HV Controller PCB Review

[dawiggleman]

Overall, nice work so far and good initial layout. Couple notes:

• In future, do all work on branches so merge conflicts can be caught prior to pushing to main
• Do we need a battery protection circuit for the supplemental batteries? At least an undervoltage sense? Does the powerpath do that?
• Looks like the green violations remaining on the board are height constraints of your 3D bodies. Change this rule to a higher value or an actual constraint if we have one

Spread out these vias a little more if you can, otherwise you have thin paths for current to get to the middle vias

Are you aware the DCDC converter footprint does not have holes? Right now there are just exposed copper:

While you're at it, double check the hole spacing on this footprint. Need to get it right or the whole board is unusable.

[dawiggleman]

Fix reference designators everywhere to be readable and intuitive:

P10,P8,P7,P9 dont have holes either:

[dawiggleman]

Make this VRAW_12 trace as wide as the rest of the trace

Make connectors flush with edge of board:

Put board info in this space in silkscreen (Name, board title, revision, badgerloop logo, altium logo)

The diodes footprints you're using don't have polarity indicators on them. Add them for assembly:

Tbh your vias look pretty large. Check out my mppt board to see what hole/annular ring size I'm using. Then all can be changed at once by selecting one, then right click "select similar objects" and you edit dimensions there:

Secondary thoughts on these footprints. We could just use solder paste and put the board in an oven for assembly. It will save additional complexity of this footprint and cost of adding vias in pad.

[dawiggleman]

Minor detail but make these diodes even if you can:

Can probably hide silkscreen for mount holes:

Instead of making a right angle junction like this, just route from one pad to another, then route out from that second pad:

Get rid of this acute angle by routing to the left straight left out of the pad instead of at an angle:

Route straight out of the pad here:

On the traces coming out of the resistors here, have the trace come out as perpendicular to the hole as possible:

[dawiggleman]

Last note: We need to add a "board outline". I think the best way to do it is to draw a line around the edge of the board on mechanical layer 4. It's just the black line around the edge of the board. Here's how I did it in MPPT:

See "M4" in the Layer set manager:

[ryanbear22]

pushed with all changes added