New Bipolar Boost TX and Front End

[KingJL]

If you don't find anything else before the AM (my time), I will post the updates in the morning... if you do, I will address what you find and then post the updates.

The design of the Single Board Bipolar TX w/ADuM4120 MOSFET drivers has slightly changed. U1 has been changed from an LM317 to the smaller footprint AP2204K-ADJ; As per Mdtoday request, U16 and C55 have been moved physically closer to the REF pin of the LTC2378 ADC; orientation of Q1 was changed to reduce the possibilty of crosstalk affecting the gate; the orientation of various component REF disignations was changed to enhance readability.

New PCB top veiw:


New PCB bottom veiw:


Updated schematic:
Bipolar PI ADuM Single Board Schematic.pdf

Updated BOM:
Bipolar PI Single Board BOM.pdf

Updated Gerber archive:
Bipolar-PI_singleboard_Gerbers(1-9-2020).zip

Updated Kicad archive:
TX_ADuM_single-board(1-9-2020).zip

[KingJL]

Ahh.. I see the 47uF now.

Agree, when we used that ADC here we had enough C but it was not close enough to the ADC like you did (C55 at U16). But the ADC_REF Voltage drooped at the ADC pin.



That should be better.
Ideally C55 needs to be as close to the ADC pins 7 & 8 as possible. Not into ground plane but directly to ADC's ref ground (pin 8 ).

This becomes much more important when the number of ADC bits increase. Getting good performance from a 16bit ADC is hard, 20 bit ADC is harder still.
20 bit ADC is only 7.8uV per bit.

Thank you @waltr for your input/feedback... very much appreciated!

[Mdtoday]

The design of the Single Board Bipolar TX w/ADuM4120 MOSFET drivers has slightly changed. U1 has been changed from an LM317 to the smaller footprint AP2204K-ADJ; As per Mdtoday request, U16 and C55 have been moved physically closer to the REF pin of the LTC2378 ADC; orientation of Q1 was changed to reduce the possibilty of crosstalk affecting the gate; the orientation of various component REF disignations was changed to enhance readability.
[ATTACH=CONFIG]49111[/ATTACH]

Looking really good!
Given the ground plane layer, via stitching and your actual separation / positioning of the power input, TX switching and RX circuits, I think this board should be fine.
I am part ways through checking the latest files and all is good so far, nice job.

[Mdtoday]

@KingJL, I have looked over PCB and can't spot anything but will leave it a day or so and go over again.

I have also designed 3 versions of PCB shields, with my preference leaning toward V4 below







These are very preliminary drawings just to convey the idea.
All versions would be 3D printed and outside sprayed with super shield nickel spray

[KingJL]

@KingJL, I have looked over PCB and can't spot anything but will leave it a day or so and go over again.

I have also designed 3 versions of PCB shields, with my preference leaning toward V4 below

[ATTACH]49113[/ATTACH]

[ATTACH]49114[/ATTACH]

[ATTACH]49115[/ATTACH]

These are very preliminary drawings just to convey the idea.
All versions would be 3D printed and outside sprayed with super shield nickel spray

I kind of like V4 also. Is heat buildup (especially in the TX area) going to be an issue?

[Mdtoday]

I kind of like V4 also. Is heat buildup (especially in the TX area) going to be an issue?

If we use some tin sheet top/bottom in those areas and 3D print the side walls, that should be ok I think.
Press forming a thin sheet of tin is also an option.

[KingJL]

If we use some tin sheet top/bottom in those areas and 3D print the side walls, that should be ok I think...

That should do the trick. The tin sheet can be secured to the 3D printed sidewalls with EMI shielding tape. I like it!!! Sounds like a plan!

[KingJL]

That should do the trick. The tin sheet can be secured to the 3D printed sidewalls with EMI shielding tape. I like it!!! Sounds like a plan!

Also we could use something like this or this between the MOSFETs and the tin sheet. I worked on an automotive ecu that used something akin to these to conduct heat from the MOSFET to a metal case shield. Although those were a little thicker... maybe >=3mm and were black.

[Mdtoday]

Also we could use something like this between the MOSFETs and the tin sheet. I worked on an automotive ecu that used something akin to these to conduct heat from the MOSFET to a metal case shield. Although those were a little thicker... maybe >=3mm and were black.

Yes, for sure, I use Warth heat transfer sheets for same thing in ECUs and this little 4 amp switch mode module, it's good material

[waltr]

@KingJL, I have looked over PCB and can't spot anything but will leave it a day or so and go over again.

I have also designed 3 versions of PCB shields, with my preference leaning toward V4 below

[ATTACH]49113[/ATTACH]

[ATTACH]49114[/ATTACH]

[ATTACH]49115[/ATTACH]

These are very preliminary drawings just to convey the idea.
All versions would be 3D printed and outside sprayed with super shield nickel spray

The idea of shields is good BUT - what is the purpose???
1- Keep external EMI out of RX circuit?
2- Keep EMI inside and from radiating- FCC/CE EMI compliance?
3- Which parts of the circuit need shield?

v4 will not work since it has a huge opening where the processor plugs in. This will allow RF energy in enter/exit.

