I have been working on this layout. Lack of my training, my layout looks amateurish. Can I please get some general direction/tips on improving this design?
Some details:
OK, here are my tips
0) As has been noted, do not place vias within SMT pads.
1) Start with ground and power. Ground is the most important single entity on your board. The higher your signal frequencies the more important a ground plane is. This means that USB (480 MHz) is a real stressor and Ethernet (100 MHz) is only marginally better. Power planes are nice but not as important. Make all power traces as thick as you can, and provide decoupling capacitors (0.1 uF ceramics are a good default value) as close to the ICs as possible. In general, try for one decoupling capacitor per power pin. The consequences of inadequate ground and power routing/decoupling can be bizarre beyond belief. If your voltage regulators are located off the board, include at least one larger decoupling capacitor per voltage, 10 uF to 100 uF is a good start. For preference, tantalum or MLCC. Avoid aluminum electrolytics in digital applications - they tend to have lousy high-frequency characteristics.
2) Only after you have a good solid ground plane established should you start running signal traces. Give first priority to high speed and analog signals. Signals like audio need some care to keep them away from digital lines as much as possible: the human ear can detect distortions in sound in a very sensitive manner.
3) Be extremely wary of thinking you can scrimp on layers to save money, especially for either high-frequency or mixed analog/digital boards. USB or Ethernet counts as high frequency.
4) Put reference designators on every part.
5) Learn how to design controlled-impedance lines, both single and differential.
6) Unless you will be soldering parts on the board by hand, avoid placing parts on both sides. This will increase assembly costs substantially.
Other things like keeping reference designators to a single orientation and adding diode polarity symbols next to the patterns are very helpful for later troubleshooting.
The input and output capacitors for the voltage regulators are often required to be very close to the regulator pins for stability, (to verify this consult the spec sheet for the part).
If you are hand soldering smt parts then keep adequate spacing between parts so that you don't create shorts or over heat parts, (for example: C2-D1, R6-DS2).
The traces to the voltage regulators should be thicker, especially to the GND pins, to provide a bit of heat sinking, (refer to the spec sheet for examples). http://www.ti.com/lit/ds/symlink/lp2985-n.pdf
General High Speed layout guidelines (USB 2.0) will give you some idea. Below are some ideas from an applications document published by Texas Instruments, it is highly worthwhile to spend some time reading this or a similar document.
From: "High-Speed Interface Layout Guidelines" -SPRAAR7E–August 2014–Revised July 2015
1) High Speed signals should be routed over a solid ground plane (Not void or Power.)
2) Use serpentine routing to match interpair lengths of high speed signals (such as the USB differential pair.)
3) To minimize crosstalk in high-speed interface implementations, the spacing between the signal pairs must be a minimum of 5 times the width of the trace
4) Increasing the via anti-pad diameter reduces the capacitive effects of the via and the overall insertion loss. Ensure that anti-pad diameter for vias on any high-speed signal are as large as possible (30 mils provides significant benefits without imposing undue implementation hardship).
