged quite densely with only .020 between components in the tight spots, and no room for package outlines. The circuit is layed out very nicely, and is electrically excellent, but unfortunately, there is no room for designators. 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. 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. 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. 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. 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. 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. 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. 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. 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. Anyone out there got any useful ideas? JaMi Smith * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * __ Do You Yahoo!? Yahoo! Games - play chess, backgammon, pool and more http://games.yahoo.com/ * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Shortened Designator on Silkscreen
What I have done is to unhide the Comment field and use it to label small components so the Ref Des is not changed and therefore corresponds with the schematic/netlist. Obviously everybody involved needs to understand and approve such a shortcut. I then show the Ref Des on the Assembly drawing where the IC is to be placed. On one design that had multiple identical channels, a box (Top Overlay and Bottom Overlay) was drawn around the identical sections and a Text Field added to the Box saying Channel N and then the individual components were just labeled (using the Comment) as you indicated using the shortened designator. Since all Rn in the channels were identical and there were no other Rns (i.e. make sure that if you have R1-1, R1-2, etc. there is no R1 in the non repeated section of the board) the assembly personnel had no difficulty stuffing the boards. On another design, I was asked to use Alpha characters for the indicators (again using comments) so I had sections that looked like alphabet soup! JaMi Smith wrote: I have a small problem with small parts in a small area on a small board (so what else is new?). * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Shortened Designator on Silkscreen
Those components are supposed to be placed by machine aren't they ? If not, you should get better trained people, or instruct them differently. Or have a placement plan in 10 to 1 size on paper. And do the prototypes yourself. Rene -- Ing.Buero R.Tschaggelar - http://www.ibrtses.com JaMi Smith wrote: [ high error rate in manual SMD placement ] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Shortened Designator on Silkscreen
here come the 0201's !!
try putting some text and boxes around those
saw a recent article about hand reworking them
pretty scary
apparently it takes something known as 'operator skill'
re this thread
i think the best idea is what dgulley said
use the comment field and hide the desig
this way the database is still good and you don't have to use 'loose'
text
another idea (depending on how many values) is to use a simple code
like:
'A' or '1' = 1.00K res
'B' or '2' = 0.01m cap
it doesn't tell you which of several is which but it's pretty small and
easy to build this way
JAMI, re: your component to component spacing
can this be pick and placed?
Dennis Saputelli
Dwight wrote:
-Original Message-
From: JaMi Smith [mailto:[EMAIL PROTECTED]]
Sent: Tuesday, April 23, 2002 11:30 AM
snip
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.
Position the refs as if they didn't have the _1, _2...; then it's only 4
global edits -- use the brace notation like this:
{_1=}
That will remove all the _1's; do the same for 2,3, and 4. You can backup
just the .pcb within your current ddb, do the 4 edits, generate the full
gerbers, then copy back the real pcb.
So far we've used notation like R1A, R1B, etc. This saves one character
width. But we're only down to 0603, not 0402 like you! We also supply the
assembly house a printout of the board that's about 2x normal so they can
double-check anything unclear.
--
___
www.integratedcontrolsinc.comIntegrated Controls, Inc.
tel: 415-647-04802851 21st Street
fax: 415-647-3003San Francisco, CA 94110
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] Shortened Designator on Silkscreen
WARNING
after i sent this it occurred to me that the comment field may get
trashed by a netlist load
david can you confirm that this works?
do you use the sync or netlist load?
Dennis Saputelli
Dennis Saputelli wrote:
here come the 0201's !!
try putting some text and boxes around those
saw a recent article about hand reworking them
pretty scary
apparently it takes something known as 'operator skill'
re this thread
i think the best idea is what dgulley said
use the comment field and hide the desig
this way the database is still good and you don't have to use 'loose'
text
another idea (depending on how many values) is to use a simple code
like:
'A' or '1' = 1.00K res
'B' or '2' = 0.01m cap
it doesn't tell you which of several is which but it's pretty small and
easy to build this way
JAMI, re: your component to component spacing
can this be pick and placed?
