Hub Module Bare PCB Description ----------------------------------- Rev. 15-Feb-2017 Good for Production This note is a description of the bare Hub printed circuit board. We are asking the assembly vendor to obtain the bare Hub Module PCBs to insure that they are comfortable with the quality of the PCB and have included in it all rails and tooling holes that their assembly process may require. For this Hub project we are comfortable paying for a high quality pcb with optimum surface finish to insure that there are no assembly problems. Hub Bare Circuit Board Specifications: Size: The overall outer dimensions of the Hub PCB are 315.0 mm in X by 322.25 mm in Y. The card is approximately rectangular with a notch in its front edge and a bump out on its backplane edge. Please see the dimensioned Gerber plot for details, artwork_16_mechanical_drawing. Layers: 22 Most of the card is alternating trace and ground plane layers. Material: The laminate dielectric material must be appropriate for carrying high frequency 10 GHz digital signals. We assume that this will be a high quality high frequency low dielectric loss material that the bare pcb vendor is comfortable and experienced working with. Controlled Impedance: The Hub circuit board requires 100 Ohm controlled impedance differential pairs. 100 Ohm differential trace pairs are used on layers: 1, 3, 5, 7, 9, 14, 16, 18, 20, 22. In the gerber files all 100 Ohm differential trace pairs on these layers were drawn with a trace width of 0.14 mm and a center to center spacing of 0.4 mm. All 0.14 mm width traces on these layers should be adjusted to have a 100 Ohm differential controlled impedance. In all of the gerber files the 0.14 mm trace width is used exclusively for these 100 Ohm differential traces. Layer Summary: PCB Controlled Layer Layer Type Function Impedance ------- --------------------- ------------ 1 Signal Traces 100 Ohm Diff 2 Ground Plane Upper Type 3 Signal Traces 100 Ohm Diff 4 Ground Plane Upper Type 5 Signal Traces 100 Ohm Diff 6 Ground Plane Upper Type 7 Signal Traces 100 Ohm Diff 8 Ground Plane Middle Type 9 Power Fills and Signals 100 Ohm Diff 10 Ground Plane Middle Type 11 Power Fills 12 Power Fills 13 Ground Plane Middle Type 14 Power Fills and Signals 100 Ohm Diff 15 Ground Plane Middle Type 16 Signal Traces 100 Ohm Diff 17 Ground Plane Lower Type 18 Signal Traces 100 Ohm Diff 19 Ground Plane Lower Type 20 Signal Traces 100 Ohm Diff 21 Ground Plane Lower Type 22 Signal Traces 100 Ohm Diff Copper Weight: 1/2 oz minimum on all Signal and Ground Plane layers. 1 oz minimum on all layers with Power Fills i.e. 1 oz on Layers: 9, 11, 12, 14 Thickness: The nominal thickness will be in the range of 3.0 mm. Stackup: Please use the stackup that was prepared by Gus Trakas on about 10-Sept-2016 Job Name: Hub PCB Stackup, Customer: Debron Electronics, Part Num: Hub PCB Stackup Ground Planes: There are 3 different copper patterns used for the 10 ground planes in the Hub card. The Upper ground plane pattern is used on pcb layers: 2, 4, 6. The Middle ground plane pattern is used on pcb layers: 8, 10, 13, 15. The Lower ground plane pattern is used on pcb layers: 17, 19, 21. All three ground planes are supplied as negative gerber data. Mill Thickness from the Back side: 4.0 mm wide strips along the top edge and the bottom edge must be milled from the BACK side to a thickness of 2.0 mm to allow insertion into card guides. The Back side silkscreen plot labels the area to be milled down. Via "Tenting": Currently the Solder Mask has been relieved from all of the via drill holes, i.e there is no Solder Mask "tenting" of any of the vias or component pin holes. Plugged Vias: This board includes a number of components that have a center Exposed Pad that must be soldered to a grounded Thermal Land for cooling. These Thermal Lands are connected to the internal ground planes by an array of vias to conduct heat away from these components. To prevent solder from being sucked into these vias during the assembly process we need these vias to be plugged. There are some additional "routing vias" that needed to be placed very close to SMD component pads and thus risked the same solder wicking problem. Separate gerber files have been provided that indicate the location of all of the vias