Mike, My intent in doing this is to allow me to maintain .006 trace widths, .006 spacing ( .005/.005 finished) in my design without reducing my pad size to a degree that it makes it difficult to maintain annular ring. The problem connector has .040 pads on a .050 pitch. Here're the pad/hole requirements: A) .013-.019 finished holes. B) 2 x .002 annular ring internal C) 2 x .002 etchback D) .012 mfg. allowance So that tells me I need a minimum pad of .039. Without reducing my requirements or increasing the manufacturing difficulty it seems to me I gain a lot by removing unused pads. Routing a 6 mil trace down a 10 mil slot gives me 2 mils per side of clearance. By removing the unused pads my trace is now (worst case) 4 mils from the edge of the barrel, and nominally my 6 mil trace is 25 mils from the center of an 18-20 mil barrel. That sounds like a big improvement to me, or am I missing something? -Mike Hiteshew > ---------- > From: Mcmaster, Michael[SMTP:[log in to unmask]] > Reply To: TechNet E-Mail Forum.;Mcmaster, Michael > Sent: Wednesday, January 10, 2001 2:05 PM > To: [log in to unmask] > Subject: Re: [TN] Unused Inner Layer Pads: Remove or Not? > > I'm probably saying the same thing as George. The critical part of your > question is that your asking if you can remove the pads to increase wiring > density during layout. The answer is absolutely not. Remember what the > pad > is for, to make an interconnect to the drilled hole. The reason it's > larger > than the hole is to make sure the hole is still in the pad when all the > manufacturing tolerances are taken into account. The non-functional pad > means there's no interconnect on that hole on that layer, but the drilled > hole will still be there. The non-functional pads are friendly reminders > to > keep traces out of that area. > > If you need more room, you need to ask two question of your board > fabricator > and one of yourself. For the fabricator, the first question is "how much > larger than the drilled hole must a pad be and still capture the hole"? > The > second is "what's the minimum pad to trace space they can etch?" For you, > "from a reliability viewpoint, what's the minimum conductor-to-conductor > spacing I want in the finished board?" Take the larger of the answers to > the last two questions and add it half the answer to the first. If you a > run a trace closer to a hole than that, your fabricator will be throwing > them away for shorts at electrical test or you'll have boards which don't > meet your reliability expectations. > > For example, your fabricator says I need a pad 0.010" larger than the > drilled hole and I can etch a 0.004" space. You follow IPC and want a > minimum 0.0035" spacing. You should put in the desired pad size (while > your > at it, if you're cutting it this close, you might as well find out the > exact > drill bit diameter they will use). Then rout traces with a minimum 0.004" > spacing. > --------------------------------------------------------------------------------- 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 To temporarily halt delivery of Technet send the following message: SET Technet NOMAIL 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 ---------------------------------------------------------------------------------