Hi Mathew, IPC-782-A is meant to be very much only a guide - it was generated by about 200 companies sending volunteers to the IPC sub-committee, and as a result gives dimensions, pad sizes and specifications which will virtually guarantee manufacturability for any assembly process. That's the rub - 782A has a poor reputation for being something it isn't, and it was never meant to be a definitive document because of the broad range of requirements designers face. Some designers complain bitterly that its suggestions are very broad and no help at all in tight boards. I think most designers expect it to give minimum sizes so that they know what they can get away with, but that particular issue depends on your assembly process and your board fab shop. In your case, use it (782A) as a guide. Talk first with your assembly people about solder paste deposition tolerances, component placement accuracy and tolerance and reflow/wave soldering requirements. Talk then with your board fabricator about types of solder mask, solder mask fabrication tolerances and track widths/spaces and tolerances. Then sit down and plan your board before you start - how much room you have for placement and tracking will be your major decision. Then work out your pad sizes, track sizes and placement clearances to get to where you want to go. Any one of us could give you lots of specific recommendations - they'll all be a little different. For example, I do mobile phone layouts and I bet my pads are smaller than most, but that's only because they have to be to get everything to fit. If you're looking for something more definite, Jim Blankenhorn at SMT Plus has a series of manuals with defined sizes that you might find useful. I've spoken with a number of designers who use his manual (and libraries now too, I think) and they say they've never had trouble. Might be worth your while to chase that up. If I can help you some more, email me directly at [log in to unmask] Cheers Andy Kowalewski (972) 550 6365 ____________________Reply Separator____________________ Subject: [DC] IPC-SM-720A pad dimensions etc? Author: Matthew Lamkin <[log in to unmask]> Date: 3/10/00 3:55 PM Hi there, can someone clearup/clarify some little problems that I have in understanding the dimensioning of SMT pads from this std etc. What I'm trying to do is re-create the footprints that I use with Cadstar3, to be what the IPC-SM-782A specifies them to be, as we have recently got new pick & place machines that can use these pads instead of the extremely massive ones that we had to use with the old machines. First off, the 0805 resistor's: Subsection 8.1 page 3, says that the grid placement courtyard is measured in 0.5mm x 0.5mm squares, and that the 0805 uses a 4x8 courtyard. This equates to 4mm x 2mm. Therefor this leaves a placement gap between the pads of 0.4mm at the ends & 0.25mm along the length. However any other books that I have, say that I should leave a minimum of 1mm gap between the pads, which means that I should be creating a placement outline 0.5mm from the edge of the pads. Can I reduce this placement gap to that in the standard now? or am I interpreting it wrongly? Next 1206 resistors: The same subsection says that the grid placement courtyard is to be 4x10 (2mm x 5mm). This leaves 0.3mm at the ends & 0.1mm along the length. Surely this is wrong, as it is smaller than the 0805, can someone clarify this for me. Next problem is that I have a 1n4002 diode in a package called D1F from Flint electronics. Looking through the catalogue shows that DO214 is only a gnats kneecap different. This is given a placement courtyard of 8x16 (8mm x 4mm) which leaves 0.6mm at the ends & 0.8mm along the length. This package is higher than the resistors, so how do I work out the placement courtyard distance? I know that there can be a difference in spacing depending upon the height to allow for correct heat transfer, but how do I work it out? I also have similar problems with SMT relays, as I need to know how far away I need to place smaller components, based upon its height. Next problem is Soldermask clearance. I'm aware that solder mask is generally to be 0.2mm (0.008") larger than the pads. Does this mean that for a square/rectangular pad, would this be 0.1mm (0.004") each side of the pad? I know that there has to be some allowance for misalignment of the board/mask, however I think that I have previously had this 0.008" bigger each side, giving me little room for running tracks near the SMT pads. However now that I need to make a new SMT board, the size of a box of matches with loads of components on I can see that I have to reduce my component dimensions accordingly. Many Thanks - Matthew Lamkin.