C3g Aikido Phono

[Andrew]

No, reason not to make the tracks thicker too, or even create blocks of voltage.

[simon]

Okay here's the C3g first stage with all tracks now 3mm wide (except where I've had to make them a touch thinner for access) and I've dobbed in a number of 1mm dia vias. There looks to be a lot of space on the pcb viewed like this, but there really isn't at real size!

Full ground place on the bottom, mostly full ground plane on the top except for the bottom right corner with is a HT/VCC plane.
.

C3g with vias render.png (114.76 KiB) Viewed 3628 times

[Andrew]

I would increase the gaps a bit now between the tracks and the fill ins.

[simon]

I'm glad you mentioned this, I've left the settings as default but I have been wondering whether there was more chance if capacitive coupling with larger tracks and planes. But I couldn't work out how that might affect the charge adversely. From a "feel" perspective a larger gap seems better to me though.

[Nick]

I would start with the nets being set for current and voltage requirements. After that you know that whatever you do is safe. In terms of current make sure vias or holes are big enough.

[Nick]

Also at the frequency we are working at capacitance is unlikely to be that much a problem. If needed surround traces with guards.

[simon]

Currents are small, heaters aside, and I had the signal nets 1mm wide which would be more than sufficient. I guess longer nets may have some resistance and wider traces would minimise this.

The heater nets were/are 3mm and fairly short.

As the currents are so small why is the size of the vias important? I can't work out why.

[Max N]

I’m learning a lot from this thread, and realising that my own pcbs could be improved a lot.
So, I will attempt to answer the question to check my own understanding, if that’s ok.

Thinking about impedance, going from low impedance to higher, at one end of the scale we have a block of copper, then a thick copper plate, then a thin copper plate, then a short thick wire, then a long thin wire. If we have a pcb with ground planes on either side, then increasing the number and size of the vias connecting them will decrease the impedance between them, in the same way that a thick copper wire has lower impedance than a thin copper wire?

[Max N]

I’m also guessing that these effects become more measurable and more significant as frequency goes up.
I’ve been battling a high frequency oscillation and/or radio pick up on the current project. I have lots of long wires……
I know that’s a long way from vias, but…

[Nick]

As the currents are so small why is the size of the vias important? I can't work out why.

They probably are not, its just you said they would not be as big as shown, I just said they could be not that they should be. There are probably some papers out there about vias and impedance.

[simon]

Ah okay, I'd got the wrong end of the stick. I did have a read about vias but much was about thermal management. I'll have another look later.

[Nick]

Yep it's common to link them from behind a heat producing part to give extra area for dissapation.

[simon]

Further reading about voltage and clearance was an interesting rabbit hole - clearance, creepage and dendritic growth. Also that >15V is considered high voltage . This page was helpful:
https://resources.altium.com/p/pcb-trac ... gh-voltage

FR-4 has a voltage breakdown of 20kV/mm, so a 1.6mm thick board is good for over 30kV. No problem there with an HT of 250V.

IPC-2221 seems to be a reasonable standard to use for high voltage, this is table 6.1 from it courtesy of another Altium page:
https://resources.altium.com/p/using-an ... age-design
.

IPC2221B voltage clearances.png (216.28 KiB) Viewed 3452 times

I'm guessing that B1 internal conductors are the traces beneath soldermask, and B2 are exposed solder pads. In which case the nets should be a minimum of 0.2mm apart and the exposed pads 1.25mm.

Using an online trace width calculator, for 20mA the minimum width is 0.0013mm with a voltage drop of 0.43V, based on an ambient temperature of 20C (not bloody likely this winter!), a temp rise of 50C, track length of 50mm, and 1oz board.

370+20mA for the C3g heater requires 0.080mm width with a voltage drop of 0.14V. E88CC heaters are 300mA.

A 1mm wide track has a current capacity of 2.5A with insignificant voltage drop.

So as long as my assumptions are sound the physical requirements are fairly skinny.

[Nick]

All good except that I think b1 means for a 3 or more later board and the traces on the internal layers

[simon]

Cool. I'll make them larger than the minimum anyway.