Good for Production HTM Card Bare PCB Description --------------------------------- Rev. 24-Apr-2018 This note is a description of the bare HTM printed circuit board. HTM Bare Circuit Board Specifications: Size: The overall outer dimensions of the HTM PCB are 280.0 mm in X by 322.25 mm in Y. The card is approximately rectangular with a notch in its front edge. Please see the gerber file: artwork_9_mechanical_drawing Layers: 10 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. The Isola FR408HR material would work well. Controlled Impedance: The HTM circuit board requires 100 Ohm controlled impedance differential pairs. 100 Ohm differential trace pairs are used on layers: 1, 3, 8, 10 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 Power Fills 6 Power Fills 7 Ground Plane Lower Type 8 Signal Traces 100 Ohm Diff 9 Ground Plane Lower Type 10 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: 5 and 6 Thickness: The nominal thickness should be in the range 2.2 mm to 2.6 mm. The overall thickness must not be over 2.6 mm. Stackup: Please suggest a stackup to satisfy the design details presented in this document. Ground Planes: There are 2 different copper patterns used for the 4 ground planes in the HTM card. The Upper ground plane pattern is used on pcb layers: 2, 4 The Lower ground plane pattern is used on pcb layers: 9, 10 Both ground plane gerber files are supplied as negative gerber data. 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: The Top side of 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 to plug these vias. A gerber file is provided that indicates the location of all of the vias that need to be plugged from the Top side of the card. This gerber file contains a "flash" for each via that needs to be plugged. 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 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 4 back-drill drill files are provided. - From the bottom this card requires 2 back-drill depths for each of 2 hole sizes. - 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 pin holes. The filename format for the 6 back-drill files is: bk_drill - nominal_original_hole_diameter - drill_from_Top_or_Bottom - layers_that_MUST_REMAIN_CONNECTED The names of the 4 back-drill files are: bk_drill_0.25_from_Bottom_keep_L3_to_L1 bk_drill_0.25_from_Bottom_keep_L8_to_L1 bk_drill_0.46_from_Bottom_keep_L6_to_L1 bk_drill_0.46_from_Bottom_keep_L8_to_L1 Solder Mask and Silkscreen Colors: Standard Green solder mask and White silkscreen are fine with us for this card. Solder Mask Openings: As designed the Solder Mask openings are 0.05 mm larger on all edges than the pads that these openings expose. Through Hole Drill Information: The HTM Card requires both plated and un-plated drill holes. All drill 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 16 2 0.30 699 3 0.46 160 4 0.60 218 5 0.89 82 6 1.00 14 8 1.10 22 10 1.60 24 11 2.00 4 12 2.20 2 14 2.70 6 16 3.00 7 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 Connector J23 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 HTM Card 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 J13, J14 Solder pin on connector J12 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 the component "Power_12V" and the 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 TRANS_MP and REC_MP 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 & bottom handle These holes are for metric M2.5 screws. 3.00 mm Mounting Screw Holes for 4-40 screws. Un-Plated Through Holes: Nominal Drill Hole Number Diameter Count ------ -------- ----- 7 1.00 8 9 1.50 2 13 2.30 9 15 2.70 1 17 3.00 8 Details about the Un-Plated Through Holes Nominal Hole Diameter Usage Description and Tolerance -------- ---------------------------------------------- 1.00 mm Alignment Pin Holes for Connectors: J1 J2 J3 and J11 Molex 87332-4020 connector alignment pin. Molex hole specification: 1.00 mm +- 0.05 mm Samtec ASP-122953-01 Spec. 40 mils 1.50 mm Device ID Pin for TRANS_MP and REC_MP Avago hole specification: 1.50 mm 2.30 mm Mounting Hole for Single LED Light-Pipes Manufactures specification: 2.30 mm diameter 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 on this care are 0.14 mm wide The minimum copper to copper clearance is 0.16 mm. 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: This is a list of the Gerber files that are provided for the manufacture of the bare HTM circuit boards. All 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_fill_L5 artwork_4_trace_fill_L6 artwork_5_trace_L8 artwork_6_trace_L10_bot artwork_7_gnd_plane_Ls_2_4 negative data artwork_8_gnd_plane_Ls_7_9 negative data artwork_9_mechanical_drawing artwork_10_silkscreen_top artwork_11_silkscreen_bot artwork_12_solder_mask_top artwork_13_solder_mask_bot artwork_14_paste_stencil_top artwork_15_paste_stencil_bot artwork_16_plugs_top 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 HTM Cards. Technical Contact: Dan Edmunds Phone: (517) 884-5521 Email: edmunds@pa.msu.edu