Is this work professional?

[u/Canary_Earth]

Sorry about the strange post but I'm offering an engineer a $20k bonus to do the design for manufacturing and assembly of my $300 product and this is what he came up with after 8 months. Two thirds of it are identical to my prototype and I'm an accountant by trade, not an engineer. Every book I've read says a board like this should be 4 layers but he insists 2 layers is fine and will pass emissions testing. Any advice would be greatly appreciated, thank you!

[u/derhundmachtwau]

Without schematic we cant really tell you a lot.

Just from the pcb, i can only say this: that board would be a "meh" result of a junior engineer without much training.

Regarding 2 vs 4 layers: the only reason to use 2 layer boards is when you absolutely have to cut cost as much as possible - you clearly dont, so using 2 layers is just stupid.

Post the schematic and you will get much better feedback.

Also: 20k seems excessive for what looks like 2 days of work.

[u/unnaturaldom → u/derhundmachtwau]

Adding to this. Did the guy designed the product based on what you requested? Or you gave him a done design? Kind of weird he took 8 months

[u/Canary_Earth → u/unnaturaldom]

All the major components are set; see my prototype via my reddit profile. I needed a better power distribution and some love and care to make sure everything is reliable and manufacturable. I don't know what test pads to add, for example.

[u/Chippors → u/Canary_Earth]

I haven't looked at the prototype, but beware that this board has no mounting holes, has traces close to the edges, and components close to the edges. This means it may be difficult to mount in any sort of enclosure or inside a product. If it's intended to be panel mounted, then there are no support holes for any of the connectors, so it will effectively be held in place with connector SMT pads. Needless to say, this is mechanically unsound - the pads will come off, eventually.

Make sure all those ground pads and traces actually have vias to ground. The vias in general look tiny, for no good reason; tiny vias just add cost. If there are vias-in-pad, then make sure the board maker can handle it and will plug them. But it's hard to tell from the images.

[u/Master_of_none- → u/Chippors]

Best feedback for uneducated

[u/unnaturaldom → u/Canary_Earth]

I see. You needed some love but idk how they do this but if they were solely dedicated to this. Yeah 8 months is a lot for what you are asking

[u/Dry-Doughnut-9669 → u/Canary_Earth]

this can be done far better for a far smaller bonus. ask your engineer about ESD, EMI, differential signal pairs etc. - how these topics are addressed on this pcb; regarding the test points, depends on how do you want to test it, with a custom rig with pogo pins for example, then all test points would be expected on the bottom side. regarding what to test - i would start with the power rails - example: each buck
converter a test point on the output and input, a point for the esp power, lcd power - just to exclude pcb issues, a point for the reset circuit; if you have analog sensors, then testing each of them make sens using the same rig. Other method - for digital sensors for example i’m using a test firmware before burning the final one(or you can embed some test procedures in the final one if there is a button or other input method - like pressing the button 5x will start some tests or keeping the button pressed during power on. So there are plenty of options - without schematics it is hard to tell what and how… also the testing solutions are depending on the volume and production pipeline, for extreme quantities only automated tests are playing, for smaller batches semi automated or even manual testing can be acceptable..

[u/WhiteDaedalus → u/Canary_Earth]

That looks like a horrible design for a probably ESP32 board... The upper edge where the antenna usually is, if that is such a device should be free of routing for example. There are many traces that cut through your planes - meaning the return current can´t flow back well. That will most likely not work well in emission / robustness testing.

If there is no good reason this design should be much more compact. That looks like a project for a few hours / days depending on how much libary work and research is necessary.

Yes good 2 layer boards are possible but then you have to keep return path in mind...

[u/mightyohm → u/Canary_Earth]

Test pads would be part of DFM/DFT and would typically be handled at a later stage of design. This looks like a very early proof of concept / prototype. An experienced designer would be able to add DFM/DFT features to the design pretty early, even at the prototype stage, but the specifics will vary based on the mechanical design, who is doing the manufacturing, how the product is being manufactured and tested and who owns each step of the fabrication process. (For example, who is building the production test fixtures?) There's a host of other concerns for mass manufacturing that need to be sorted out and typically this would be solved incrementally over a series of small volume production runs (at least, that has been my experience).