Can anyone give me some advice on task ordering? I’ve looked at the manual but it’s not obvious what I need to do.
Basically what I would like to know is what order to complete the following tasks:
a. Add Edge.Cuts
b. Create/Fill bottom layer ground plane zone
c. Create/Fill top layer ground plane zone
d. Export .dsn file to freerouter and import .ses file into pcbnew
e. Manually add via stitching to connect isolated areas of ground plane, refill ground planes, and add more vias until all areas are filled.
Will the order I’ve listed above work best, or is there a better task sequence? Have I missed out any tasks?
Lastly, should my Edge.Cuts be the same outline as the edge of my ground plane zones?
The answer to the order-of-operations questions is a waffling, non-committed, “It depends.”
The answer to your last question is more definite.
There are two factors to consider here. First, your board fabricator will require a minimum “setback” distance from the Edge.Cut line (i.e., the edge of the board) to any copper feature (trace, zone, pad, etc). The required distance varies from one vendor to another, and board-edge setback is typically greater than the required copper-to-copper clearance. (That’s because copper features can be optically plotted and etched more accurately than the mechanical milling operation that creates the outline.) Going from memory, setback requirements currently range from 10 mils (0.25mm) to 50 mils (1.25mm). (An assembler using automated pick-and-place machines may also have a board-edge setback requirement for components, different from the board fabricator’s requirement.)
Second, Kicad’s “Fill” algorithm treats an Edge.Cut line like a trace. When you fill the zone KiCAD usually does an excellent job of following the edge cut, minus the “Clearance” parameter set for that zone. (At least this is true when the edge cut is a completely closed polygon.) If the zone outline wobbles a little around the edge cut line - or even cuts across concave sections of the edge cut - the filling algorithm almost always follows the edge cut, minus the “Clearance” value set in the zone’s “Properties”. See atch image.
So it is safe to define a ground plane zone right up to the Edge.Cut line - or even outside the line - as long as the zone defines its Clearance at least as large as the required board-edge setback. If the zone’s Clearance parameter is less than the required setback, the ground plane zone will need to be defined INSIDE the Edge.Cut lines.
As for your order-of-operations question:
If the board outline has specific mechanical constraints - e.g., it must fit a particular enclosure, switches or connectors must be at specified locations, etc - the Edge.Cuts would probably be the first thing defined in KiCAD. If the outline requirements are indefinite - e.g., “Try to keep it under 4” X 7" . . . " - the Edge.Cuts may be the LAST thing you define. You’d simply lay out the board in a way that seems most reasonable, then draw a rectangle around the circuit and call it the Edge.Cut.
I may not define the fill zones until after the layout starts to take shape. As I work with the layout I will typically Fill and Un-Fill a zone several times as I visualize how traces pass through, or around, the zone. KiCAD makes it extremely easy to Fill or Un-Fill a zone, so filling the zones can be done at any time. In fact, the DRC tool will automagically refill all zones (without mentioning it to you).
I don’t use the autorouter in KiCAD, nor any other PCB layout program I’ve used.
I add vias as I work with component groups or zones, rather than saving vias for a last step.
Probably the most significant - and time-consuming - part of board layout is placing components. When designing from-scratch I first group components that seem to naturally “belong together” - the LED with its current limiting resistor; the 3-terminal regulator with its input and output capacitors; the opamp with its associated passive components; etc. Then I start to arrange these groups in an approximate pattern, in the manner I visualize they will land on the board. This might be based on signal flow, or possibly based on where connectors and switches are located, or where there seems to be area available on the board.
I typically start the board layout by placing and connecting one of these groups, then add others. Experience and intuition tell me which group is the most critical, or the most difficult to lay out, and that is where I start.
