Ground plane for Backplanes

[Mark T]

Maybe a bit late to ask this as I already sent the files for manufacture.

On RcBus the ground and power are at the middle of the bus, so effectively the signals are crossing a slot in the ground at each side of the ground and power connection if the backplane has a ground layer. Most backplanes don’t have a ground plane so maybe there is nothing to consider here, just the position of the ground and power at the middle.

With DIN41612 connectors it seems common practice to put power on a1, b1, c1 and ground on a32, b32, c32, for example on ECB. If 5v is decoupled to ground close to pin 1 on both the backplane and the module then the signal connections are crossing a slot in the ground but this is a slot effectively closed at each end.

Any thoughts on which of these two choices is better for signal integrity or EMI/RFI?

[Mark T]

The backplane boards arrived and looking good, though not built and tested yet. I ordered 5 and received 8.

These are six layer boards from allpcb at 150*100 mm for $1 for 5, introductory offer. The stack up used was Ground, Signal (a) and power, Ground, Signal (b) and power, Ground, Signal (c) and power. I requested they use their alternate stack up of approx 0.2 mm prepreg and 0.4mm core to try to increase transmission line impedance, but as I used 8mil traces the estimated impedance is less than 50 ohm for rows a and b. I reduced the annular ring of pads on internal and top layer to 10mil, though this might be reduced further. Pads with no connection on inner layers can possibly be removed but then I would need to stop the ground fill from creating a short to ground and I was impatient to submit this.

Traces on each layer are arranged to connect each pad at 45 degrees and flow through to 45 degrees on the opposite side, with ground fill between signals on each signal plane.

Spacing of connectors on 15mm centres to match the 150x100mm pcb offer and the extruded aluminium rails that I plan to use.

Power to be supplied from one of the modules or from a separate front panel pcb.

This is an entirely passive backplane with vcc on pin 1 of every row and ground on pin 32 of every row. No daisy chain set up and none of the pins from 2 to 31 are committed. There is an extra row of ground pins at each end to allow for experimenting with bus termination and an additional b and c row at the left edge to allow a right angled plug to extend to another backplane, but the 15mm space between connectors will not be maintained. This might be used instead for a front panel on the rear of the chassis.

I’m planning to use 64 way a+b connectors, but included row c on the top signal layer for future experiments.

I’ll probably add 0.1uF smt capacitors between vcc and ground at pin 1 of each connector and also the same on each module.

I might have a problem driving the low impedance, though I do plan to buffer signals to the bus.

[Tom Storey]

I don't think(?) theres much argument in it, but as I understand it for digital the best choice for signal integrity etc is to have a ground plane adjacent to each signal layer, with traces sized to create 50ohm impedance (greater distance between reference and signal = thicker traces.)

If Robert Feranec's videos have taught me anything, its that signals aren't just a voltage level, but also a current flow. And the return current flow would ideally like to return to the source via the reference plane following the same path back (not as the crow flies as such). Any interruptions to this path will have some kind of an effect.

ECB's power/gnd arrangement isn't great in this respect, but I think in the context of the kind of system that would be using it, it just happens to work. Contrast that to something like PCIe where between every diffpair is a ground pin...

The thing with low speed digital circuits like we tend to encounter in retro computers is that they tend to be so "slow" that most of the effects simply don't get "felt", except perhaps in the worst of cases. It would be interesting to stick one next to an EMI meter to see what it was spewing out though. :-)

--
You received this message because you are subscribed to the Google Groups "retro-comp" group.
To unsubscribe from this group and stop receiving emails from it, send an email to retro-comp+...@googlegroups.com.
To view this discussion visit https://groups.google.com/d/msgid/retro-comp/c67407d1-8b09-4bdb-abc7-20b802307142n%40googlegroups.com.

[Mark T]

I watched a yutube video recently where the guy expained the power of the signal is carried by the dielectric not the copper which just creates the waveguide. I tried to find it again to post a link but can’t find it now. He showed examples of field measurements for signals crossing slots in the groundplane, for slots open at one end, closed at one end and as a series of slots. The slot open at one end was the worst for emmissions.

Its not so much the frequency of the signal, but the rise and fall times of the edges and the fourier transform of those edges into the frequency domain.

