Re: [PEDA] metric footprint
John, Assume that you don't have any info from the mfg other than the package dimensions. How do you then come up with a footprint? Specifically, I find that the dimensions requested by Protel are typically not the dimensions provided by the mfg datasheet, so it can get confusing to figure out where the pads need to be. As an example, I've got a 8x8 QFP (specifically an FTDI FT232BM USB chip) that apparently isn't a standard package. In going through the Protel process of creating a custom footprint, the dimensions given in the datasheet tell the size of the plastic package and the extent of the pins, but Protel wants the distance between the center of the pads from one side to the other and the vertical distance between the the centerline of the horizontal pins and the nearest vertical pin. These calculations, at least for me, seem to take several tries before I get something that looks right. Moreover, selecting a pad size seems arbitrary at first glance, but I'm sure there are good conventions for chosing the pad size. If there are rules of thumb for determining pad size, I'm interested in knowing them, so if you know of any, lead on. Bryn Wolfe John Haddy wrote: Try: http://tsc.jeita.or.jp/eds/DATA/PACKAGE/ED731120.PDF John Haddy -Original Message- From: Rene Tschaggelar [mailto:[EMAIL PROTECTED] Sent: Tuesday, 3 June 2003 6:51 PM To: Protel EDA Forum Subject: Re: [PEDA] metric footprint Is there no footprint given in a manufacturers datasheet ? It just a minute or two to make this footprint, much faster than a websearch. Rene * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] metric footprint
Bryn, The IPC has a calculator at http://landpatterns.ipc.org/default.asp that can assist with the land pattern design. But be warned: there's a fundamental flaw with IPC-SM-782 calculation method that adds all tolerances together (thus assuming that every parameter will be at worst-case condition at the same time) rather than taking the root-mean-square of the tolerances (which is a more statistically appropriate calculation). The effect of this is that if you enter every parameter at its full tolerance limits, you'll end up with a land pattern design that's far larger than it needs to be in reality. I usually trim some values (e.g. side fillet=0) as a matter of course. I also do two designs with the calculator: one with all parameters at nominal (no min/max variation); and one with the full tolerances entered. I then compare the two and pick a middle ground based on experience and manufacturability. For example, the calculator will happily cough up lands that are so wide that manufacturing design-rule-violating solder mask slivers will result between adjacent lands. For gull-wing type packages, I usually start with the assumption that I'm happy with 0 heel fillet when the IC pins are at minimum spacing, while I want a toe fillet of the same width as the thickness of the lead when the pins are at their maximum spacing. There's also some fundamental differences between land patterns that are intended for wave soldering versus those designed for reflow (in general, reflow patterns can have smaller lands). This type of thing should be discussed with your assembler since they'll have lots of experience with what doesn't work. Despite its flaws, IPC-SM-782 is still a useful document (the front part, not the cheat sheets in the back half) and I'd recommend that all designers at least read the text to understand the philosophyof land pattern design. Hope this helps, John Haddy -Original Message- From: Bryn Wolfe [mailto:[EMAIL PROTECTED] Sent: Wednesday, 4 June 2003 1:09 AM To: Protel EDA Forum Subject: Re: [PEDA] metric footprint John, Assume that you don't have any info from the mfg other than the package dimensions. How do you then come up with a footprint? Specifically, I find that the dimensions requested by Protel are typically not the dimensions provided by the mfg datasheet, so it can get confusing to figure out where the pads need to be. As an example, I've got a 8x8 QFP (specifically an FTDI FT232BM USB chip) that apparently isn't a standard package. In going through the Protel process of creating a custom footprint, the dimensions given in the datasheet tell the size of the plastic package and the extent of the pins, but Protel wants the distance between the center of the pads from one side to the other and the vertical distance between the the centerline of the horizontal pins and the nearest vertical pin. These calculations, at least for me, seem to take several tries before I get something that looks right. Moreover, selecting a pad size seems arbitrary at first glance, but I'm sure there are good conventions for chosing the pad size. If there are rules of thumb for determining pad size, I'm interested in knowing them, so if you know of any, lead on. Bryn Wolfe John Haddy wrote: Try: http://tsc.jeita.or.jp/eds/DATA/PACKAGE/ED731120.PDF John Haddy -Original Message- From: Rene Tschaggelar [mailto:[EMAIL PROTECTED] Sent: Tuesday, 3 June 2003 6:51 PM To: Protel EDA Forum Subject: Re: [PEDA] metric footprint Is there no footprint given in a manufacturers datasheet ? It just a minute or two to make this footprint, much faster than a websearch. Rene * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] metric footprint
