Date: Sun Oct 23 23:37:56 2016 Subject: RE: Hub PCB Review & Discussion Hi All: In preparation for our call, I have answered as many questions as possible below. Please review and we can discuss during the call. Thanks, Gus Trakas, P.Eng. | Field Applications Engineer Viasystems Toronto, Inc., a member of TTM Technologies Group Small Routing and BGA Escape Vias: ---------------------------------- Recommended Land Diameter and Hole Diameter for: - Smallest rational practical to manufacture size via that I may use for the High-Speed 100 Ohm differential signals for trace routing and to escape from within the BGA ? Land Dia and Hole Dia -- Using a PCB thickness of 3.05mm, the preferred minimum DRILLED hole size is 0.25mm and pad size of 0.5mm for Class 2 compliance. - Next to smallest size that I may use for normal tight CMOS digital signal routing ? Land Dia and Hole Dia -- Next size up would be 0.3mm DRILL and 0.55mm pad. - This pcb is going to be about 3.0 mm thick. -- Correct. - How to specify the Hole Diameter for these small routing vias: Drill Dia or Finished Dia ? -- Preferred is to specify finished diameter similar to other holes, but for vias have the hole size tolerance as +0/-. - Relieve the Solder Mask or not ? aka Tent or not ? -- Preferred is to not tent to prevent chemical entrapment as stated below. Currently the Solder Mask is relieved on all via holes. My understanding is that I should un-Tent all vias to minimize the problems of chemical entrapment. -- Correct. How far back from the drill hole diameter must I relieve the Solder Mask to un-Tent the via ? -- Preferred encroached soldermask opening is drill size +0.15mm. For the larger vias that are actually component pins, for example for the press-in connectors, I will specify the Finished Diameter and clearly these vias are not tented. -- OK. Back Drilling the High-Speed Vias: ---------------------------------- The design has *about* 720 vias that need to be Back-Drilled so that they can handle the high-speed differential signals. These vias always connect from an internal signal layer to either the top or bottom surface layer. Some of these high-speed differential signal vias are out in the routing area of the card and some are under the FPGA in the escape from its BGA pattern. What design rules should I use for back-drilling ? -- See below. How much bigger in Diameter is the Back-Drill than the Via Hole ? -- Typical oversize for a back drill is 0.2mm larger than the DRILL (not finished) size. What do I need to say in the Hub PCB Description to rationally specify these back-drills ? -- Best is to have the holes requiring back drill as a separate drill size, which can then be linked to the fab drawing note requirements. For example, for 0.25mm holes, the holes requiring back drill can be 0.251mm. I'm setup to provide a separate drill file for each type of back-drill, e.g. a drill file defined as the XY locations to back-drill from the Top side cutting through L16 but do not break the connections on L18. Is this the correct way to specify back-drills ? -- OK. This will work. Plugging Holes to prevent Solder Wicking into them during assembly re-flow: ---------------------------------------- - The Hub PCB design has may QFN components (on both sides) with a center Thermal/Ground pad that contains an array of vias that tie to the ground planes. - The design also has two linear regulators with large pads that include an array of vias to carry away the heat from these parts. - The design also has some routing vias that are quite close to normal SMD component pads. Some are close enough that there is only 0.1 or 0.2 mm of Solder Mask barricade between the Solder Mask relief for the component pad and the relief for the un-Tented routing via. I assume that in all 3 of these cases these holes need to be plugged to prevent solder wicking into the holes during reflow. I'm ready to provide Gerber files with just an appropriate diameter flash at the X,Y coordinate of all of these holes. I would provide a separate file for plugs needed on the Top side and for the plugs needed on the Bottom side. Is this the correct way to handle this whole problem of solder wicking into holes in or very close to pads ? -- Yes. Providing separate files for holes requiring bottom or top plugs is perfect. The outline of the Hub PCB includes some internal corners: ---------------------------------------------------------- How small of a routing tool diameter can be used on these internal corners ? Front panel components must fit into these internal corners so I must specify the width of the notch in the PCB front edge to accommodate the routing tool diameter. -- Our smallest router bit that can be used for internal corners is 0.8mm. In cases where a square corner is required, a drill hit can be added to the corner. On Fri, 21 Oct 2016, George Cherrick wrote: Meeting Tue, Oct 25, 2016 9:00 AM - 9:45 AM Eastern Standard Time Please join my meeting from your computer,... https://global.gotomeeting.com/join/633342045 You can also dial in using your phone. United States +1 (646) 749-3122 Access Code: 633-342-045