Re: [PEDA] Assembly drawings
Mr. Lomax Thank you for the information it will work for this project. However I would like to have this done automatically, one less thing too worry about and one less thing for someone to forget. I would like to build a server to do what it is I need to have done, I have never tried something like this and was hoping that some one could give me some guidance or lead me into the right direction on how to get started, and what I might need. I looked into the Protel archives and didn't find any information on building servers or what I need to get started. Regards, Ted -Original Message- From: Abd ul-Rahman Lomax [mailto:[EMAIL PROTECTED] Sent: Wednesday, October 15, 2003 6:16 PM To: Protel EDA Forum; [EMAIL PROTECTED] Subject: Re: [PEDA] Assembly drawings At 03:47 PM 10/15/2003, [EMAIL PROTECTED] wrote: I have been given the task to add assembly drawings to a design that another engineer is working on using protel 99SE. I would like to go into the library that he is currently using and just add a mechanical layer 1 to each part with a .comment string, and update the PCB from the library. There are about 100 parts on the secondary side of the PCB, is there a way to automatically change the mechanical layer to layer 2 with out having to select each out line and cut it and past it on another layer for the parts on the secondary side of the PCB? Is there another way that this can be accomplished that I am should be looking into. Okay, let me see if I understand this. In infer that what you want is an assembly drawing and for this you want to use a .comment string because that string will normally hold type information from schematic. Further, the PCB you are working with has components on both sides, so you want to make two assembly layers, one for top and one for bottom. This is actually pretty routine. Let me suggest that you don't want to change the footprints in the library. Every part already has a .comment string unless you have done something to remove it. What you want to do is to make it visible and move it to the appropriate layer. This is not complicated to accomplish. First, to make working simple, double-click on any reference designator and use a global edit to hide all designators -- you can bring them back later. Then double-click on any component and use another global edit on the Comment tab to make all comments visible. Then double-click on any Top Side Comment and globally edit all comments on the Top Overlay layer (assuming that it is on the default layer) to the Mech layer you want to use. Normally, I'd be using Mech 1 for outline, so I'd choose a different one. Whatever layer I choose, I'd name it functionally, so, in this case, I'd end up moving all the Top Overlay Comments to Top Assembly. Then I would likewise move all Bottom Overlay Comments to Bot Assembly. I think Mr. Tontis knows how to use global edits properly, so I haven't included details about that I might then bring back all the reference designators. If I want both reference designators and comments on the assembly drawings, I might use the autopositioning feature to place them in complementary positions, or it might be necessary to manually retouch the positions, or it might not be possible to have both. If I want both, I'd simply merge, in a plot, Outline, Top Overlay, and Top Assy layers. If there is room, I'd also have top and multilayer pads in the plot. Anyway, all this is a few minutes work, except for the retouching of text positions if that is needed. This email and any files transmitted with it are confidential and intended solely for the use of the individual or entity to whom they are addressed. If you have received this email in error please notify the system manager. This message contains confidential information and is intended only for the individual named. If you are not the named addressee you should not disseminate, distribute or copy this e-mail. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Assembly drawings
At 12:06 PM 10/21/2003, you wrote: Mr. Lomax Thank you for the information it will work for this project. However I would like to have this done automatically, one less thing too worry about and one less thing for someone to forget. I would like to build a server to do what it is I need to have done, I have never tried something like this and was hoping that some one could give me some guidance or lead me into the right direction on how to get started, and what I might need. I looked into the Protel archives and didn't find any information on building servers or what I need to get started. If your company procedures require an assembly drawing, you won't be able to forget it. I know that the process can be automated, and it can probably be automated within Protel, someone else will be able to write more about that. I'd be tempted to do it off-line. Since I think the ASCII database is not as complete as the binary at this time (is this also true for DXP?), I'd think of writing the ASCII PCB file, processing it to create a new PCB file with the necessary primitives, loading that file, and copying the new stuff into the original file. This is not at all a difficult task, which is why I'd think of doing it that way. It is easy enough to do it manually that I never got around to automating the process. If you do more than one assembly drawing a week, it would probably be worth it. And, of course, a utility would be of interest to other users. I'd suggest some discussion first to hash out exactly what the utility would do, what options would it have, etc. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
[PEDA] Assembly drawings
