Beagleboard:PCB Design Guide

The rules below are provided publicly with the intention of helping basic PCB designs to be cost-effective, manufacturer-friendly and user-friendly. These rules are made as generic as possible and DO NOT guarantee your design will work. They also DO NOT reflect our manufacturing capability in any way.

PCB Design

Fabrication

• Always keep your board size to a minimum. Larger boards cost more.
• Always keep standard board shapes like rectangles or squares if shape is not important for your PCB. Non-standard PCB shape may increase the fab cost.
• Avoid internal cutouts if they are not required. Internal cutouts will introduce more cost at fab shop.
• Go with 2 or 4 layers for simple design. Only go higher if required by your design.
• Standard PCBs have 0.062" thickness and are made of FR4 material. Use these unless you have a different reason.

Footprint

• Each LED needs to be labeled with its function. This will be useful when using and troubleshooting. Examples: Power, User, CPU Activity, etc.
• Each button/switch needs to be labeled with its function. Sometimes it is useful to label the switch state as well. Examples: Power, Reset, Boot, etc.
• Each connector/header needs to be labeled with its function even for connectors with obvious functionalities. Examples: HDMI, Ethernet, Expansion, Serial, Input, etc.
• Pin 1 of each header needs to have a square pad. This is standard and will be helpful in assembly and troubleshooting.
• Include any information that you think can help manufacturing, using, or troubleshooting your board. Examples:
  • For any part that has polarity, ensure the correct orientation is clear on its footprint. Examples: LED and diode require diode symbol markings; polarized capacitor and batteries require positive marking.
  • It is very helpful to label pin numbers in intervals especially for connectors/headers with high number of positions. It will save some time from counting all the pins. Examples: 5, 10, 15.
  • Adding signal name for each pin can be helpful if space allows and the number of position of that connector/header is not too high.
  • Other parts (i.e. ICs) may also need its pin 1 to be labeled.
  • Polarity markings should be visible even after the parts are mounted for inspecting purposes.
• Use standard reference designators for standard parts. See below for common designators:

Connectors/Ports	P1, P2, etc
Headers	J1, J2, etc
ICs	U1, U2, etc
Switches/Buttons	SW1, SW2, S1, S2, etc
LEDs	D1, D2, etc

Layout

• Avoid using trace width that is smaller than 10 mils.
• General power traces need to be at least 20 mils in width. You can use the chart below for Power Trace Width vs Amp

Power Trace Current vs Trace Width For 1oz Copper
Temp Rise	10 C	20 C	30 C
Width (mil)	Max Current (A)
10	1	1.2	1.5
15	1.2	1.3	1.6
20	1.3	1.7	2.4
25	1.7	2.2	2.8
30	1.9	2.5	3.2

• Keep a minimum of 10 mils between traces.
• Keep a minimum of 10 mils from copper to PCB edge for outer layers and 15 mils for inner layers.
• It is recommended to add ground pour especially for two layer boards. It usually makes it easier for routing. It can also reduce electrical noise and provide additional heat sinking.
• Minimize the number of vias. Avoid using blind vias or buried vias as they will introduce much more cost to your PCB.
• Add useful information to the board as silkscreen. Examples: it is useful to add voltage limits to an input voltage connector (i.e. 2.5V-5V) to avoid connecting wrong voltage to the board.

Assembly

• If possible put all parts or at least through-hole parts on one side of the PCB. This will reduce the assembly cost
• Add fiducials to your board. Fiducials are used by pick-and-place machine to accurately locate the circuit pattern.
• Use 1mm diameter fiducials with good contrast. Use fiducials on both sides if both have SMT parts.
• It is recommended to use three fiducials. Place them as far apart as possible near the corners.