Dan's Notes on the Cold Board --------------------------------- Initial Rev. 14-May-2020 Current Rev. 24-June-2020 Zoom meeting with Niyaz about the cold board on 14-May-2020. - The circular 56 mm OD shape is needed. - The two heavy traces in has auto-cad drawing are filament connections to provide a source of electrons. - He switches the signal from one side to the other because the GPO coax enters on one side of the chamber and the chip trench needs to be on the other side. - He is going to pass to me some dimensions, e.g. his 50 Ohm trace design, mounting hole locations, trench size, radius of connector mount locations, polar angle of connector mount locations - I do not know if they just need to get uwave power over each of their 14 runs or if they need low loss and no reflections, i.e. constant Zo on these runs ? - I did not fully understand the requirements for the chip trench: Does it need to go the whole way down to the bottom copper or can one leave 5 or 10 mils of dielectric over it ? Does the chip need to contact the copper at the bottom of the trench - I don't think so. Date: 15-May-2020: ------------------ - Using a standard 5 pin THD GPO connector, e.g. A008-L15-03 to launch the signal on the opposite side of the card from where the connector is mounted (i.e. doing this in the normal uwave way) does not work in this case because: They want to use the high dielectric constant laminate Dk = 10.0 or 10.2 which drives down the Zo of the section of the line passing through the card to 38 or 40 Ohm range. The Reference Plane height above the surface of the PCB is different for the normal straight through 5 pin THD connector and the blind surface mount SMD connector 5 pin THD A008-L15-03 70 to 74 mil Ref Plane above pcb blind SMD A012-P95-01 88 to 94 mil Ref Plane above pcb This 20 mil difference is twice the axial tolerance for GPO. Why did Corning make them different ? - My main concern with the current layout is that all 14 signals change surfaces right next to each other where there is the least control of return currents and the maximum likelihood of cross-talk. A better solution might be to change signal surfaces right near where the GPO connectors are mounted. That provides plenty of isolated space for each signal to have a good controlled Zo transfer through the card and will minimize cross-talk. Once the transfer is done then one can use the ground backed co-planar run over to the bonding pad next to the chip trench. - From Niyaz's auto-cad drawing I try to extract some approximate dimensions based on knowing the 56 mm diameter. Things are not supper accurate but this is the best data that I have for now. Extract and Rationalize: The chip trench is about 2.25 mm wide and 7.0 mm long The radius to the 4 mounting holes is about 23.5 mm The diameter of the mounting holes is about 4.2 mm The radius to the 16 GPO connectors is about 23.5 mm The width of the small uwave traces is about 0.35 mm The width of the wide filament is about 0.55 mm The pads on the top side are about 0.35 mm Wide x 1.50 mm Long The pitch of the top side pads is about 1.10 mm Rotational Placement - I believe that: The X and Y axis are midway between two CPO connectors. The 4 mounting holes are at 45 degrees between the X and Y axis. Thus any pair of adjacent mounting holes are 90 degrees apart. The 4 GPO connectors between any pair of adjacent mounting holes are evenly spaced. I think that it is 20 deg between adjacent connectors. I think that it is 15 deg from a conn to a mount hole. So starting at the normal place in Quadrant #1 and rotating in the normal CCW direction we have: 10 deg Conn. J1 30 deg Conn. J2 45 deg Mounting Hole 60 deg Conn. J3 80 deg Conn. J4 100 deg Conn. J5 120 deg Conn. J6 135 deg Mounting Hole 150 deg Conn. J7 170 deg Conn. J8 190 deg Conn. J9 210 deg Conn. J10 225 deg Mounting Hole 240 deg Conn. J11 260 deg Conn. J12 280 deg Conn. J13 300 deg Conn. J14 315 deg Mounting Hole 330 deg Conn. J15 350 deg Conn. J16 - Review some of the transmission line Zo calculators: http://www.rfcafe.com/references/electrical/transmission-lines.htm https://chemandy.com/calculators/coplanar-waveguide-with-ground-calculator.htm https://www.pasternack.com/t-calculator-microstrip.aspx - Does Pasternack have a version of the GPO connectors ? Yes They (and perhaps the world) call GPO ---> SMP and have numbers like: PE44944 which includes 2 alignment Ground posts. Other Pasternack SMP solder mount male connectors include: 44840, 44879, 44910, 44947, 44966, 44967 - Other manufacturers of SMP connectors include the usual suspects: Molex, Amphenol, Radiall, Samtek, Cinch, Hirose, Rosenberger. The SMP family of connectors is actually: MIL-STD-348B. Digi-Key list over 100 male pcb mount SMP in stock. Some are much less expensive than the Corning Gilbert military connectors. For the blind male vertical smd SMP connectors there appears to be two "standards" for the height of the Reference Plane above the surface of the pcb: about 52 mils or about 90 mils. Currently I'm rather certain that the connectors that Niyaz is using have the 90 mil Reference Plane above