that need to be plugged from the Top and from the Bottom. These gerber files contain a "flash" for each via that needs to be plugged. I made these flashes 0.02 mm smaller than the nominal diameter of the drill hole for the via. Note that some of these vias risk sucking in solder from both the top side and bottom side of the card and thus need to be plugged on both sides. These vias appear in both of the via plugging gerber files. Thieving Fill Pattern: If the bare board vendor wants to include a thieving fill pattern in any sections of this card we are happy to discuss that requirement. I assume that the thieving pattern will be kept back 2.5 mm minimum from any trace routing. Back-Drill of Via and Connector Pin Holes: This card includes a large number of layer to layer transitions for its high-speed 100 Ohm differential traces. We need the vias and the connector pin holes that make these layer transitions to be back-drilled. All high-speed vias that will require back-drilling are made with a nominal 0.25 mm drill diameter. All of the connector pins that will require back-drilling are made with a nominal 0.46 mm drill. Thus there are only two hole diameters that will require back-drilling. My understanding is that the diameter of the back-drill will be 0.20 mm over the size of the drill that was used to make the original hole. In total 11 back-drill drill files have been provided. - There are separate files for back-drill from the Top side and from the Bottom side of the card. - There are separate files for each of the required back-drill Depths. The file names indicate the layers that Must Remain Electrically Connected. - There are separate files for back-drilling the 0.25 mm vias and the 0.46 mm connector pins. The filename format for the 11 back-drill files is: bk_drill - nominal_hole_diameter - drill_from_Top_or_Bottom - layers_that_Must_Remain_Connected Solder Mask and Silkscreen Colors: Standard Green solder mask and White silkscreen are fine with us for this card. Solder Mask Minimum Width: The recommended layout for the array of 74 QFN-16 packages along the back edge of the card has a large center pad with little clearance to the surrounding perimeter pin pads. This results in a Solder Mask line width of only about 0.90 mm separating the center pad from the surrounding perimeter pin pads. As designed the Solder Mask openings are 0.05 mm larger on all edges than the pads that these openings expose. If the 0.90 mm Solder Mask line width is too narrow please let me know and I could trade off some of the 0.05 mm Solder Mask separation form the pad copper for a larger Solder Mark line width between the center and perimeter pads. Through Hole Drill Information: The Hub Module requires both plated and un-plated drill holes. All holes go the whole way through the card. Hole Diameter is in mm. Plated Through Holes: Nominal Drill Hole Number Diameter Count ------ -------- ----- 1 0.25 1114 2 0.30 5986 3 0.46 1189 4 0.60 618 5 0.89 100 6 1.00 14 8 1.10 52 11 1.60 36 12 2.00 4 13 2.20 2 16 2.70 3 18 3.00 4 20 3.20 3 Details about the Plated Through Holes Nominal Hole Diameter Usage Description and Tolerance -------- -------------------------------------------------- 0.25 mm Smallest vias for the high-speed signals These vias use a 0.52 mm pad diameter. These vias may close during plating. 0.30 mm Normal signal vias & low current power/ground vias These vias use a 0.60 mm or 0.65 mm pad diameter. These vias may close during plating. 0.46 mm Press-In pins on Backplane Connectors J20 : J24 Medium size power/ground vias and via arrays The 0.46 mm hole diameter vias must be designed to work with the Press-In pins of the TE Connectivity Part Number 2065657-1 connectors. Please see page 9 of the TE Connectivity Application Specification 114-13059 a copy of which is available in the same web directory as the rest of the Hub Module bare board manufacturing files. These vias are for HM-Zd PLUS type connector press-in pins. 0.60 mm Large Vias, with 1.10 mm Pad diameter, the hole may reduce in diameter as required during plating. 