Dennis Saputelli
Dwight wrote:
-Original Message-
From: JaMi Smith [mailto:[EMAIL PROTECTED]]
Sent: Tuesday, April 23, 2002 11:30 AM
snip
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.
Position the refs as if they didn't have the _1, _2...; then it's only 4
global edits -- use the brace notation like this:
{_1=}
That will remove all the _1's; do the same for 2,3, and 4. You can backup
just the .pcb within your current ddb, do the 4 edits, generate the full
gerbers, then copy back the real pcb.
So far we've used notation like R1A, R1B, etc. This saves one character
width. But we're only down to 0603, not 0402 like you! We also supply the
assembly house a printout of the board that's about 2x normal so they can
double-check anything unclear.
--
___
www.integratedcontrolsinc.comIntegrated Controls, Inc.
tel: 415-647-04802851 21st Street
fax: 415-647-3003San Francisco, CA 94110
--
___
www.integratedcontrolsinc.comIntegrated Controls, Inc.
tel: 415-647-04802851 21st Street
fax: 415-647-3003San Francisco, CA 94110
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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] Shortened Designator on Silkscreen
Sounds like you are using cut and pasted sections and getting Protel to automatically renumber the new pasted sections. Protels renumbering system is very poor - actually unusable, and the best way I found to renumber whilst keeping sch and pcb numbers synced is to download and install a renumbering server from the RSI website. This will allow you to shorten the designators. Another way to ease assembly on tightly packed board is to have a slightly different style of footprint between caps and resistors. Maybe resistors have squared off silkscreen outlines whilst caps have circular outlines so when you look at the board the outlines aid in identifying the part type. ___ Clive Broome IDT Sydney Design CentrePh: +61 2 9763 3513 8 Baywater Dr, Homebush Fax:+61 2 9763 3409 Sydney, NSW, 2127 Email:[EMAIL PROTECTED] Australia ___ JaMi Smith [EMAIL PROTECTED] on 04/24/2002 04:30:27 AM Please respond to Protel EDA Forum [EMAIL PROTECTED] To: Protel EDA Forum [EMAIL PROTECTED] cc: JaMi Smith [EMAIL PROTECTED] (bcc: Clive Broome/sdc) Subject: [PEDA] Shortened Designator on Silkscreen I have a small problem with small parts in a small area on a small board (so what else is new?). I have 4 parallel channels of a Quad Transimpedance Amplifier circuit, which is very high gain and requires good isolation. The circuit is all descrete analog components, mostly 0402, except for the S0-8 op-amps, and is packaged quite densely with only .020 between components in the tight spots, and no room for package outlines. The circuit is layed out very nicely, and is electrically excellent, but unfortunately, there is no room for designators. 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. 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. 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. 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. 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. 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. 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. 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. 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. Anyone out there got any useful ideas? JaMi Smith * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Shortened Designator on Silkscreen
Actually, this is a VERY good point, the Comment IS updated on a netlist load. I have used two methods: a) Set the Comment field in the schematic (assuming I have control) b) edit the macros generated by the netlist load to delete any changes to the comments (these are usually the last macros generated so they are easy to find) It really depends on how many revisions the design will be going through and making sure that ALL non standard design flows are carefully and fully documented within the project. I have not tried it with sync, but would assume that the comments are over written there as well. David W. Gulley Destiny Designs Dennis Saputelli wrote: WARNING after i sent this it occurred to me that the comment field may get trashed by a netlist load david can you confirm that this works? do you use the sync or netlist load? Dennis Saputelli * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] Shortened Designator on Silkscreen
On 09:14 AM 24/04/2002 +1000, [EMAIL PROTECTED] said: ..snip..keeping sch and pcb numbers synced is to download and install a renumbering server from the RSI website. RSI www site or Qualecad web site? I thought the re-numbering server was from John Williams at Qualecad. http://www.qualecad.com/page3.html Look at the Reference Designator Modifier freeware server. 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] Shortened Designator on Silkscreen
