ROCK Design Details ---------------------------- Original Rev. 23-MAY-1997 Most Recent Rev. 14-SEPT-1997 Cosmetic Details: ----------------- The trace that connects TCM-2620 Pin #45, AutoBias, from its via to the adjacent GND via is cosmetic copper on layer Signal_1. ? The slice in the Gnd Plane is a cosmetic line placed on layer POWER_3. ? Board_Rock Geometry ------------------- 3 Routing Layers Planes Net Names (in order of definition): THERM_GND GROUND '+5V_ANL' '+5V_DIG' Mentor Layer Usage ------------------ Physical Logical Function -------- -------------- -------------------- 1 Signal_1, Pad_1 Component Side: Pads and connections 2 Power_1 Therm_Gnd 3 Power_2 Ground 4 Power_3 +5V_ANL 5 Power_4 +5V_DIG 6 Signal_2 All connections 9 Signal_3, Pad_1 Not actually used DAM_1 "Target Area Lable" for Board Outline DAM_2 "Target Area Lable" for Component Side DAM_3 "Target Area Lable" for Solder Side GLUE_MASK_1 Drawing of the rectangular cut out GLUE_MASK_2 Component Side Therm_Gnd relief for critical analog components What the Rock Board itself should look like: Silk Screen lettering 1. Therm_Gnd Plane with embedded pads and stub traces to the pads 2. Power Plane split +5V_Anl and +5V_Dig 3. Ground Plane 4. Signal Traces 5. Ground Plane 6. Therm_Gnd Plane with embedded THD pads Note that there is no Solder Mask layer on either side. Note that the Therm_Gnd Plane on the component side may be removed from the areas of sensitive analog stuff. Note that the Power Plane may be removed from the areas of sensitive analog stuff. Artwork Order ------------- Artwork Brd Order Layr Number Layers Special Stuff ---- ------ -------------------------------- ---------------------------- Test 1 Board_Outline, Target, Dam_1 Comp 2 Signal_1, Pad_2, Power_1, Target, Dam_2, Glue_Mask_2 --- 2 3 Power_3, Power_4, Target Thermal_Relief, Clear 50 mil 3 4 Power_2, Target Thermal_Relief, Clear 50 mil 4 5 Signal_2, Target 5 6 Power_2, Target Thermal_Relief, Clear 50 mil Solder 7 Signal_3, Pad_2, Power_1, Target, Dam_3 Silk 8 Silkscreen_1,Target Artwork Order Number 1 is the Test Plot of the Board Outline. It uses the Dam_1 layer to hold the "Label" for this plot that goes in the target text area. This label is kept on a private layer so that it will not show when the Board Outline is implicitly turn on again during the generation of the planes to generate the plane edge relief. Artwork Order Number 3 is the split +5V_Anl +5V_Dig planes Artwork Order Numbers 4 and 6 are identical GND Planes. One must hand edit the "target area label" between the plots of these two copies of the GND Plane. To get "Target Area Labels" to appear on the Component Side and Solder Side plots I needed to put the labels on their own level. I expect that this is because Signal_1 and Signal_3 are embedded in the THERM_GND plane. Gerber File vs Baord Layer File Name Contents Location in Board Stack -------------- ---------------------------- --------------------------- ArtWork_01.Grb Test plot of board outline ArtWork_02.Grb Comp side Traces Pads & Plane Component Side ArtWork_03.Grb Power Plane, +5V Anl & Dig Next to Component Side ArtWork_04.Grb Ground Plane #1 Next to Next to Comp Side ArtWork_05.Grb Signal Traces Next to Next to Solder Side ArtWork_06.Grb Ground Plane #2 Next to Solder Side ArtWork_07.Grb Solder side Pads & Plane Solder Side ArtWork_08.Grb Component side Silkscreen On the Component Side Apertures Used (after editing Art_2 and Art_7) ----------------------------------------------- File Name Apertures Used D-Code -------------- ------------------------------------------------------- ArtWork_01.Grb 11 ArtWork_02.Grb 11, 12, 18, 19, 71 ArtWork_03.Grb 10, 11, 16, 17, 