RPL1116 (MSO1000Z) and PLA2216 (MSO5000) Active Logic Probe teardown

[joeyjoejoe]

I can get the 7324 symbol in the KiCad library - should help clean up the project a bit if it's a standard symbol.

[dren.dk]

According to the datasheet there's plenty of protection diodes built into the LMH7322, so no external diodes should be needed.

The presence of the input network should be plenty to limit the current in the built-in protection diodes, to the point where you'd have to go seriously nuts to damage anything through a 90k resistor.

Putting the pod directly on the scope is a terrible idea, the whole point of putting the input comparators in the pod is to keep the sensitive single-ended input leads short and get the signals converted to robust LVDS for the long journey through the ribbon cable to the scope.

[wraper]

According to the datasheet there's plenty of protection diodes built into the LMH7322, so no external diodes should be needed.

ESD protection is not better than average MCU has.

The presence of the input network should be plenty to limit the current in the built-in protection diodes, to the point where you'd have to go seriously nuts to damage anything through a 90k resistor.

Not nuts. Spark can easily jump over small resistor. If there are spark gaps on PCB, then it would not happen, though.

[dren.dk]

Hmm, iIt would not be too hard to model the input network in LTSPICE along with the 100 pF + 1k5 resistor needed to simulate a HBM discharge.
See: https://en.wikipedia.org/wiki/Human-body_model

I have not done any simulation or calculations, but my gut feeling is that the energy that makes it into the device is on the very low end that can easily be handled by the built-in diodes.

Do you want to do the simulation?

[wraper]

HBM is something so low in energy that not even worth considering for finished device IMO. Real discharge often will have over 20kV and higher capacitance.

[TK]

Remember this is a digital POD, it is not going to take high voltage in.  I have several logic analyzers (HP, Agilent, Zeroplus, saleae) and I have also analyzed the digital input on Agilent 54622D... the only protection they have is the resistor divider (I think it is 10:1, if I remember correctly).  Even the very expensive high end Agilent Logic Analyzers had resistor network at the input of the comparators.

[dren.dk]

How large discharges are logic analyzers typically designed to survive?

I failed to find a rating of the internal protection diodes of the LMH73222 in the datasheet, the closed I got is that the device survives 2.5 kV HBM and 250 V MM, but perhaps a simulation results of those discharges can be used as a bench mark for discharges though the network.

My guess is that someone experienced in the art of test and consumer gear has already done those simulations and possibly even real-world tests and concluded that nothing reasonable would harm the inputs.

[Vtech]

How large discharges are logic analyzers typically designed to survive?

I think you shouldn't plug it directly into mains socket

Logic analyzers are used in different situations than analog scope probes. You probe some CPU and interface signals not ~kV levels on IGBTs of your 10kW converter. From my experience, input divider of logic pod is enough protection. I've blown several scope probes including high voltage one but never hurt a logic analyzer.

For proper input protection you would need some bigger size resistors (like 1206 at least) and some TVS with breakdown voltage above +-15V and that would be bad for fast signals and signal integrity.

[SilverSolder]

How large discharges are logic analyzers typically designed to survive?

Funnily enough, I was just looking at the specs of the 54622D for other reasons...  -   the digital inputs are rated at max +/-40V peak.

The destruction level is probably quite a bit higher than that.

[dren.dk]

I'm starting to lay out the board and I've used relatively agricultural 0603 passives for the layout, because I suspect I'll have to hand-assemble it:)

I'm having a hard time making it work on two layers, so I think I'm about to buckle and go 4-layer, which is a first for me:)

Getting the pitch of ICs down to 10 mm should be easy enough with 4 layers, even when dedicating a whole layer just for ground.

I think the stack should be something like this:

TOP: Signals  (and almost all components)
1: Ground plane
2: Power and jumpers
Bottom: Power, jumpers and decoupling caps.

I like having the ground plane and uninteresting stuff on the inner layers for debugging, but I worry that sticking the ground plane in the middle means that it's much less effective as a heat sink, is that a valid concern?

[texaspyro]

Bottom: Power, jumpers and decoupling caps.

Try to keep all parts on the top layer... it makes it a LOT easier for most people to build.  Double sided components tend not to work well with a home reflow oven.

[Rerouter]

for the lmh7322, its easy to pull off 2 layers, It will just be a little wider than the original, Have fun, For the second block, I just duplicated and renamed the references, would probably recommend similar for the other, equally without the silk, you can pack them very close, may just need to nudge the matching networks a tad if you want it as small as possible.

[Vtech]

This layout looks teally nice but I think there will be problems with overheating. Thermal pad is not connected to large plane.
Look at the attached thermal image of Rigol's RPL1116 pad without the case. Chip temperature already above 60degC!
This design (I'm taking about Rerouter's layout) would requires some heatsink glued to the chips.

[Rerouter]

That was just to give you an idea on how to do a 2 sided, PCB with all components on 1 side,

The traces can be nudged to get some good via coupling to the VEE pins (-2.5V on the schematic), To the same extent the -2.5V connection to the capactors and similar could be made much thicker to pull some heat with them

At 38C/W, and what reads as about 0.25W of dissipation from the datasheet, I cant see where there is much need for over the top PCB cooling.

Edit:
Part of the extra heating your seeing there is from the ones on the back, Ironically by making it on the same side, the density of the heat sources would be lower.

Edit2: Here is what you could do if you wanted some extra heat sinking.

Edit3: Just to make clear, at this point I have put 0 effort into impedance matching, If you guys need help with it, I would just need to know what board thickness your working towards.

[ebclr]

What about to make the board for only one channel, a very tiny board, and use 16 boards connected to one big adaptor board. Will this improve signal integrity since the wire will be differential and less susceptible to noise?

Do this make any sense?

[Rerouter]

Single channel PCB's would be a bit of a pain due to the common wires between all the channels, meaning at the wiring loom side you would have a proper mess.

8 channel podlets is easy enough, and 4 channel I would probably call the cut-off for wiring mess issues.

Also Third go at it, each channel pair is 12.5 x 22.8mm in size, so 8 channels can be made into a board about 50mm in size, I suppose if you rotated the resistor networks you could scrape back enough room to try and cram both podlets onto a 50 x 50 mm pcb order. but I don't see the point seeing as you generally get 5 or 10 boards per order.

[joeyjoejoe]

What size components are these? 0805?

[Rerouter]

0603 and a 0.5mm pitch QFN, If your not used to Kicad, the Red is the Copper pads / traces, the Purple is the solder mask (currently at the default, can easily be trimmed down), and the White is the "courtyard" essentially a spacing guide for components so they are easy for most pick/place machines to use. In general I have found kicads default courtyards are relaxed enough that most people should be able to hand solder them.

[ebclr]

Interesting tool to make a team PCB, porting to this tool

https://upverter.com/3DgeekStore/c728af4c317fb73e/lmh7322/

[Rerouter]

Link seems to be broken?

[ebclr]

https://upverter.com/3DgeekStore/   then find for lmh7322/

[ebclr]

need one email to be invite to the project collaboration, Tell and I will add

[Rerouter]

Probably my last run for a while on this, All that's left is adding the 50 pin connector, and routing for it. as you only need to route half the channels, it should be easy. I just can't be bothered making the footprint.

[joeyjoejoe]

I can help with the footprint. Do we know what sort of connector it is?

I've got a pull request in for the 7324 symbol.

[Rerouter]

2x25 1.27mm pitch, intended for mounting on the edge of the PCB, so 1 row of pins per side of the board

Don't know the exact plug part number.

I suspect this means the PCB is 1.0mm or 0.8mm thick.