Whether or not we use a via in pad is determined by what is connecting to the pad. For instance... Mostly what we design are load boards or probe cards for testing wafers. If the interface requires that the pogo pad have a centered hole then the pad is made large enough to take the abuse. Most of the time we offset the via from the center of the pad because this is how the interface requires it. When we design for SMDs we always offset the pad from the via to make the solder connection possible. The only reliability issue we have had with "via in pad" is if the pad was too small and tended to lift if rework was required. The only suggestion I have is to make sure that the application is well understood and that if the via is going to be the solder point make sure that the via annular ring is at least 2.5 times the diameter of the drill size (not always possible!). We have found that this decreases problems in the field and increases reliability. If the via is not a solder point then the annular ring can be as small as required to anchor the via properly. Gary At 07:24 PM 2/19/98 -0600, you wrote: >All, > I have been watching this discussion with interest and unless I missed some posts have found only 2 answers to the original question. Can I assume that not many companies are using "via in pad"? Is there a reliability issue with this design practice? Any responses are welcome. > >Thanks, > >Geoff Kishpaugh >Motorola Inc. >1900 Winchester Rd, IL-46 >Libertyville, IL, 60048 >Phone: 847-523-0067 >Fax: 847-523-0078 >email: [log in to unmask] > >------------------------------------------ > >Hi Leonard, > >We typically see blind vias up to .013 drilled size in .030 x .060 pads. You should actually put >the via towards the end of the pads, rather than the center. Board thickness does make a >difference and the ratio of board thickness to drilled hole size (aspect ratio) should not >exceed 10:1 for blind or thru-vias drilled with conventional equipment and 1:1 for controlled >depth laser drilling, where the drilled via size can go down to .006 inches. The aspect ratios >mentioned are only for the "blind" portion being drilled and not the thickness of the entire >board. > >You may contact me offline at 817-481-7281 should you have additional questions or wish to >discuss this further. > >Regards, > >Keith Larson >Circuit Technology Inc. > >-----Clip------ > >Leonard; >The only large company to use via in land on a regular >basis is Lucent, they have the process down pat. >The trick is to figure how much solder you going >to lose to the hole. >It real helps on high density boards. >Lou >-----Clip------ > >Leonard Toohey wrote: > >> What is the state of the industry regarding putting >> vias in the center of SMT discrete device pads? >> >> I am mainly wanting to know about 0603, 0805 and 1206 devices. >> Is board thickness a factor? >> What about via hole size? >> >> Thanks, >> >> Leonard Toohey >> [log in to unmask] >> 12303 Technology Blvd. >> Austin, TX 78727 >> Ph(512) 257-5423 >> Fx(512) 249-7236 >> http://www.netspeed.com > >################################################################ >TechNet E-Mail Forum provided as a free service by IPC using LISTSERV 1.8c >################################################################ >To subscribe/unsubscribe, send a message to [log in to unmask] with following text in the body: >To subscribe: SUBSCRIBE TechNet < >To unsubscribe: SIGNOFF TechNet >################################################################ >Please visit IPC web site (http://jefry.ipc.org/forum.htm) for additional information. >For the technical support contact Dmitriy Sklyar at [log in to unmask] or 847-509-9700 ext.311 >################################################################ > > > ================================================== 0000,0000,ffffGary Griffin Engineering Manager Phone (408) 501-7156 Fax (408) 437-1976 Pager 1-800-759-7243 Pin: 145-1886 Alpha pager email griffin_p or [log in to unmask] SABER group Interface Products ################################################################ TechNet E-Mail Forum provided as a free service by IPC using LISTSERV 1.8c ################################################################ To subscribe/unsubscribe, send a message to [log in to unmask] with following text in the body: To subscribe: SUBSCRIBE TechNet To unsubscribe: SIGNOFF TechNet ################################################################ Please visit IPC web site (http://jefry.ipc.org/forum.htm) for additional information. For the technical support contact Dmitriy Sklyar at [log in to unmask] or 847-509-9700 ext.311 ################################################################