# How can I better label my PCB?

I am working on a Teensy 2.0 clone for general learning in circuit design. The autorouter of CircuitMaker was able to route my board. Now I just have to clean up the aesthetics. I am trying to figure out what I should do with the labels of the components.

The board is small enough that there isn't much room to put the text next to the component.

I thought of removing the labels entirely, but I don't want to be looking up for the location when I populate the PCB.

I also thought of putting the label on the bottom, but I am not sure if that's useful at all for all my SMD components.

• I know this is an exciting time, when you get your first board out the door, but I recommend you pour through this site looking and reading any anything that involves a pcb tag. You might be able to get away with your board this time, but next time, you might not be so lucky. It's a good opportunity to learn and get better :) – efox29 Aug 14 '15 at 3:39
• Thanks for comment. Yes I guess there is no easy answer for this. Only patience and hard work. I will do some reading first! – Adam Lee Aug 14 '15 at 3:43
• I'm not sure that your layout of the crystal is good. If you do a search for PCB crystal, you'll find some insights. – Nick Alexeev Aug 14 '15 at 5:25
• Hi Nick, I searched for PCB crystal, and found this design guideline written by Atmel - atmel.com/Images/doc8128.pdf. – Adam Lee Aug 14 '15 at 6:05
• One thing that jumps out is that I should not run a trace directly underneath the crystal. Thanks for letting me know! – Adam Lee Aug 14 '15 at 6:06

As said in the comments, the routing of the crystal could be improved.

And I'm not happy about the power distribution. The 5V from USB (upper pin) is directly connected to a pin in the upper left of the IC. But there are some more pins of the IC connected to 5V, and the traces to them are long and branched. You should connect all 5V pins (and GND pins) using very short tracks, as it is usually also recommended by the datasheet. May be, your tracks don't cause problems on that PCB. But if you observe some strange problems with your IC, these power tracks may be the reason, though it will be hard to identify them as the definite reason.

So, even for a small, simple boards, follow guidelines to prevent problems and ... get practice!

And also: Try to route your board by hand. This allows to move parts around and find better positions for them. The resulting layout usually has a better design, though it takes time to route by hand.

Another point: What package are C1 and C2? If you solder by hand, 1206 could still be soldered by a solder iron with standard tip / thicker solder wire, if you have nothing else. For 0805 you should already have a thin solder wire and solder tip. 0603 is tiny and you need two really steady hands and some practice.

Coming back to your initial question:

• Silk screens (that white paint on PCBs) don't have a high resolution, OSHpark speaks about 200dpi. Also, you want to be able to read the labels easily. So, don't make them too small / thin. I would say, the height should be not less than 25mil, which is about the diameter of the pads of the three connectors at the border.
• In the past, it was said that you should use fixed-width vector fonts which could be drawn by a photo plotter, not that smooth fonts. This may be outdated as today, any shape can be produced. However, those bulky fonts offer a high readability.
• Silk screen is clipped to the solder stop mask, i.e. it's only printed onto stop mask, never onto metal. If you don't definitely know that your vias will be covered by the stop mask, don't place labels on vias. E.g. your label "Y1" would be clipped.
• If there is not much space as for your R2 R1 C7, shift them e.g. down and keep their relative position. (see the other answer)
• Of course, don't place labels under a part (J1, SW1) and make it unambiguous to which part a label belongs.

Another hint: Print your board to paper scaled 1:1. This often shows you size-related problems you aren't aware of when looking at the screen. You may need to find out how to hide/unhide layers, e.g. you should print only pads, vias, names (where the labels are) and stop mask of the top layer.

• 1. Shorter GND and VCC traces 2. Better routing around the crystal and 5V 3. Make sure to use font bigger than 25mil 4. Check for clipped labels. 5. Use relative positions for labels away from the part 6. Use better names. No J1, SW1 etc... 7. Print a 1:1 mockup. All points taken to heart. Much appreciated! – Adam Lee Aug 15 '15 at 22:41

You can use the unused area on the PCB something similar to the below examples:

Avoid to place the component names on top of a solder pad or any hole as they will not appear on the actual PCB.

You will not have any surprises on the silkscreen if you use the vector font.

Make sure to learn the minimum font height and thickness requirements from the production house.

• Thanks. I will make sure I use a vector font and check with OSHPark's design rule on silkscreen. – Adam Lee Aug 15 '15 at 22:30