I had a few questions:
Question 1: Frank uses very wide traces for +Vz and -Vz coming out of the LTZ1000, to reduce ohmic losses in the traces. However, my understanding is that once the LTZ1000 is insulated (e.g. in a bit of foam), the majority of the heat egress is through the copper traces. Here I've tried out a layout which takes the opposite approach: use skinny traces to minimize the heat egress. My understanding is that the down-side of this approach is that R1 can be considered to have two parts: the 120R resistor, and the trace leading to it, and the trace leading to it has the poor temperature coefficient of copper. My question is, how can I develop an intuition about which side of this trade-off is better, optimizing the tempco of R1 via fat traces, or minimizing heat egress via skinny traces?
Main idea for these broad traces is having very good thermal conductivity, so that the solder joints of the LTZ1000 pins 3 +4 are approximately on the same temperature as the corresponding solder joints of +Ref and -Ref.
The +Ref PCB track carries the zener current of 4mA, whereas the -Ref track carries about 200µA only, i.e. both collector currents. Evidently, I did not balance both tracks in terms of voltage difference across these paths. So I doubt, that it will make any difference, if you use smaller tracks.
Anyhow, as I have a single sided board, the number of solder joints / thermocouples is reduced to a minimum, and these are pairwise symmetric from the LTZ1000 footpoint to the outer jacks, so cancelling each other.
As all these solder joints are located on one horizontal plane, that should help to equalize the temperature difference between all of them.
2 layers or even 4 layers create much more potential thermocouples (i.e. by the vias), and these are additionally distributed over different planes, like the top side, where you will definitely have a different temperature than on the bottom side.
So I think, that your 4 layer approach is not so good regarding thermal aspects, and also over-engineered, and too costly.
Keep things simple!
Regarding the resistors R1 (120 Ohm) , R4 / R5 (12k / 1k) , and R2 (70k), I arranged them around the LTZ1000, so that the lowest resistor value is closest to the LTZ, providing lowest parasitic track resistance. The influence on the T.C. of the 120 Oh resistor should be quite low.
I think, that's the optimum way, and you should again avoid additional layers.
Question 2: I had two ideas for the thermal treatment of R1 through R5. Either include those resistors inside of the foam which insulates the LTZ1000, effectively creating a tiny oven, or do your best to totally isolate them from the heat of the LTZ1000. I'm not sure which is the better approach, and I've attached sketches of both approaches. Keeping them in the oven would raise the temperature of the resistors, which isn't ideal if the the flat spot on their tempco curve is near room temperature (like with Vishay foils), but they would effectively be in a (pseudo) temperature-regulated environment, so maybe that doesn't matter so much?
The thermal isolation idea I have in mind is to laser-cut some rings of EVA foam (marked on the board with silk-screened zones). The inner ring would be a "hat" with a lid which isolates the LTZ1000. Then there would be an air gap (with a few ventilation holes in the board), followed by an outer ring of foam, which would be an open-topped column, and the inside face would be lined with a thermal reflector (aluminum or copper foil). The idea would be to insulate the LTZ1000 (reducing its total heat output via copper trace conduction, convection, and radiation), then have a "chimney" which creates a thermally isolated zone -- thermal radiation is bounced / absorbed by the outer foam ring, and convected away before it can reach R1 - R5. Thoughts?
Additional notes:
- I've used a 4-layer design, where the outer layers form an EMI shield, joined by via stitching.
- The grey box outline surrounding the board indicates the inner dimensions of a Hammond 1590B diecast case.
I would love to get any feedback on this layout. I'm reaching into (personally) unexplored territory with this board layout, so if there things which strike you as obviously wrong, I probably don't see them, so please point them out!
edit: "EVA foam", not "EPA foam"
edit2: Hmm, perhaps the convection holes around the foam are hurting more than helping? They would cool off the LTZ, forcing it to draw more power and just raise the temperature inside of the 1590B enclosure?
That's all too complicated and over-engineered, again!
I have enclosed the PCB inside a styrofoam box, and omitted the Styrofoam cap on top of the LTZ1000.
This box suppresses any air draught from outside, and lets the whole interior warm up to about 7°C above ambient temperature.
So a certain amount of heat is flowing through this enclosure, to guarantee stability of the oven regulator, but reduces also the oven power for the non-A version.
That's about 16mA @ 12V, 22°C
It was possible to reduce the overall T.C. to near zero by the nominal 400k resistor (R10), so I would not waste any thoughts about an additional oven for the resistors, or a convoluted isolation.
Same goes for the ground plane layer, for EMC suppression, that's also not necessary.
As you have a pure DC application, such a layer makes no sense at all, as the EMC disturbance comes from outside (mains, switch mode PSU, etc.)
Therefore, a simple tuner box all around the PCB is much more effective, as all of my measurements demonstrate. (I.e. not a single glitch anymore, during nearly 100h of measurement)
My approach delivers very good results, like more complicated ones (e.g. from TiN) obviously do also.
You might go ahead with your design, but you'll never get better results, as these existing designs are optimized already.
And I don't see any idea or ansatz in your proposal, why / how this would give any better results.
Frank