I have some time today to continue this discussion.
Sent from my iPhone > On Aug 11, 2017, at 10:15, Richard Wilbur <[email protected]> wrote: > On Thu, Aug 10, 2017 at 2:01 AM, [email protected] > <[email protected]> wrote: >> GND shielding parallel to the differentials is interrupted quite >> often. Those GND tracks act as shields, for emission and reception. >> I'd try to put as much parallel GND as possible. >> >> And trace the parallel GND around the via's, see attachment. >> >> Make sure the'res as much solid GND on the layer above and below the >> traces, again shielding. microstrip differential-mode signal with ground shield traces ground signal+ signal- ground dielectric dielectric dielectric dielectric ground ground ground ground ground ground Here the dipole antenna remains small and the half-strength fields between each signal trace and its associated ground guard shield trace work to truncate electric fields in the plane of the PCB. The fields are still insignificant in far field (because the traces are close together, have opposite potential and currents, and the fields cancel each other). It seems the best argument for including ground shield traces on this layout might be to guard against coupling signals between differential pairs that were packed in too closely to otherwise meet the recommended distance between different signal pairs. But with the dimensions of our layout being the minimum allowed by the board fabricator, the min(s) = min(w) => d = s + w + s = 3 * s.[1] So if we were to remove the ground shield traces from between differential pairs we could meet the inter-pair spacing recommendations without moving anything else. This may explain the design by the wits-tech senior engineer you mentioned which worked without ground shield traces between the differential pairs. The ground shield traces surrounding a differential pair on the same layer will mostly block common-mode signal radiation and coupling. They will have little beneficial effect on differential signals--but can contribute asymmetric loading (lower single-ended impedance of one trace) to the differential pair (through asymmetric geometry) which will convert some differential energy into common-mode energy. In other words, if we are expecting significant common-mode signal, whether from pathologies in the layout or incompetence of the differential-mode signal driver, then ground shield traces may be in order. Regardless, caveat emptor (let the buyer beware): 1. asymmetries in ground guard shield implementation contribute to conversion of differential signal to common-mode signal (which for a differential receiver is noise, thus lowering signal-to-noise ratio), 2. symmetric ground guard shield traces reduce the single-ended impedance of both traces of the differential pair, lowering the differential impedance of the pair. The effect is distance-dependent, the greater the spacing the less-pronounced the effect. Another interesting reference on high-speed HDMI PCB layout is TI's SLLA324[2]. Notice how in none of the layouts pictured in Figures 4, 6, or 8 are there any ground shield traces. Judging from the eye diagrams in Figure 10, even with fairly close pair-to-pair spacing there doesn't seem to be significant cross-talk between the pairs (look for noise at transitions): 1. in the absence of ground shield traces 2. running at top speed of HDMI v1.4 (340MHz pixel clock, 1080p video, 3.4GHz data rate) 3. space between differential pairs doesn't seem to be all that large. Figure 4 looks like it depicts a similar connector (micro HDMI <=> type D) and it looks like they have a similar pair length relationship (which, interestingly enough, they don't seem to take any pains to equalize): length(D2) < length(D0) < length(D1) < length(CLK) So, for the HDMI differential signals' sake, we don't necessarily need: 1. Ground guard traces between neighboring differential pairs 2. Ground guard traces between HDMI differential pairs and other circuits 3. Multiple ground vias riveting along the side of the board to block emissions 4. Perfectly matched inter-pair lengths On the other hand: 1. Ground guard traces can be important in reducing noise radiated from single-ended circuits and coupled into other single-ended circuits on the board. 2. Ground fences, traces riveted with multiple ground vias, can help even more with the goals of "reducing noise radiated from and coupled into other single-ended circuits on the board" as above. In other words, if we had more board space there are several things we could do differently: increase differential pair trace width and spacing, ground shield trace spacing. But as it stands I believe it will likely work fine. Without changing anything else we could drop the ground shield traces which would serve to increase our differential impedance. We would want to retain the ground vias near signal vias. Reference: [1] HDMI, p. 5.2 [2] SLLA324, pp. 4-7 Bibliography: Texas Instruments (TI): "HDMI Design Guide", High-Speed Interface Products, June 2007, http://e2e.ti.com/cfs-file/__key/telligent-evolution-components-attachments/00-138-01-00-00-10-65-80/Texas-Instruments-HDMI-Design-Guide.pdf Texas Instruments (TI): SLLA324 February 2012 Application Report, "TPD12S016 PCB Layout Guidelines for HDMI ESD" http://www.ti.com/lit/an/slla324/slla324.pdf _______________________________________________ arm-netbook mailing list [email protected] http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook Send large attachments to [email protected]
