Ken, There are manufacturability reasons for both dimensions. It is not uncommon for small caps and resistors to pull to the center of one of their respective pads. This can result in an open if the component pulls far enough away from the opposing pad; and often results in tombstoning if the pull gets just enough torque to lift the lead away from the solder on the opposing pad. Moving the two pads closer together is the safest and easiest way to prevent tombstoning. This is because when one side of the cap or resistor is pulled towards a pad due to different wetting speeds, the opposite end of the component will still remain squarely on the opposing pad, allowing the small amount of surface tension on the slower wetting termination to resist the torque of surface tension on the pulled side. To prevent tombstoning, the centerline of the pads should match the centerline of the component termination. It is also not uncommon for solder paste to get squeezed underneath a component when it is placed on the board. When this happens, it often occurs that the squeezed solderpaste does not coalesce into the molten solder comprising the joint. Instead, the squeezed solderpaste emerges from underneath as a free-floating solder ball, sometimes called a squeeze-ball. One common method of preventing this is to use a home plate design on the solder-paste stencil. The home plate design is intended to reduce the amount of solder-paste that can get squeezed underneath the component. An alternate method of reducing the amount of solder paste underneath the component is to move the two pads farther apart so the ends of the component just touch the solder paste. As you can see, the reason behind the two different dimensions depends on the point of view a person is coming from. My personal point of view is to put the pads close together, and put the solder-paste stencil openings farther apart (the stencil guys hate me), solving both problems. Another reason behind pad farther apart is for wave soldering as you implied. With wave soldering, it is often assumed the component will be glued first; thus preventing it from pulling to one side on another. Having the pad reach under the component serves no purpose, so the pads can be farther apart, allowing a larger surface to catch solder from the wave. I hope this helps Thanks Ryan Grant Advanced Technology Engineer MCMS (208) 898-1145 [log in to unmask] > -----Original Message----- > From: Ken Patel [SMTP:[log in to unmask]] > Sent: Friday, November 17, 2000 1:03 PM > To: [log in to unmask] > Subject: [TN] Designer/Assembler: Need help on 0603 spacing problem. > > Designer/Assembler, > I was surprised to see 35 mil spacing between pads of 0603. Looking the > IPC-SM-782 that number is 24 mils. Why such as difference? Does any user > aware of requiring 35 mils spacing for 603 cap using any standard foot > print > library? What is the spacing being used for reflow and wave for 0603 caps. > Can Assembly house shall catch this kind of problem across the board > during > prototype? And how difficult is that job or is it almost impossible, I > mean > using any program as later on design engineer said that they never > complained before and why now! > I still have to contact my layout house yet on his foot print selection. > re, > ken patel > > -------------------------------------------------------------------------- > ------- > Technet Mail List provided as a free service by IPC using LISTSERV 1.8d > To unsubscribe, send a message to [log in to unmask] with following text in > the BODY (NOT the subject field): SIGNOFF Technet > Search previous postings at: www.ipc.org > On-Line Resources & Databases > > E-mail Archives > Please visit IPC web site (http://www.ipc.org/html/forum.htm) for > additional > information, or contact Keach Sasamori at [log in to unmask] or 847-509-9700 > ext.5315 > -------------------------------------------------------------------------- > ------- --------------------------------------------------------------------------------- Technet Mail List provided as a free service by IPC using LISTSERV 1.8d To unsubscribe, send a message to [log in to unmask] with following text in the BODY (NOT the subject field): SIGNOFF Technet Search previous postings at: www.ipc.org > On-Line Resources & Databases > E-mail Archives Please visit IPC web site (http://www.ipc.org/html/forum.htm) for additional information, or contact Keach Sasamori at [log in to unmask] or 847-509-9700 ext.5315 ---------------------------------------------------------------------------------