I'll have to find a demo copy and give Solidworks a try one day. I know it's a popular produce, perhaps the top in the field. About 10 years ago I bought a license for TurboCad 8 which is mostly a 2D drafting tool, and I've been using that so I'm proficient with it. They had some 3D features too but it was poor.
Here's the updated PCB. After switching the headers, I routed VUSB at the top of the board - any issue with routing close to edges? I did this to avoid cutting the ground plane under the JTAG traces.
I also VUSB to U6 very close to the USB data lines as an attempt to minimize the amount of ground plane splitting in that area but am unsure if having power close to data would cause any issues.
The VUSB near the top will be OK. I agree, routing it downward would split the ground plane too much again, so I also like it at the top and I would have done the same.
Traces near the edge, be it power or signal, are mostly frowned upon because it can cause EMI due to energy radiating out from the edges of the board. This occurs because the EM field is no longer fully contained within the dielectric of the board and can escape to free air more easily, as lines of flux wrap around the board edge and close underneath the board (close, as in opposite to open). With the EM field in two mediums (air and FR4) propagating down the board you get an antenna.
Even so, this is usually only going to be a problem at speeds above 100 MHz
[*] or so, and also with a ground plane beneath the signal trace for the EM field to return to. You don't have this, and your power trace is planar with your ground, so the EM field is different. You actually have a slot line radiator, but it's a poor radiator at your operating frequencies, a poor radiator at switching PSU frequencies, and the trace is not likely to have any high-speed transients on it anyways.
When thinking about any trace that is near the edge, you should think about what will that trace be used for and will there be periodic current demands that will cause high-frequency switching components to appear on the trace? Even if it's a low speed trace or in this case a power trace, it might have switching with fast edge rates above 100 MHz or so. Since this particular trace goes off-board via the header pin, you have to ask yourself where does it go from there, and will there be any high-frequency periodic current demands? If so, these will be possible sources of EM radiation.
The rule of thumb for traces near the edge is to make the edge of the trace at least as far from the edge of the board as the board is thick. So for a 1.6 mm thick board you want to keep the trace about 1.6 mm away from the edge. Some say 2x as far, but I think for a power trace which might have just 10's of millivolts of transient edges then the changing EM field is going to be weak anyways so keeping the power trace about 1.0 to 1.6 mm away from the edge should be fine. And as I said above, your EM field on that trace is not leaving via the edge anyways, as the trace is co-planar with the ground plane.
The board looks great!
Get it made ! not yet
![Smiley :)](https://www.eevblog.com/forum/Smileys/default/smiley.gif)
... I have a comment coming...
EDIT: change the cyan power trace to the green trace. This opens up the analog ground better to the analog inputs, and splits the plane better into the analog and digital regions. It keeps the analog return currents off the digital ground plane better with this change. It is still not a split ground plane, just careful routing of the split to keep analog currents on the analog side and digital currents on the digital side. After this, you can get it made
[*] There are published papers (
pdf) with experimental results showing edge-radiated near-field EM radiation at -50 dB for a 100 MHz signal when the signal trace is approx 2x the dielectric thickness away from the edge. It gets better with increased distance from the edge and worse with higher frequencies.