I have been given the task to add assembly drawings to a design that another engineer is working on using protel 99SE. I would like to go into the library that he is currently using and just add a mechanical layer 1 to each part with a .comment string, and update the PCB from the library. There are about 100 parts on the secondary side of the PCB, is there a way to automatically change the mechanical layer to layer 2 with out having to select each out line and cut it and past it on another layer for the parts on the secondary side of the PCB? Is there another way that this can be accomplished that I am should be looking into. Regards, Ted Tontis CID Engage Networks Inc. 1320 N. Dr. Martin Luther King Drive River Level Milwaukee, WI 53212 PH 414-918-4267 FX 414-273-7601 This email and any files transmitted with it are confidential and intended solely for the use of the individual or entity to whom they are addressed. If you have received this email in error please notify the system manager. This message contains confidential information and is intended only for the individual named. If you are not the named addressee you should not disseminate, distribute or copy this e-mail. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Assembly drawings
Hi Ted You could try selecting all the components on the bottom layer, unlock their primitives, then change the tracks/attributes on mechanical layer 1 to mechanical layer 2 - that applies to the bottom assembly drawing. Make sure when you do the global change that you match by selection and layer and set the scope to all primitives. You'll have to perform this operation for each of tracks (make sure you include arcs - subtle checkbox on the bottom right of the change track dialogue box), strings and any other item. After doing this, also make sure you re-lock the component primitives. I hope this isn't too garbled. Cheers, Brendon. [EMAIL PROTECTED] 10/16/03 08:47 AM Please respond to Protel EDA Forum [EMAIL PROTECTED] To [EMAIL PROTECTED] cc Subject [PEDA] Assembly drawings I have been given the task to add assembly drawings to a design that another engineer is working on using protel 99SE. I would like to go into the library that he is currently using and just add a mechanical layer 1 to each part with a .comment string, and update the PCB from the library. There are about 100 parts on the secondary side of the PCB, is there a way to automatically change the mechanical layer to layer 2 with out having to select each out line and cut it and past it on another layer for the parts on the secondary side of the PCB? Is there another way that this can be accomplished that I am should be looking into. Regards, Ted Tontis CID Engage Networks Inc. 1320 N. Dr. Martin Luther King Drive River Level Milwaukee, WI 53212 PH 414-918-4267 FX 414-273-7601 This email and any files transmitted with it are confidential and intended solely for the use of the individual or entity to whom they are addressed. If you have received this email in error please notify the system manager. This message contains confidential information and is intended only for the individual named. If you are not the named addressee you should not disseminate, distribute or copy this e-mail. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Assembly drawings
At 03:47 PM 10/15/2003, [EMAIL PROTECTED] wrote: I have been given the task to add assembly drawings to a design that another engineer is working on using protel 99SE. I would like to go into the library that he is currently using and just add a mechanical layer 1 to each part with a .comment string, and update the PCB from the library. There are about 100 parts on the secondary side of the PCB, is there a way to automatically change the mechanical layer to layer 2 with out having to select each out line and cut it and past it on another layer for the parts on the secondary side of the PCB? Is there another way that this can be accomplished that I am should be looking into. Okay, let me see if I understand this. In infer that what you want is an assembly drawing and for this you want to use a .comment string because that string will normally hold type information from schematic. Further, the PCB you are working with has components on both sides, so you want to make two assembly layers, one for top and one for bottom. This is actually pretty routine. Let me suggest that you don't want to change the footprints in the library. Every part already has a .comment string unless you have done something to remove it. What you want to do is to make it visible and move it to the appropriate layer. This is not complicated to accomplish. First, to make working simple, double-click on any reference designator and use a global edit to hide all designators -- you can bring them back later. Then double-click on any component and use another global edit on the Comment tab to make all comments visible. Then double-click on any Top Side Comment and globally edit all comments on the Top Overlay layer (assuming that it is on the default layer) to the Mech layer you want to use. Normally, I'd be using Mech 1 for outline, so I'd choose a different one. Whatever layer I choose, I'd name it functionally, so, in this case, I'd end up moving all the Top Overlay Comments to Top Assembly. Then I would likewise move all Bottom Overlay Comments to Bot Assembly. I think Mr. Tontis knows how to use global edits properly, so I haven't included details about that I might then bring back all the reference designators. If I want both reference designators and comments on the assembly drawings, I might use the autopositioning feature to place them in complementary positions, or it might be necessary to manually retouch the positions, or it might not be possible to have both. If I want both, I'd simply merge, in a plot, Outline, Top Overlay, and Top Assy layers. If there is room, I'd also have top and multilayer pads in the plot. Anyway, all this is a few minutes work, except for the retouching of text positions if that is needed. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Assembly Drawings (ex Bug - Move Selection ...)
At 03:32 PM 4/6/01 +1000, Geoff Harland wrote: That is all very well, but text information is lost when you create Gerber files and then import them back into Protel again (on a different layer); each letter within each string gets converted into strokes (within the Gerber files), and as such, gets converted into non-text material. If I were to then create Acrobat files from such a PCB file, other users would not be able to search for R104 (say) on the Assembly drawing page(s) while using Acrobat's (text) searching feature This is correct. If you want more than graphics, the gerber import method I use would be less than satisfactory. However, this is a case where it would not be difficult to write a server or utility that would place text strings as needed on the mech layer of choice, from the relevant overlay layer. Abdulrahman Lomax Food for thought. I reported the problem concerning the usage of Windows fonts (to both Protel and this forum) before SP6 was released, and had hopes that this problem would be rectified by SP6. (Regrettably, that was not the case.) An optimistic interpretation would be that my report occurred too late in the piece for Protel to rectify the associated problem in SP6, but that this will be rectified in SP7. However, if for whatever reason this is *not* rectifed in SP7 (such as Protel not regarding this problem of being of sufficient seriousness to rectify, for instance), then the longer it takes for me to create a suitable process in an addon server, the longer I will have to keep on mirroring PCBs in order to produce top side Assembly Drawings of a satisfactory nature. So at the risk of spending some time on a process which might not be required after SP7 is released, I will at least consider creating something which will create a mirrored image of the Top Overlay layer (and the pads on the Top signal and MultiLayer layers) on one (or two?) of the Mechanical layers. Such a process would also allow me to create both the Top side Assembly Drawing and the Bottom side Assembly Drawing in one hit (and if I so wanted, on the *same* page rather than on separate pages). It shouldn't take an undue amount of time to write the associated code... Would such a process be of interest to you, or other users, as well? (You could avoid the requirement of having to generate Gerber files and then importing them back onto one or more Mechanical layers.) If I have reason to believe that other users would also be interested in this capability (even if it is used for other reasons), I would be more motivated to put the required time in. 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 join or leave this list visit: * http://www.techservinc.com/protelusers/subscrib.html * - or email - * mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] Assembly Drawings
snip There are two desireable utilities, really. (1) Make a fabrication drawing: create drill symbols and a drill chart on a specified layer. (2) Make an assembly drawing: take a layer, mirrored or not mirrored, and copy it to a specified layer. We've been discussing item 2. A top or bottom overlay, plus a top or bottom padmaster, usually will make a pretty good basic assembly drawing; one adds format and notes, etc. snip The existing tools work, but it could be a smoother process, and being unable to see the drill chart in the PCB editor is a general nuisance. I can understand why they did it, though. Abdulrahman Lomax While the initial idea was to facilitate creating Assembly Drawings, layer imaging could certainly be generalised to support copying/imaging any source layer to any destination layer, and with optional mirroring (and an optional offset, especially when mirroring is *not* selected, but arguably also relevant even when mirroring *is* selected); in other words, item 2 above. A case could probably also be made for being able to qualify which primitives on the source layer get to be imaged to the destination layer, such as arcs, fills, ... , polygons, component Designator strings, etc. That suggests a dialog box with similarities to the one provided for configuring layers (within Printout definitions) in the PCB Power Print Server. (My preference would be for additionally providing support for parameters so that users could then avoid having to invoke that dialog box, should they so wish.) I confess to having mused about item 1 above, or functionality of a similar nature, from time to time. In particular, my vision has been of creating full circle-arcs on a particular layer whose locations and diameters match all holes in the PCB file; i.e. such a full-circle arc for each (and every) hole. A printout from such a layer would differ from printouts from Drill Drawing and Drill Guide layers, but still be similar, in the sense that it would also document holes in the PCB file. But while the Power Print Server does provide enhanced capabilities as far as printouts in general are concerned, perhaps there is something to be said for users being able to acquire yet more capability when it comes to creating customised printouts that document holes/drilling information. So I will also give some thought to the idea of adding assorted types of primitves to a particular layer to document such details (and of being able to update such information when so requested?). It is also fair enough to say that highly-polished products would not necessarily be released first-time. But certainly these could evolve as users acquire experience in using these... 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 join or leave this list visit: * http://www.techservinc.com/protelusers/subscrib.html * - or email - * mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum * * Contact the list manager: * mailto:[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