I’ll include caps on the backplane and boards from Vcc to ground to try to close the slot. It might not work, but I don’t think it will cause any problems.

I might route the clock on one of the centre pins with an adjacent ground and add some additional grounds if i have unused signals.

[Mark T]

I found the link again, it was from 6502.org sticky thread on high speed digital circuits. Its over two hours but quite interesting.

https://www.youtube.com/watch?v=ySuUZEjARPY

[Mark T]

I finished assembling the rack, I think its turned out OK but found a few things that might be improved.

I used pcb for a bracket to mount the backplane to the rails. Size fits within the allpcb limit of 150 mm x 100 mm for double sided boards, 5 for $5, but only for green pcbs, i had considered splitting the bracket into 75mm lengths and ordering from jlcpcb in blue.

Similar for the pcbs holding the guide rails, so these are also green. I used the drawing from an aliexpress listing for the guide rails, showing mounting plate thickness of 1mm and holes at 4.7 mm diameter. 1mm pcb thickness is too thin and the holes are a loose fit, so I probably need to add some glue.

Position of the pcb for the guide rails in the aluminium rail slots was adjusted with packing pieces and then the gaps filled with hot melt goo. I don’t think it should be sold as glue because it doesn’t stick much, but it does fill the gaps.

I had planned on using 2mm aluminium plates for the side panels, but couldn’t find 2mm aluminium sheet in small sizes locally. I think plexiglass turned out better, I would have had a problem machining aluminium neatly, but a desktop router was able to.drill the side panels and make a reasonable finish on the cut edges. This also makes it easier to see the alignment of the boards to the connectors.

The guide rails for the leftmost slot need to be sanded down by about 0.8mm to fit as the first slot is centred on 4.2mm from the left panel. These black rails are 10mm wide. I had expected this but wanted to keep 10mm height available on the component side of each board.

I need to replace the nylock nuts on the backplane connectors with ordinary nuts as the locknuts prevent the plugs from being fully inserted.

Now I need to concentrate on boards to go in the rack.

[Mark T]

The overall height is 121mm, but maybe I should change this to 5 inch, 127mm to be same as 3u rack. Not sure if this helps compatibility of front panels due to 15mm width with 4.2mm pcb centre from left edge. I can get plexiglass precut at 5x7 inch which would make it easier to make the side panels. 

For the guide rails it might be better to cut slots in plexiglass, I was surprised how well the desktop cnc router cut the plexiglass, but putting a lead in on the slots might not be so easy.

[7alken]

hi, interesting, I saw that VERY cool altium video too, probably important at higher freqs, up to 166MHz (say, VHF)), another beyond seems to be near to black magic, to me, at least ))
Petr

[Mark T]

Its the rise and fall times that determine the frequency, it will be easy to get harmonics at 166 MHz even with 74hct series.

13MHz master clock on GSM phones used to desensitize GSM channel 5 and 70 receiver, and that wasn’t even a 13MHz square wave.

[7alken]

ya, understood, and crazy ... btw, just yesterday I chatted about SiTime MEMS oscillators programability and the machine found my miss of OTP on these,
I thought they are REprogrammable, so in case of TimeMachine-II use, FP "clean" parts for prototyping are required ... but at least DigiKey had article they can put into them
anything on every order ... so, even weird clocks for old video processors etc ...and they have programmable also that rise/fall times; cool;
here is the chat:
https://chatgpt.com/share/68251444-976c-8000-b71b-a5bd5a8d593e

[Mark T]

Well I measured the impedance of one of the buried traces using a nano vna at 44ohms, slightly lower than the online impedance calculator but not far out.

Used a pcb mount sma connector soldered into A3 on slot 10 and ground at the adjacent row of ground pins. Calibrated the vna at the end of a short length of Rg402 using the same style sma connector with open circuit and short circuit, and N type 50 ohm load Via an adapter. The first minimum on |Z| was at 203MHz for 1/4 wavelength and |Z| was 44ohm at 101.5MHz for 1/8 wavelength.

Then terminated A3 at slot 1 with 44 ohm, 47 // 680, to verify approximately 44 ohm from 50MHz to 900 MHz.

This was without any DIN41612 connectors fitted, but I don’t want to solder those in place until I confirm I can drive the bus with buffers.