Help/advice/guidance translating schematics onto a pcb

[Cqwet Dbdfte]

Not sure how KiCAD does DRC (design rules check) but board houses like JLC has design rule setups for various programs, to make the board both manufacturable and (mostly) error free. (but not optimal).
You may see some faint lines around tracks and vias, do not put anything inside those.

 

[djmiggymigz]

Not sure how KiCAD does DRC (design rules check) but board houses like JLC has design rule setups for various programs, to make the board both manufacturable and (mostly) error free. (but not optimal).
You may see some faint lines around tracks and vias, do not put anything inside those.

Yupp, I found a github files that loaded all the JLC rules in and then double checked/edited the numbers myself in reference to JLC's website! Learned a good bit there too since I had to figure out what "annular width" is among most other parameters!

1) The -- acute angles -- that you see here in this image of your PCB-layout are also known as "acid traps"!!! These are a NO-NO!!!

View attachment 137093

What happens here is.....during the fabrication etching process, the acid that is used to etch the copper off of the laminate is caught inside these -- acute angles -- and ends up ever-so-slightly etching away the copper -- UNDERNEATH -- these angles. Over a period of time, the copper tracks at these points of your PCB may loosen and cause the PCB-track to actually pull-away from the laminate itself. What this means is.....you need to perform all of your track-routing to be be either at a 45-degree or a 90-degree angle.

In addition.....and, I am only assuming that this image may have been taken with the PCB at a slight angle, but.....this image shows that your component copper pad and your N/C Drill hole are -- NOT concentric -- meaning, they're not in perfect alignment with one another. In other words, the "white hole" and the "yellow pad" should be in perfect alignment (or, "concentric") with each other.

2) Your -- track-to-pad -- clearances are "WAY TOO CLOSE" than is necessary:

View attachment 137094 -- View attachment 137095 -- View attachment 137096
>> Don't be afraid to offer at least 15- to 20-mils of clearance between
your tracks and pads, especially on a layout as "loose" as this.

3) R8 is both placed and routed as a -- stub-route -- scenario:
View attachment 137097
View attachment 137098
>> The two upper-most yellow pads shown here are the component pads for R8 and the lower-left corner track that connects to another pad and then angles upwards to the upper-left at a 45-degree angle (also creating the "acute angle") is its same net connecting track. Since R8 is placed in the manner in which it is, technically.....it is -- NOT -- directly within the circuit's operation, but instead is "off-to-the-side", so to speak. While doing this may not much matter with a resistor, it -- DOES -- make quite a difference with capacitors!!! I have worked inside many engineering environments where the Electronics Engineers have literally shown me on their test equipment how the placing and routing of a component using a "stub-route" makes a difference in the circuit operation. And, this minute effect is additive as well. Meaning, the more components that are placed and routed using -- stub-routes -- the less the overall circuit behaves as it was designed to do!!!

However, while in your particular layout circumstance, it probably doesn't matter one hoot.....-- NOT -- placing and routing components in a --stub-route -- situation is a good habit to learn about and get into as you are learning the "PCB Design" ropes and techniques.

/

Yeesh thank you for such a detailed response and critique!! I didn't notice those acute angles at all. I have KiCad set to place tracks at 45/90 degrees but looks like 2 45's meeting caused that issue! Is this something that will still work just is not ideal? I fixed it in the design but I already ordered the pcb's using the design that you were referencing so unless its mission critical to fix that I may jusst try the existing boards out. (The jfets I bought arent cheap tho so I'd rather not risk frying them!)

Also, yeah I took these screenshots in KiCad's 3D model viewer which automatically displays the board from a perspective that shows the depth of the board.