the pcb surface. So far the Molex blind male solder mount parts that I have found have a lower Reference Plane than the Corning Gilbert parts, i.e. a shorter distance from the pcb surface to the insertion reference plane in the male connector. Date: 16-May-2020: ------------------ What specifically should I put into a first draft layout: - Design for a 30 mil thick (0.762 mm) Rogers AD1000 laminate with 1/2 oz copper on both sides and a Dk of about 10.35 - Use the Pasternack 44944 with the correct Reference Plane height and the two Ground posts. These are on the Bottom side of the boards - Exit the GPO with a co-planar pattern that uses is the same trace width as you will use for the wire bond pads on the Top side of the card. This ground backed co-planar design is: trace width 0.38 mm (to match the 15 mil diameter center contact wire on the connector), gap width 0.25 mm, Dk effective 5.91, Zo 51.0 Ohm. The two gaps and center trace have a full width of 0.88 mm which fits nicely within the slot in the solder disk of the GPO connector. Start the center trace run 2.00 mm from the center of the GPO connector, i.e. right in the middle of the distance from the center cylinder of the connector to the outer radius of the solder disk. Exclude ground copper from a disk of diameter 2.0 mm centered on the center of the GPO connector. Exclude ground copper for the length and width of the slot in the connector's Solder Disk. Note that in designing the Mentor Graphics geometry for the PE44944 there is some confusion as to the width of the slot in the connectors solder disk. This slot is either 0.045" or 0.035" wide. I think that the slot is 0.035" wide and that the circular opening in the center of the solder disk is 0.045" diameter. - A short radial distance from the connector change sides using a 5 wire array pattern. - For now I will *assume* that the radius to the center of the GPO connectors is 23.5 mm. - For now I will *assume* that the radius to the center of the mounting screw holes is 23.5 mm and that the diameter of the mounting screw holes should be 4.2 mm. Date: 18-May-2020: ------------------ In layout and routing of the Cold Board one must keep in mind the physical scale that makes a significant impact on the propagation of the micro-wave signals. Niyaz wants this card to work at up to 20 GHz. 20 GHz is a wavelength of 15 mm in free space. The traces on this card will probably have a velocity factor in the range of 0.5 to 0.6 so the wavelength on this card will be about 8 mm. The normal rule of thumb is that imperfections of physical size less than 1/20 of a wavelength are not a problem. This is a scale of about 0.4 mm. The normal rule of thumb is that imperfections of physical size less than 1/8 of a wave length are OK for certain aspects of a layout, e.g. how close the ground tie rivets are placed next to each other. This is a scale of about 1.0 mm. Date: 30-May-2020: ------------------ Notes from zoom meeting with Niyaz on Friday 29-May-2020: - Yes, there is a major change in the Cold Board design since the original 3 drawing sketch from Niyaz. The new design uses Corning A012-P95-12 (-T) connectors. These are very nice connectors that themselves take the signal through the card with their coaxial structure and then launch the signal on the Top side of the card. This eliminates the issue of transferring all the uwave signals from the Bottom to the Top right next to the Chip Trench. - I have frozen the design work that I did to implement Niyaz's original 3 drawing concept design and will start a new Mentor layout for Niyaz's new design for the Cold Brd. - Niyaz wrote a nice complete description of his new design for the Cold Board and I put this on the Cold Board web site. His write up of the new design contains 6 drawing with almost all of the required dimensions now specified. - In neither the old or new design does the Cold Board mount the whole way down against the copper Cover Plate for the Chamber. There is typically ?? mm between the bottom surface of the Cold Board and the surface of the copper Cover Plate. There there is no issue of traces on the bottom side of the PCB shorting to the Cover Plate and there is no issue of the connector Reference Plane height above the PCB bottom surface being slightly different for the new connectors than it is for the old type of Rosenberger SMP connector. That is the "seating depth of the two types of SMP connectors can be different and the new A012-P95-12 (-T) connectors will still physically work OK. In his new design there are a number of points that still need final decisions - but none of them block getting started with a Mentor layout for his new design. These issues are: - One can not mill the Chip Trench the whole way down to the bottom copper. The thickness of the typical test chip is 0.5 mm. So do we want to move from a 20 mil thick laminate to a 25 or 30 mil thick laminate so that a 0.5 mm deep Chip Trench can be milled in it and still leave 5 or 19 mills of dielectric support over the bottom copper ? Do we want to ask the Physics Dept M Shop about milling the trench ? Do we want the layout to include some vias in the trench so that one can use a probe to poke an old chip out of the trench when getting ready to test a new chip ? - We will move from the original sketch of 1/2 oz copper on top and 2 oz copper on the bottom to a balanced 1/2 oz on both sides. That make the card a lot easier to etch accurately, i.e. do not need to pre-distort the trace widths as much. - The diameter of the 4 Mounting Screw Holes is still in question. They are currently specified a 4.4 mm Dia and Niyaz thinks that the Mounting Screws are size 2-64. 