I'm not familiar with any current work reflecting this. (Doesn't mean that I'm up to the minute with my reading though...) IPC-SM-782a suggests (section 3.3.3.1) fillets in the range of: Toe: 0.4mm - 0.6mm Heel: 0.0mm - 0.2mm Side: -0.02mm - 0.02mm I've always been wary of excess heel fillet since, to my way of thinking, extra metal in this region must necessarily restrict the ability of a lead to flex in accomodation of thermal stresses. Note that this is my assumption rather than having a basis in any published work. I note, though, that in the example land patterns in the back of IPC-SM-782a the QFP toe and heel fillets are generally about equal. John Haddy -Original Message- From: Ian Wilson [mailto:[EMAIL PROTECTED] Sent: Wednesday, 4 June 2003 10:00 AM To: Protel EDA Forum Subject: Re: [PEDA] metric footprint On 08:24 AM 4/06/2003, John Haddy said: ..snip.. For gull-wing type packages, I usually start with the assumption that I'm happy with 0 heel fillet when the IC pins are at minimum spacing, while I want a toe fillet of the same width as the thickness of the lead when the pins are at their maximum spacing. I thought I had read somewhere, or seen in a seminar or something, that the heel is the dominant fillet and the toe is less relevant. If this is the case wouldn't you need to ensure a suitable minimum heel fillet and let the toe fillet reduce in length under worst case conditions? Are there any current references on heel fillet v toe fillet? Thanks, 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/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
Re: [PEDA] metric footprint
John Haddy wrote: I'm not familiar with any current work reflecting this. (Doesn't mean that I'm up to the minute with my reading though...) IPC-SM-782a suggests (section 3.3.3.1) fillets in the range of: Toe: 0.4mm - 0.6mm Heel: 0.0mm - 0.2mm Side: -0.02mm - 0.02mm I've always been wary of excess heel fillet since, to my way of thinking, extra metal in this region must necessarily restrict the ability of a lead to flex in accommodation of thermal stresses. Note that this is my assumption rather than having a basis in any published work. I note, though, that in the example land patterns in the back of IPC-SM-782a the QFP toe and heel fillets are generally about equal. John Haddy I would always ensure that there is some heel fillet as this is often the strongest external part of the joint. In many cases the toe of a lead can solder quite poorly (it is not tinned due having been cropped after the lead was plated). A sound heel filet prevents a weak solder joint lifting due to crack propagation from the thermal expansion of the package. if you have no heal fillet then any expansion forces are concentrated at the pad/foot interface with the peel action concentrated by the small size of the interface normal to the direction of the force. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] metric footprint
Is there no footprint given in a manufacturers datasheet ? It just a minute or two to make this footprint, much faster than a websearch. Rene Tim Fifield wrote: Does anybody have a footprint for a SSOP24-P-300-1.00B? The part is a Toshiba TPD7203F gate driver IC. Pin pitch is 1mm and body with pin width is 8mm. IPC-SM-782 book doesn't have anything and I can't quickly find anything else on the web. I'm going to keep searching but I thought I'd ask here too. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] metric footprint
Try: http://tsc.jeita.or.jp/eds/DATA/PACKAGE/ED731120.PDF John Haddy -Original Message- From: Rene Tschaggelar [mailto:[EMAIL PROTECTED] Sent: Tuesday, 3 June 2003 6:51 PM To: Protel EDA Forum Subject: Re: [PEDA] metric footprint Is there no footprint given in a manufacturers datasheet ? It just a minute or two to make this footprint, much faster than a websearch. Rene Tim Fifield wrote: Does anybody have a footprint for a SSOP24-P-300-1.00B? The part is a Toshiba TPD7203F gate driver IC. Pin pitch is 1mm and body with pin width is 8mm. IPC-SM-782 book doesn't have anything and I can't quickly find anything else on the web. I'm going to keep searching but I thought I'd ask here too. * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * 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] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *