Re: [PEDA] PCB breakoffs
Ian, Effectively, this kind of PCB are only used with stable mechanical support (generally machined RF enclosures). The optional breakable part of the PCB is considered like a totally independent print with it's own mechanical fixation; holes have sufficient tolerances in diameter to avoid constraints. The only precautions are taken during components placement, soldering, initial test and transport, In fact, it is as if we had 2 well fixed independant PCB connected by some resistors. Have a nice day, Rudolf - Original Message - From: Ian Wilson [EMAIL PROTECTED] To: Protel EDA Forum [EMAIL PROTECTED] Sent: Wednesday, June 26, 2002 10:19 AM Subject: Re: [PEDA] PCB breakoffs On 08:15 AM 26/06/2002 +0200, Rudolf Schaffer said: Hello, In this case, we use v-grooving and SMD 0 ohm with a convenient foot-print, for each net (if not too many!) crossing over. We naturally have 2 plans d'implantation depending upon the cutted/non cutted PCB part. Have a nice day, Rudolf Schaffer Rudolf, I am intrigued by this. How do you prevent flexing of the board from transferring stress onto the small surface mount resistors and cracking them or the solder joints? A V-groove flexes at quite a sharp angle. (by design). I guess some thing like this would never be used in anything but very stable controlled environments. Actually now that I think about it this stress is a problem also for the routed/break-off tab implementation but maybe the copper is a little more malleable than those ceramic resistors. Ian Wilson * Tracking #: 533015C9F8865B4F90F49353E155EDDCD7B65F11 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] PCB breakoffs
Hello, In this case, we use v-grooving and SMD 0 ohm with a convenient foot-print, for each net (if not too many!) crossing over. We naturally have 2 plans d'implantation depending upon the cutted/non cutted PCB part. Have a nice day, Rudolf Schaffer RD Engineer Phone +41 32 754 38 33 Fax +41 32 754 38 36 Web www.livetools.tv - Original Message - From: Bagotronix Tech Support [EMAIL PROTECTED] To: Protel EDA Forum [EMAIL PROTECTED] Sent: Monday, June 24, 2002 9:16 PM Subject: [PEDA] PCB breakoffs Hello, all: We have had our domain transferred to a new ISP last week, so e-mail has just begun working normally (I hope!). Anyway, I want to make a PCB that has a break-off area with extra circuitry on it. The idea is that some users may not need the extra circuitry, so they can break off that area of the board to reduce the size. I know this is easy for cheap PCB material (phenolic, etc.) but does this work with FR-4 and such? If this is feasible with FR-4, what technique should I use to make the break-off? I assume I will have to lay out a bunch of unplated holes spaced in a line, with traces going inbetween holes. And I assume that the way to indicate this to the fab is to put comments on the drill layer. Thanks in advance for your help. If no one replies, I will assume our e-mail still isn't working right. Best regards, Ivan Baggett Bagotronix Inc. website: www.bagotronix.com * Tracking #: E0D56A16817ACA4091A0139DC100BD9938215AA3 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] PCB breakoffs
I used via/hole size of 1mm/0.7mm. Could be smaller if they had sharp tool for V-grooving. Igor -Original Message- From: Danny Bishop [mailto:[EMAIL PROTECTED]] Sent: Wednesday, 26 June 2002 2:44 PM To: 'Protel EDA Forum' Subject: Re: [PEDA] PCB breakoffs not a bad idea if you use big vias -Original Message- From: Igor Gmitrovic [mailto:[EMAIL PROTECTED]] Sent: Wednesday, 26 June 2002 11:44 AM To: Protel EDA Forum Subject: Re: [PEDA] PCB breakoffs Ivan, you could V-groove the board and put vias on the tracks where they cross the V-groove line. Igor -Original Message- From: Jim McGrath [mailto:[EMAIL PROTECTED]] Sent: Tuesday, 25 June 2002 11:14 PM To: Protel EDA Forum Subject: Re: [PEDA] PCB breakoffs Ivan, Yes you can use FR4. I would score the board and use ribbon cable to interconnect from board A to board B. Jim Bagotronix Tech Support wrote: Hello, all: We have had our domain transferred to a new ISP last week, so e-mail has just begun working normally (I hope!). Anyway, I want to make a PCB that has a break-off area with extra circuitry on it. The idea is that some users may not need the extra circuitry, so they can break off that area of the board to reduce the size. I know this is easy for cheap PCB material (phenolic, etc.) but does this work with FR-4 and such? If this is feasible with FR-4, what technique should I use to make the break-off? I assume I will have to lay out a bunch of unplated holes spaced in a line, with traces going inbetween holes. And I assume that the way to indicate this to the fab is to put comments on the drill layer. Thanks in advance for your help. If no one replies, I will assume our e-mail still isn't working right. Best regards, Ivan Baggett Bagotronix Inc. website: www.bagotronix.com ** ** * Tracking #: FA14B7B41BC3F5459A4E929EDF87298D738F4111 * ** ** * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] PCB breakoffs
