[jrblasde]

I should also make two more comments. First, the diameter of this PCB is 1.45", to match the diameter of the multi-section capacitor I am replacing. The QC connectors I am using for the twist lock connectors are positioned exactly where they will pass through the cutouts in the chassis. And second, all clearances and creepage distances are in excess ofthe 3mm design constraint. Hence why there are no cutouts or notches in the PCB. I believe the smallest distance measured was 5 mm.

[morzh]

With 450V on separate, especially the opposite layers you simply do not have to worry about breakdown. Not with 62 mils, not with 31 mil....

Looks good.
I would beef up the caps' pads sizes. Also, if you have tall caps, and you also have the tabs that could be twisted, using teardrops makes sense.

[jrblasde]

What are teardrops? Is that a style of capacitor?

[morzh]

No. Teardrops is a style of a trace entry into a pad.

https://www.pcbway.com/blog/PCB_Basic_In...166ec.html

[jrblasde]

Okay, yes. I’m familiar with the concept but knew it as a fillet. Let me make the modifications. You raise a good idea.

[morzh]

Yes, fillet is another name for teardrops, or, rather, one of the type of it. The most popular one.
Teardrops will not be generated if the trace enters into the pad not radially, or if the entry segment is short.
Most CADs will generate them automatically if the option is enabled.

[jrblasde]

Here we are. Not too difficult at all!

   

[morzh]

BTA, the trick to add a teardrop to a pad that is not directly on the way of your 45 degree trace (your square pads) is to break the trace in the middle and zig-zag to another 45 degree trace that noaw has the target pad on its way.
(Or, in case you do not mind using non-45 degree angles, just to go to "any angle" routing mode and draw a direct trace between the two pads).

[jrblasde]

Here we are, I was able to relocate the solder lug connectors to be precisely 45 degrees from the respective terminal on each capacitor. Clearances are still at 5mm, which exceeds the 3mm minimum.

   

[morzh]

It always looks more colorful in CAD than on the PCB

SInce I do not know the dimensions of your solder lugs/tabd, make sure they are not to close to the caps' barrels and will not rub against it.
Also, personally, with high voltages I try to run the traces (if they cross the aluminym can outline) on the opposite side to the one the caps are mounted on. I honestly do not know what the insulation property of that film that covers the caps.

[jrblasde]

Luckily my plan is for those solder lugs to be on the underside of the PCB, whereas the capacitors will be on the top side. Even so, I know that the through-hole connector will protrude just a bit through the top. I measured, and there should be 3.4mm of clearance between the connector and the edge of the capacitor. Great consideration!

As for the comment about the high voltage traces, I hadn't considered this. You clearly have a lot of experience designing PCBs. I welcome all of these comments! Lets fix this by placing all traces on the bottom layer. All traces will be on the opposite side of the PCB compared to the capacitors. The traces connecting to the negative contacts will be equipotential with the chassis, so it wouldn't matter if the solder mask were scraped and the trace contacted the chassis. Additionally, the two positive contacts could not possibly touch the chassis as they are located in the area of the cutout in the chassis.

   

[morzh]

Yep.

It always help to put some sort of keepout outline, which is not necessarily the "keepout" keepout, but just some outline denoting the area where certain things should not enter.
Could be on a mechanical layer, so it does not show up in the artwork.
In this case it's the cutout you've mentioned.
It immediately visualizes the relation of the cutout and the traces/pads/outlines etc.