When importing a netlist to pcbnew, I get what appears to be a random placement. While the schematic placement is usually not a final placement for layout, it’s surely better than random.
For example, say I have a schematic like this (click to enlarge). The leds are annotated D1-8 down the first column.
This is the placement that comes out of netlist read. I don’t see a pattern.

If I run this script from my github, I’ll get this:

Not final, but it’s a sane starting point.
This short two minute video demonstrates. Not much to show, really:
 

How does it work? Pretty simple, actually. I parse the sch file for its device locations 1 and apply them to the layout. Most of it has been covered in my previous posts, but there are a couple of new things.

Where’s the schematic?

kicad has some infrastructure, called kiway, to pass information between applications. I suspect one could ask for a schematic file path there. I found it easy enough to ask pcbnew for the path to the current board and simply change the file extension.
[code]
import pcbnew
board = pcbnew.GetBoard()
board_path = board.GetFileName()
sch_path = board_path.replace(“.kicad_pcb”, “.sch”)
[/code]

Getting location/transform from the sch

components look like this in the sch files:
[code]
$Comp
L Device:LED D49
U 1 1 5A3B7115
P 6650 1500
F 0 “D49” H 6641 1716 50 0000 C CNN
F 1 “LED” H 6641 1625 50 0000 C CNN
F 2 “Miles:LED_5730” H 6650 1500 50 0001 C CNN
F 3 “~” H 6650 1500 50 0001 C CNN
1 6650 1500
1 0 0 -1
$EndComp
[/code]
I found a bit of documentation on the format on this website, but it’s not complicated. The things we need are:

• field 3 – “F 3” for the footprint name and location
• transform – “1 0 0 -1”. At first glance, this might seem a goofy way to represent it, but it’s just a matrix to multiply a point by.
• I also look at $Comp and $EndComp to ensure I’m not parsing locations from wire segments.

That’s it, really. Just have to remember that eeschema stores coordinates in thousandths of an inch and pcbnew uses millionths of a mm.