On 08:15 AM 26/06/2002 +0200, Rudolf Schaffer said: Hello, In this case, we use v-grooving and SMD 0 ohm with a convenient foot-print, for each net (if not too many!) crossing over. We naturally have 2 plans d'implantation depending upon the cutted/non cutted PCB part. Have a nice day, Rudolf Schaffer Rudolf, I am intrigued by this. How do you prevent flexing of the board from transferring stress onto the small surface mount resistors and cracking them or the solder joints? A V-groove flexes at quite a sharp angle. (by design). I guess some thing like this would never be used in anything but very stable controlled environments. Actually now that I think about it this stress is a problem also for the routed/break-off tab implementation but maybe the copper is a little more malleable than those ceramic resistors. Ian Wilson * Tracking #: 533015C9F8865B4F90F49353E155EDDCD7B65F11 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] PCB breakoffs
Just FYI Design for breakaway tabs can be found in IPC Standard IPC- although I personally don't find it very helpful... Tim Fifield -Original Message- From: Danny Bishop [mailto:[EMAIL PROTECTED]] Sent: Tuesday, June 25, 2002 8:39 PM To: 'Protel EDA Forum' Subject: Re: [PEDA] PCB breakoffs Ivan the technique you describe is a standard way to panelize/depanelize boards with FR4( to be used with routing, rather than scoring/v-grooving), but I don't know about running tracks between them. I wouldn't break it off with copper connecting the two parts together. Perhaps you should consider an IDC connector between the two. Danny -Original Message- From: Bagotronix Tech Support [mailto:[EMAIL PROTECTED]] Sent: Tuesday, 25 June 2002 5:16 AM To: Protel EDA Forum Subject: [PEDA] PCB breakoffs Hello, all: We have had our domain transferred to a new ISP last week, so e-mail has just begun working normally (I hope!). Anyway, I want to make a PCB that has a break-off area with extra circuitry on it. The idea is that some users may not need the extra circuitry, so they can break off that area of the board to reduce the size. I know this is easy for cheap PCB material (phenolic, etc.) but does this work with FR-4 and such? If this is feasible with FR-4, what technique should I use to make the break-off? I assume I will have to lay out a bunch of unplated holes spaced in a line, with traces going inbetween holes. And I assume that the way to indicate this to the fab is to put comments on the drill layer. Thanks in advance for your help. If no one replies, I will assume our e-mail still isn't working right. Best regards, Ivan Baggett Bagotronix Inc. website: www.bagotronix.com ** ** * Tracking #: E0D56A16817ACA4091A0139DC100BD9938215AA3 * ** ** * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] PCB breakoffs
I would use a ribbon cable that was previously suggested, or use a flex circuit. Running traces to the edge of a board would cause lamination and corrosion problems. If the copper is run through the tab and then the board is snapped apart that copper track will be exposed on the edge. Also there would be no ground or power plane under the tracks, unless it is not a multilayer board After removal of the unneeded card it could be possible for those tracks to become an unwanted antenna. Regards, Ted * Tracking #: EDA8C6609E34194CA37E9C3B230CC8E9EB73FAA0 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] PCB breakoffs
i concur with this i can say from experience that running traces through the breakaway area is problematic ok for protos maybe the traces tear and flop around, sometimes peeling way back for limited production you could dremel a 'wide' area of the trace and then break away Dennis Saputelli [EMAIL PROTECTED] wrote: I would use a ribbon cable that was previously suggested, or use a flex circuit. Running traces to the edge of a board would cause lamination and corrosion problems. If the copper is run through the tab and then the board is snapped apart that copper track will be exposed on the edge. Also there would be no ground or power plane under the tracks, unless it is not a multilayer board After removal of the unneeded card it could be possible for those tracks to become an unwanted antenna. Regards, Ted * Tracking #: EDA8C6609E34194CA37E9C3B230CC8E9EB73FAA0 * -- ___ 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 * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