18, 19, 70, 71, 20 ArtWork_04.Grb 10, 11, 16, 17, 18, 19, 70, 71, 20 ArtWork_05.Grb 10, 11, 12, 13, 14, 15 ArtWork_06.Grb 10, 11, 16, 17, 18, 19, 70, 71, 20 ArtWork_07.Grb 11, 16, 17, 18, 19 ArtWork_08.Grb 11 Note that on files Artwork_02 (the Component side) and Artwork_07 (the Solder side) the definition of apertures D16 and D18 needs to be a donut, (i.e. to produce a pad surrounded by an air gap) where as on all other layers D16 and D18 are solid circular flashes. Note that on files Artwork_02 (the Component side) and Artwork_07 (the Solder side) one must hand remove all of the keep away flashes for the 4-40 drill holes. The 4-40 drill holes are buried in the Component and Solder side Thermal planes. So, remove all of the D10 and D70 flashes from files Artwork_02 and Artwork_07. Note that on file Artwork_02 (the Component side) one must hand remove the one D17 flash. This removes this 33 mill thermal relief flash from the Therm-Gnd end of R?? which connects the Therm-Gnd to the signal Ground. The thermal relief flash is not wanted on the Component side because this pattern has already been drawn by a 20 mil outline air gap. The actual connection to Therm-Gnd is made by the thermal relief on the Solder side. Hole Count ---------- Finished Size mils Count ------------------ ------- 13 91 35 122 4-40 90 10 UnConnected Pin Count = 19 -------------------------- Rectangular Cutout ------------------ There is a Rectangular Cutout under the 68 pin socket. Plate walls of this hole (and plate the edges of this card itself). The drawing says that this rectangular cutout is 0.715" x 0.715". The larger IR Labs board from summer 1997 has a cutout of this size. The ?? card from Jeff has a 0.650"x0.650" cutout. The rectangular plate on top of the rectangular block in the new (summer 1997) dewar is 0.750" x 0.750". The rectangular block itself is about 0.628" x 0.627" (I expect the target cross section for the block was 0.625" x 0.625" . The distance between rows of pins, from one side to the other on the inside of a 68 pin socket is 0.800". The outside diameter of our thermal relief for the pads for this socket is 0.084". Need to keep the planes back about 20 or 25 mil. All power plane connections go to the outer ring of pins on the socket. Both analog grounds go to the outer ring of pins. The digital ground goes to a pin on the inner ring. The only thing that needs to go through the rectangular hole in the ROCK is the rectangular block. The 0.750" x 0.750" plate mounts onto the block after the ROCK is installed. So let's setup the cutout in the following way: 0.042" for pad thermal relief plus 0.008" plane copper plus 0.025" plane relief --> 0.075" socket pin center to edge of cutout --> 0.650" x 0.650" ID of the rectangular cutout This uses a 50 mill wide line shape to relieve the planes. The center of the 68 pin package is at x = 1.900" y = 1.600" so the corners of the cutout (and of the plane relief line) are at: 1.575 , 1.925 +-------+ 2.225 , 1.925 | | | | 1.575 , 1.275 +-------+ 2.225 , 1.275 Thermal Contact --------------- The bridge that comes down over the TCM-2620 uses three 4-40 screws on each side to hold it to the cold plate. The foot print of each side of the this bridge is 1.000" long by 0.190" wide. Sending out the Manufacturing Data ---------------------------------- By had move from the DIRAC [...ROCK] directory to the /Copy_to_Flop_Dir directory the following files: APERTURE_TABLE_REPORT.TXT ---> aperture.txt DRILL_TABLE_REPORT.TXT ---> drill.txt Manufacture_Instructions.TXT ---> instruct.txt COPY_TO_FLOPPY_DIRECTORY.SH located in /rock_uber is used to move Gerber and drill data files from /pcb/mfg to the /Copy_to_Flop_Dir