0.89 mm Press-In Pins on RJ45 connector RJ1, RJ2, RJ3 Solder pin on connector J2 The RJ45 Press-In pins are on TE Connectivity Part Number 1888653-4 connectors. TE Conn specification for finished hole diameter is: 0.89 mm +- 0.06 mm. 1.00 mm Press-In Pins on Backplane Connector P10 These Press-In pins are the small pins on TE Connectivity Part Number 1766500-1 connector. The TE Connectivity specification for finished hole diameter is: 1.00 mm +0.09 mm -0.06 mm. 1.10 mm Largest Vias, with 3.00 mm Pad diameter, the hole may reduce in diameter as required during plating. 1.60 mm Medium current solder in pins on Power Modules "Power Entry" and Power_12V" Press-In Pins on Backplane Connector P10 The Press-In pins are the large pins on TE Connectivity Part Number 1766500-1 connector. The TE Connectivity specification for finished hole diameter is: 1.60 mm +0.09 mm -0.06 mm. 2.00 mm Mounting Screw Holes for TRN_MP1 and REC_MP2 These holes are for metric M1.6 screws. 2.20 mm High current solder in pins on "Power_12V" module These holes are for 1.57 mm diameter high current pins. 2.70 mm Mounting Screw Holes for: K1, K2, & bottom handle These holes are for metric M2.5 screws. 3.00 mm Mounting Screw Holes for the Heat-Sink These holes are for 4-40 screws. 3.20 mm Mounting Screw Holes for the ROD Mezzanine These holes are for metric M3 screws. Un-Plated Through Holes: Nominal Drill Hole Number Diameter Count ------ -------- ----- 7 1.00 2 9 1.40 1 10 1.50 15 14 2.30 6 15 2.40 8 17 2.70 1 19 3.00 4 Details about the Un-Plated Through Holes Nominal Hole Diameter Usage Description and Tolerance -------- ---------------------------------------------- 1.00 mm Alignment Pin Holes for Connector J3 Molex 87332-4020 connector alignment pin. Molex hole specification: 1.00 mm +- 0.05 mm 1.40 mm Alignment Pin Upper for Socket "IPMC" Molex 87782-3003 Upper alignment pin. Molex hole specification: 1.40 mm +- 0.05 mm 1.50 mm Alignment Pin Middle for Socket "IPMC" Device ID Pin for TRN_MP1 and REC_MP1 Mounting Hole for Dual-Quad LED Light-Pipes Molex 87782-3003 Middle alignment pin. Molex hole specification: 1.50 mm +- 0.05 mm 2.30 mm Mounting Hole for Single LED Light-Pipes Manufactures specification: 2.30 mm diameter 2.40 mm Mounting Holes for Backplane MPO_1 : MPO_4 These holes are for 2-56 screws. 2.70 mm * Mounting Hole for Upper Handle This hole is for metric M2.5 screws. 3.00 mm * Mounting Holes for the Front Brackets These holes are for 4-40 screws. * These holes have surface pads but the hole tunnel is not plated. Traces and Clearances: The narrowest traces are 0.12 mm which is used only in the dual trace routing under the 400 pin MegArray connectors. In the 1 mm pitch BGA break-out area there are 0.13 mm wide traces. The narrowest traces in all other areas of the card is 0.14 mm wide The minimum copper to copper clearance is 0.12 mm which is used only in the dual track routing under the MegArray connectors. All other copper to copper clearances are larger. Surface Finish: The surface finish should be selected to allow optimum SMD component assembly. I assume that this will be gold finish of some type. This decision should be made in consultation with the assembly vendor. Bare card electrical test: All cards 100% electrically tested. Currently I can not provide an IPC 356 net list. The net list will need to be extracted from the gerber data. Gerber Files: Gerber data is in mm. Each coordinate is 6 digits long with 3 digits after the decimal point. Gerber File Names: artwork_1_trace_L1_top artwork_2_trace_L3 artwork_3_trace_L5 artwork_4_trace_L7 artwork_5_trace_fill_L9 artwork_6_trace_fill_L11 artwork_7_trace_fill_L12 artwork_8_trace_fill_L14 artwork_9_trace_L16 artwork_10_trace_L18 artwork_11_trace_L20 artwork_12_trace_L22_bot artwork_13_gnd_plane_Ls_2_4_6 negative data artwork_14_gnd_plane_Ls_8_10_13_15 negative data artwork_15_gnd_plane_Ls_17_19_21 negative data artwork_16_mechanical_drawing artwork_17_silkscreen_top artwork_18_silkscreen_bot artwork_19_solder_mask_top artwork_20_solder_mask_bot artwork_21_paste_stencil_top artwork_22_paste_stencil_bot artwork_23_plugs_top artwork_24_plugs_bottom Please speak up if you see anything that does not look right to you in this design. I'm happy to provide any other information that I can to facilitate the manufacture of these circuit boards. Thank you for your help making the Hub Modules. Technical Contact: Dan Edmunds Phone: (517) 884-5521 Email: edmunds@pa.msu.edu FAX: (517) 355-6661