Ah yes, Ian is right, bit of brain strain here! Ian Wilson [EMAIL PROTECTED] on 04/24/2002 10:35:35 AM Please respond to Protel EDA Forum [EMAIL PROTECTED] To: Protel EDA Forum [EMAIL PROTECTED] cc:(bcc: Clive Broome/sdc) Subject: Re: [PEDA] Shortened Designator on Silkscreen On 09:14 AM 24/04/2002 +1000, [EMAIL PROTECTED] said: ..snip..keeping sch and pcb numbers synced is to download and install a renumbering server from the RSI website. RSI www site or Qualecad web site? I thought the re-numbering server was from John Williams at Qualecad. http://www.qualecad.com/page3.html Look at the Reference Designator Modifier freeware server. 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] Shortened Designator on Silkscreen
I have a small problem with small parts in a small area on a small board (so what else is new?). I have 4 parallel channels of a Quad Transimpedance Amplifier circuit, which is very high gain and requires good isolation. The circuit is all descrete analog components, mostly 0402, except for the S0-8 op-amps, and is packaged quite densely with only .020 between components in the tight spots, and no room for package outlines. The circuit is layed out very nicely, and is electrically excellent, but unfortunately, there is no room for designators. snip Anyone out there got any useful ideas? JaMi Smith To start off with, this could well be my last post (or else very nearly my last post) from this email address. I'm currently looking for another job (preferably in Sydney, Australia, where I am currently living), with my current job finishing this week (the usual circumstances for this era). But I have recently signed up to these forums from my home email address, so other members of these forums will continue to hear from me on an ongoing basis, but from a different email address. Now on to this thread. It is being wise after the event, and not necessarily the best way to do it, but if you want components R1_1, R1_2, R1_3, and R1_4 (say), then add component R1_1 to the PCB file, then append a R1 string (on the Top Overlay layer) to this component (using the Menu item 'Tools/Convert/Add Selected Primitives to Component'; the component's primitives need to be in an unlocked state at the time), then create the R1_2, R1_3, and R1_4 components from copying the R1_1 component to the (Protel) clipboard and then pasting back into the PCB file, then re-annotating the pasted components as required. The additional R1 string is part of each of these components, and will thus move with its component whenever that component is moved. (Moving the string *relative* to the component will require the component's primitives need to be in an unlocked state at the time though, but keep in mind that the global command feature can be used to unlock (or relock) the primitives of more than one component at a time.) All up though, a lot of extra work is called for, even if it is all planned in advance (to minimise the amount of extra work required). But short of creating a customised addon Process of some sort (for example, one which acts upon currently selected free strings so that these are automatically appended to appropriate components which are also currently selected), I am not sure of any other way of doing it, other than the suggestion made by others to use the component's Comment strings. Concerning the use of Comment strings, the Schematic drawings could still be implemented to display component values (e.g. 10k, 100nF, etc) for each component by using one of the 16 Part Fields for this purpose, and setting the corresponding string to be visible. The Part Type (field) (for each component) could then be used to hold the desired abbreviated Designator (e.g. R1 for components R1_1, R1_2, etc), with the corresponding string set invisible (unless it was desired to keep this visible). When information was passed from the Schematic File(s) to the PCB file, the Comment string of each component would then acquire the desired abbreviated Designator for this, and any subsequent re-synchronisation between the Schematic file(s) and the PCB file would *not* result in these desired abbreviated Designators being lost or over-written for *any* of the components (in the PCB file). Some extra work called for with that method as well, but if planned in advance, the amount of extra work required could again be reduced (and probably substantially). If used, I would strongly recommend the addition of an annotation to the Schematic file(s), documenting the usage of this technique. Regards, Geoff Harland. - E-Mail Disclaimer The Information in this e-mail is confidential and may be legally privileged. It is intended solely for the addressee. Access to this e-mail by anyone else is unauthorised. If you are not the intended recipient, any disclosure, copying, distribution or any action taken or omitted to be taken in reliance on it, is prohibited and may be unlawful. Any opinions or advice contained in this e-mail are confidential and not for public display. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