@JLKing,
On schematic I see U2D is used to short the RX input (RX_BLANKING) which should help keep the RX preamp from overloading.
However, this blank switch is only when using a Mono coil.
Would it be better to have this blanking switch on the other side of U2B & U2A? Then it can Blank with an IB coil.

From the shielding subject I am looking at the GERBERs to study grounds and current flow and notice a few things.

1- The 20V path on layer In2 goes to D1 through a single small via. Is this one via large enough and have low enough impedance? Adding a few more vias may be better.
20V to D2 should be ok since it feeds to REF regulator and op-amps. D2 could be a smaller diode.

2- It may be better to 'Split' the ground plane into TX and RX sections with a 'Star' connection at/near the power connector. This help keep TX circulating current out of the RX circuit.

3- Does the Processor module (plugs into J5) really only have One Ground pin? If it has more than all should be connected.

Great effort on this whole project and waiting for more results.

PS- I did quick code to setup a PIC32MZ-EF to output timing pulses. Running in the MPLAB Simulator looks good.
It uses a hardware timing clocked at 100MHz and 7 OC modules to time pulses. Once these are setup and running the main() code does not need to do anything.
I am planning on getting a Demo board with a PIC32MZ-EF so I can measure real outputs.

[KingJL]

@JLKing... On schematic I see U2D is used to short the RX input (RX_BLANKING) which should help keep the RX preamp from overloading.
However, this blank switch is only when using a Mono coil. Would it be better to have this blanking switch on the other side of U2B & U2A? Then it can Blank with an IB coil.

Actually the purpose of U2D is more complicated than just blanking the RX. Yes it is effective at blanking the RX only in mono mode. but more importantly there is a very short (~1 usec or less) overlap where U2D is energized and the "DAMP" switchwes are energized. This extremely brief overlap has the effect of applying a very low resistance across the TX coil and quickly dissipates any residual charge in the TX circuit resulting in ZERO coil current (that is the theory anyway... in practice, the coil current usually is not zero, but is anywhere from a few micro-amps to 1 ma). This all works for both mono or IB mode. In IB mode, the need for RX blanking is less pronounced (asuming an IB is anywhere near properly balanced). In fact with the front end as designed, RX blanking is not needed at all as the frontend never goes into saturation regardless of input.

[KingJL]

The idea of shields is good BUT - what is the purpose???
1- Keep external EMI out of RX circuit?
2- Keep EMI inside and from radiating- FCC/CE EMI compliance?
3- Which parts of the circuit need shield?

v4 will not work since it has a huge opening where the processor plugs in. This will allow RF energy in enter/exit.

Part of this, I can answer. I will let @Mdtoday address the V4 issue as he has usually well thought out approaches to his design proposals.

The parts of the circuit needing shielding are the anlog RX circuitry, but it is hard to isolate all of the RX path as it consists of all current paths from the coil, damp switches, coil switch, RX blanking switch, pre-amplifier IC's, pre-amp out-put unipolarization switch, ADC input differntial coversion buffers, ADC input filter circuits, RX refernce generator, ADC refernce generator, and ADC analog supply. In fact "RX analog" includes much of the TX circuitry. This shielding is a further attempt to quiet down the RX, primarily for the 20 bit ADC envirionment.

BTW: Some how my editor envirionment has changed where I no longer have spelling issues identified. How do I turn this back on... doesn't seem to be option on the editor menu.

[waltr]

JLKing,
Thanks for the explanation of the RX_Blank function. This makes sense for where U2D is connected.

I was also thinking shielding the RX analog circuits only.
Idea being to keep switching and processor noise out of the RX signal.
However, I do not think that simply shielding this part of the circuit will do anything useful since as you said, the RX is connected to TX circuits.
More effective is the PCB design, particularly Ground paths, to keep the RX signal quiet.

I do work with very sensitive analog circuits. We (where I work) have found that Ground paths are very, very important for quiet analog and high count ADCs.

[KingJL]

... More effective is the PCB design, particularly Ground paths, to keep the RX signal quiet.

I do work with very sensitive analog circuits. We (where I work) have found that Ground paths are very, very important for quiet analog and high count ADCs.

That is why on this PCB, not only do we have a dedicated ground plane layer, but both the top and bottom layers have a ground "pour" over the full dimension of the board and all 3 layers are stitched together with an array of via's (one array spaced 10mm apart and another array offset by 5mm in both x and y directions with the same spacing), thus ensuring that there is a maximum path length of 14mm for a ground return of any signal. Also key areas have extra stitching via's to ensure the shortest paths through GND (especially for the ADuM4120's and the LTC2378 REF).

[dbanner]

BTW: Some how my editor envirionment has changed where I no longer have spelling issues identified. How do I turn this back on... doesn't seem to be option on the editor menu.

I had the same problem with firefox browser, one day it just stopped working. But with chrome browser, the spell check works fine. Very strange.