Scope Clock - HF transformer dirving circuit and PCB layout evaluation

[WawaPL]

Hi everyone,

I wanted to build scope clock for a long time now and I have managed to create this PCB by borrowing bits and pieces from another people's clocks. Right now I am stuck at PCB making. Basicaly I am unsure if layout is optimal. What is more concerning for me is that I am unsure if I made correct circuitry for driving HF transformer. This is my first time using UC3524 as driver. If someone could take a look, I would be really gratefull.

(Sorry for messy transformer wiring on schematic, I made mistake while creating a model for it)

[David Forbes]

Hi. I am certain that my scope clock designs were some of your inspiration. However, it is impossible to see what your circuit looks like because the schematic diagram does not show the transformer windings, and none of the transistors are shown as transistor symbols. Also none of the chips are labeled with part numbers. 

I recommend that you take some time to draw the schematic clearly. Then design a PC board with only the power supply and CRT portions to test those first, before trying to add the computer to it. 

It will probably take months for you to get it working well. At least it did for me. I had to learn a lot about power supplies and transformer windings and so forth. 

[gregebert]

I've been doing my own PCB designs for the past 10+ years, and the main areas to look out for are:

1. Trace-width for higher currents. There are online calculators for this, but they seem to undersize the conductors based on my gut feeling so I use them as a reference and make mine stay a lot fatter. The most I put on any trace is 2 amps, and for that I use conductors 0.25 inches wide. Be aware that feedthrus have much higher resistance, so use redundant feedthrus when possible. I do the complete power-routing first, before any signals are routed.

2. Spacing for higher voltages. Again, look for online calculators/table for creepage and clearance. There are various factors that affect spacing including pollution levels. I always pick the most conservative rules I can find. Spacing for 500V or less is pretty small, around 2mm.

3. Trace-lengths at higher frequencies. Traces are additional inductance and resistance, so if you have frequencies in the Mhz region or higher, you need to be careful about routing these signals. Generally best to keep them as short as possible and minimize bends and feedthrus. Often you will need to waste some PCB area for optimum component placement to minimize the lengths of critical signals. These should be routed after power/gnd is done and before the other signals.

4. Noise and ground loops. I dont do any precision analog designs, so I cant offer much help here, but there are a lot of good online articles on how to avoid ground loops and minimize noise coupling. I use a lot of bypass caps on my boards, and I've never had any problems with logic glitches. Generally, if you have a single power supply, it's best to run separate power and GND traces to the noiser/higher-current sections, then bring them together at 1 point.

On a recent project, I have a rather noisy DCDC converter, so I routed separate PCB traces for its power and GND, and the design works fine.

[Paolo Cravero]

Hello.

2. Spacing for higher voltages. Again, look for online calculators/table for creepage and clearance. There are various factors that affect spacing including pollution levels. I always pick the most conservative rules I can find. Spacing for 500V or less is pretty small, around 2mm.

@gregebert Have you noticed, or is it documented in some standard, an effect on the spacing with respect to the silkscreen color? I use each project to refine my board design skills by imposing new challenges to myself and I have little experience with PCBs at >150V levels. So far I have been lucky and never had to go for a second round of the same design, also considering that I usually build a couple of each circuit but get 5 PCBs from the fabhouse...

Anyway, on a Nixie design I had the feeling that the black silkscreen was "leaky" and the 180V on one line was pulling the one nearby. Is that possible, or I didn't respect the minimum spacing? I think I don't have that old KiCAD project anymore.

TIA

Paolo

[gregebert]

I've never heard of soldermask causing HV breakdown issues. If you have a blank board, you can try measuring leakage with a HV supply, and a sensitive current meter. For example, if you have a 200V (higher would be even better...) supply and a 50uA meter, you can easily see 1uA of leakage, which equates to 200Megohms. Note that using an ohmmeter wont necessarily give you the whole story, because the ohmmeter wont be testing at higher voltages where creepage effects kick-in.

I've done several boards with voltages ranging from 200V up to 2000V, and never had or suspected a creepage problem.

My biggest fears about HV wiring on PCBs are around the AC mains input (120 VAC in the US), especially the wiring leading up to the fuses on the PCB because shorts between those areas are not fuse-protected. Destructive energy requires voltage and current, so until one or both are limited, there is elevated risk. Since I use a power-entry module (IEC connector + switch + fuse) in my projects, it's a manageable risk because everything is sized to handle much more current than the fuse in the power-entry module. After I get the power thru a transformer, or a resistor, where the current is forced to be lower, I ease-up on the over-conservatism. For added protection, I use 2 fuses (1 for hot, 1 for neutral), a varistor to absorb surges, and a 0.01uF to absorb super-fast spikes that are too quick for the varistor.

[Terry S]

I've designed hundreds of boards and never had a problem with silkscreen or soldermask related to conductivity. I seriously doubt any reputable PCB manufacturer would use a mask or ink that would be the least bit conductive.

I will say most of my designs were sub 50 volts.

I never specified an ink manufacturer or specific brand, but I specified plenty of different specific solder masks. Ink was always left up to the supplier.