Interesting.... Ken Patel asked: Is there any problem spelling out "ALL GROUND/POWER PLANE CONNECTIONS SHOULD HAVE THERMAL RELIEF " on my fab drawings. Please provide me pros and cons before I make a call. Your help is greatly appreciated. Raymond Klein replied: >Ken, > >I usually take the other approach and specify thermal relief ONLY ON PIN >THROUGH PARTS. (No thermal relief is needed on press fit parts). Vias to >power and ground planes do not usually need thermal relief and it makes for >a much more continuous plane which give better electrical characteristics >and are easier for the PWB designer to route (vias can be closer together). >I've also had dense designs which would have had large gaps in the power >and ground planes if I'd used thermal relief on the hundreds of vias that >connected to these planes. > >Problems with lack of thermal reliefs may occur if a very short and wide >(>.025 in) trace is used to connect a SMT part to a via to a gnd/pwr plane. > >Ray Klein At Interphase, our boards are typically fairly dense 6 layer designs with SMT parts on both sides. 98% of all active parts are SMT packages, which have ground or power connection to internal layers by way of 0.010" PTH's. These holes have a cartwheel pattern thermal relief with four spokes. The thermal relief pads are shown on the Gerber files as "flashed" patterns. When examining the internal plane film layers, the thermal relief pads are scattered in the hundreds. The dominant majority of these connections go up through the hole, and then to an 0.030" external pad, connecting with a 0.010" width trace to an SMT rectangular pad which is 0.015" or 0.010" wide. My guess is that this design approach is a hangover from the requirements of the wave solder process days when it was necessary to get good wetting up the hole and to the topside pads. I'm not sure that there is any reason to do this on modern designs as I describe, and tend to believe Ken's approach would work, but since this is NOT what we do, can't say that there wouldn't be thermal variation in reflow on the power leads of a QFP, for instance. The electrical impedance of the power connection would likely be better (lower inductance) if the plated hole connects to the plane around the entire circumference. If there are others who use the "no thermal relief" internal connections extensively, I'd sure like to hear how it has affected (if it has) the profile and delta T, and whether it has caused any coincidental issues. regards, Jerry Cupples Interphase Corporation Dallas, TX USA http://www.iphase.com/ ############################################################## TechNet Mail List 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 <your full name> To unsubscribe: SIGNOFF TECHNET ############################################################## Please visit IPC web site (http://www.ipc.org/html/forum.htm) for additional information. For the technical support contact Dmitriy Sklyar at [log in to unmask] or 847-509-9700 ext.311 ##############################################################