2-64 is the UNF thread pitch but I wounder if they really are the much more common 2-56 size ? In either case these #2 screws are 86 mill OD about 2.18 mm. - Niyaz will look into aiming at 51 or 52 Ohm Zo and into trace dimensions needed for different dielectric thicknesses, e.g. 20, 25, 30 mill. - The two Filament traces do not need to be routed as uwave traces. The Filament is typically about 5 Ohms when cold and he uses 5 to 8 Vpp to generate electrons. I will look at rational trace widths for these two connections and into routing them as a low frequency pair. - We will need a final specification for the diameter of the through holes for the A012-P95-12 connectors. Their barrel is specified as 0.165" OD but no tolerance is given. This will be a good place to use a Finished Hole size specification with the PCB company and non- symmetric tolerances. - With the A012-P95-12 connectors there is also the issue of metal in the hole tunnel toughing the center conductor signal pin right at the edge of the hole. May want to touch that part of the hole ID with a ball mill which would be another reason for MSU machining of these cards. - Niyaz agrees that it is OK/good to hold back all copper on the top side for a very short distance from the edge of the trench (like I did in the Mentor layout for the original design). - Niyaz's drawings for the new design use a regular array of ground rivets but he agrees that it would be better to use a "follow the traces" pattern of ground rivets and then fill in with additional rivets where one can. The intent is to make all of the uwave traces as much alike a possible and the regular array of rivets would make horz and vert traces much different than 45 deg traces. The general idea for ground rivets is now about 0.4 mm Dia with follow the trace c to c spacing of about 1.5 mm and hold back from the edge of the ground plane adjacent to the signal trace by about 0.7 mm c to edge. This will be OK at 20 GHz and is within the normal range of things to manufacture. List of the major dimensions for the new design: - Radius to SMP connector centers 23.5 mm - Radius to Mounting Hole centers 23.5 mm - Starting at the normal place in Quadrant #1 and rotating in the normal CCW direction we have: 10 deg Conn. J1 30 deg Conn. J2 45 deg Mounting Hole 60 deg Conn. J3 80 deg Conn. J4 100 deg Conn. J5 120 deg Conn. J6 135 deg Mounting Hole 150 deg Conn. J7 170 deg Conn. J8 190 deg Conn. J9 210 deg Conn. J10 225 deg Mounting Hole 240 deg Conn. J11 260 deg Conn. J12 280 deg Conn. J13 300 deg Conn. J14 315 deg Mounting Hole 330 deg Conn. J15 350 deg Conn. J16 - uwave traces for now are: 0.25 mm wide with the copper ground plane held back 0.17 mm - The Center Conductor bond pads for the SMP connectors should be 0.38 mm wide and that should run for about 2.6 mm before tapering to the normal 0.25 mm wide uwave trace. Note that in reality that the Center Conductor bonding pad needs to be held back from the edge of the PCB hole by at least a little bit or else it will connect with the plating in the hole tunnel. - Vertical height of the two Filament Vias above the center of the card: 10.2 mm - Horizontal spacing c to c of the two Filament Vias: 7.4 mm i.e. 3.7 mm each side of the card's center line - Filament Via Hole diameter: 1.25 mm - Chip Trench 2.2 mm wide 7.2 mm long - The Wire Bond pads adjacent to the edge of the Chip Trench are: 1.2 mm long by 0.25 mm wide. - The Wire Bond pads are spaced: 1.0 mm c to c. Date 24-June-2020: -------------------- Meeting with Tom and Rob in the Machine Shop about doing the final machining on the Cold Board at MSU in their shop: - Yes, they can do both parts of the work, i.e. cut thinner by about 20 mils the dielectric in the Chip Trench, and cut the final round board out from a square blank. - For cutting thinner they would like to use a 1/32 inch end-mill which is about 31.25 mils diameter or about 0.794 mm diameter. - For cutting out the circular board they would like to use a 1/8 inch end-mill, 0.125 mils diameter, or about 3.175 mm diameter. - They would like the thinnest web between the perimeter of the circle and the edge of the square to be 200 mils thick or more - 200 mils is fine. Given that the finished circular Cold Board is 56 mm in diameter this means that the length of a side of the square blank board must be at least 56 mm + ( 2 x 200 mils) = 66.16 mm. - They would like the holes in the 4 corners of the square to be for 1/8 inch diameter doll pins. - If pushed they could try going to a 20 mil diameter end-mill to thin the trench.