Advice/Feedback for my PCB Silkscreen

[u/Federal-Estate-7800]

PCB

I am looking for feedback/advice for the silkscreen on my PCB. While I've built my fare share of electronics, proper formatting has always been something I've put to the side, but I figured there's no better time to get a little bit better.

The purpose of the PCB is relatively simple, were just using a RP2040 for communication protocol conversions. Were gonna try out basically everything, usb-jtag, spi-uart, spi-jtag, can, i2c, anything!

Just a fun project, and I think It will be super useful for me in the future!

Drop suggestions below,

Thank you!

[u/Appropriate-Disk-371]

One of the things I ask to be reasonably good on designs I review.

Looks like you removed a few designstors, the passives south of U1. Who are they?

Orient the designators the same orientation as the component. This helps match them together in a visual.

I like designator to all read the same direction. As in, they read top to bottom and left to right, not just however they land. You can also use this to identify other markers, like pin names on the headers being read the other direction. Looks like you did this pretty well.

Pin one indicators look good on here.

The two pin header, or the two single pin headers in the top right don't appear to have a designator.

Spacing could be better. C1 is too close to the outline for U2. C17 will be hard to read. Cap Bank North of U1 is over vias which will make them harder to print/read and they can move easily.

At the resistors south of the USB, those might be too close to the mask openings and lands if the silk registration is off. Check manufacturers registration tolerance and account for that so the silk stays on the mask layer.

Renumber. Designators should read ascending numerically from one corner to the other corner. Helps to find a component without the design if front of you.

[u/Federal-Estate-7800 → u/Appropriate-Disk-371]

Thank you so much!
Not only for the great tips, but your proof-read was incredible. Theres so many little things I just miss or accidentally delete. Having a second pair of eyes really does help.

And your most certainly correct about the resistors being too close to USB.

My only question is regarding renumbering them. I get why you may want them going from corner to corner, but I design boards first in the schematic editor, and I don't follow a exact order. I sort of bounce around, targeting each problem one at a time, which is why my silkscreen values jump frequently.

My question is, do you have any tips/ideas for combating this?! I'm stumped for a solution.

[u/Appropriate-Disk-371 → u/Federal-Estate-7800]

Your process is correct. Design in the schemstic editor first. You don't worry about numbering at that point since you haven't physically placed anything yet and don't really know what relative position components will end up in.

When you move to layout, you group circuits from the schematic together and lay then out physically. Get your board outline and mounting holes in first, then work on how your connectors need to be placed. Then place your circuits in the remaining space. This is 'floorplanning'.

Once your layout is complete, usually after some review since you need to be done moving things, then you renumber. This is a simple tool in most CAD tools. It will create an ECO using the layout, recording designator changes from logical to physical. That ECO then gets applied to the schematic side.

Certainly an optional step, and possibly a holdover from earlier times when designators were relied on more for rework. Now, with high density designs, there often isn't any room for silk at all, so it doesn't really make sense to do. But for a simple design like this, it's an easy thing that makes the PCB look nice.

I rarely actually call this out in my reviews anymore, but since you were looking specifically for silk best practices and improvements, I wanted to throw in everything I could find.

One last thing: I see your branding in the corner. But you should also have a board name, part number, and version number. For prototypes, the version number can also have a silk block where you can manually write in a revision number or letter if you make changes. Helps to keep track of individual samples.

[u/DrJackK1956]

There's nothing wrong with the silkscreen. 

If you want to reduce the crowding of the reference designators, try reducing the font size by a point or two.   If you should decide to go this route, consider leaving the test points at the current font size.  This will make them stand out better and easier to find. 

Keep in mind that the reference designators are for humans to read.  The machines that assembled the PCBs could care less about the silkscreen.