Looks like a good start!
The blocky through-hole thing in the middle needs a refdes.
Stitch *everything*.
You have two polygons on top and one on bottom flooding around things, leaving large slots in the pour (e.g., the trace from R2 to, whatever the big box thing is, pin 7?), or orphaning copper altogether (e.g., the section south of R5, or the sliver by U3).
Islands can be removed by setting the "remove copper under x" property on the polygon. Larger sections should be removed (by preventing copper pouring there, or modifying the polygon outline to exclude that area), modified (move the surrounding traces to shrink the area until it no longer forms, or grow the area until it is big enough to connect with surrounding copper or with vias), or stitched.
Stitching rules: I like to place via pairs every 500 mil or so along traces, and at the ends of peninsulas, or in the centroids of smaller overlapping regions.
Use closer spacing, or multiple vias, around high current or high dissipation areas.
Traces should be grouped (within reason; similar signals can be bused together, while high power signals for example should be kept well away), which follows from the island rule above.
Where traces intersect on opposite layers, use three or more vias to stitch across the intersection. Try to minimize overlapping area by making the traces cross at right angles. A 45 degree is fine too, but just try to minimize area. The underlying emphasis is, ensure that any given trace is never more than a little distance from the nearest grounded copper. This ensures a convenient and expected path for the image current, which keeps crosstalk and susceptibility to a minimum.
Vias produced by these rules can be grouped when convenient; think of the underlying element as the centroid of overlapping ground areas. If the overlapping region is small and it's more convenient to place one or a few vias there, rather than following the above definitions strictly, go for it!
Preferably, an island (not removed by the above rules) should be large enough that it can hold two or more vias (and therefore some current can flow through it, as a shield), or it should be excluded by the above rules. If it's still unavoidable, at least use one via, to ground it, to avoid floating copper.
All of these are illustrated in this example:
It's also a manufacturing tip to ensure even copper on both sides -- otherwise, warpage can result. It's not usually a big deal, but it's more important for two layer boards (that are more flexible) and very fine pitch components (especially QFNs, LGAs, etc.). Pouring ground (or whatever) over the entire board is an easy way to ensure that; with the added bonus that your electrical performance can be nearly as good as a 4 layer board, without the expense.
Tim
Home
Help
Search
Login
Register
