From rLab

Gavin's KiCAD Tips:

  1. Before laying tracks I would check footprints. If you have the components to hand, import the netlist in pcbnew (it will dump all the footprints on top of each other - move them apart with the M key) and print them out on a piece of paper. This is particularly useful if you have surface mount components as you can simply lay them on top of the paper and visually check that they match. If you have through-hole components check hole sizes against data-sheets. If your holes are too small, it’s pretty much unrecoverable! Watch out for components with square pins as the holes need to be large enough to accommodate the diagonal (speaking from experience here:) ) Also, if you’ve designed your own footprints, make sure you have all the layers you need - I have had a board made with solder mask over pads before as KiCad does not automatically do the solder mask layer unless you tell it to. Also check that you have the right solder mask layer selected - it’s quite easy to design a footprint with pads on one side of the board, and solder mask pulled back on the other!
  2. Set your design rules before laying tracks- track widths, clearances, via diameters (annular rings) and via drill sizes. They vary from boardhouse to boardhouse - their websites will tell you what they can do (often expressed in non-SI ‘mils'). From memory (but check) PCBWay can handle the KiCad defaults, but Ragworm, for instance, have a larger minimum size for ‘dressed holes’. You may also have to think about track width if you’re using a lot of power - the internet can tell you. It’s a good idea to keep the track sizes small enough to thread between DIP pins if you can though. If you have added power flags to your power lines on your schematic, you have the option in KiCad of specifying different track widths for them and it will handle it automatically for you.
  3. A good place to start is to have a look at the rats nest as you lay the components out and try and minimise the number of crossed lines - sometimes simply rotating a component (R key) can give you a much better layout. I normally have two or three attempts at getting a layout right as I find that as I am routeing the tracks, I start to see better ways of setting the components out. The component placing and track routeing tools snap to the grid btw - which makes for a neat layout - but you may find that you have to change the grid resolution to thread some of the tracks.
  4. Pressing V key when routeing, places a via and switches the track to the other side of the board. Vias can take up a fair amount of space, so try and place them away from areas where you are going to be threading more tracks or you’ll quickly run out of room. One obvious space saving tip (given that vias take space) - if you’ve via’d a load of tracks under a single track, un-via them and via the single track under them instead.
  5. (double-?)Clicking whilst you’re routeing will fix the position of the route so far. Pressing Esc will drop the entire track (even if it still appears to be there until you zoom or pan). You can delete individual segments of tracks via the context menu.
  6. I don’t really have a routeing strategy - others may chip in with theirs - but if things are getting really tricky then one old-school approach is to put vertical traces on one side of the board, and horizontal on the other.
  7. If you’re going to have a ground-plane - apparently good practice - then try and keep the power lines on one side of the board, and your signal lines on the other - this will help you maintain a large contiguous plane. If you have a ground-plane, you will want to set the ground pads to have thermal relief rather than a solid connection else the components will be v hard to solder as the plane will draw all the heat out of the iron - I can show you how, but it’s a but hard to describe here.

well worth doing that paper printing thing for the TSSOP component and check that you;re comfortable that the pads are long enough for hand soldering. Long pads can come in handy as you can load the pad with solder and push it up to the pin when you’re first fixing the package in place.

acid traps. You want to avoid having acute angles on your tracks (check how you’re joining the pads) as apparently they can trap etching acid