Manual Track Route

[paulvdh]

First some small things I want to get out of the way:
Generating netlist files and importing in Pcbnew has been deprecated for three or more years. Try: Eeschema / Tools / Update PCB from Schematic [F8] instead. The result is very similar, but it’s much quicker and more convenient.
What KiCad version are you using? There are some differences in the behavior of different versions.

@teenix

I should now be able to draw any amount of traces on the board without KiCad caring where they go.

That works. Quite some time ago I experimented with first drawing a bunch of tracks, and then later connecting them with footprints.

Replicating Layout features manually with arrays & blocks [Tutorial]

I just made a little mini tutial on how I would use array and block functions to create copies of features in a repetitive design. By using copies and arrays a lot of tracks can be layed out quite fast this way if your schematic / PCB structure is suitable for it. For other, more advanced ways, scripts such as the “replicate layout” script are much more suitable. Using arrays and block moves is very intuitive and easy to learn and it seems a worthwhile technique to have in your toolbox. Makin…

Another post in which I experimented with mass copies of tracks, and connecting them to connectors later in the process:

Plugin for routing parallel tracks

I’ve experimented a bit more, and this is what I’ve found to work best in this particular case: First set the grid to the spacing you want, and then draw a single track with two of the 45 degree corners. The stubs should be long like in this screenshot: [image] Then use copy & paste to make a few of them. Here I copied it 4 times to make a total of 5: [image] During paste, you give each copy a gid offset of one grid size in both X and Y direction: [image] Then repeat. I took the block …

@teenix

Say I now want to connect a new trace to the first trace. KiCad does not want anything to do with the first and tries to route around it producing multiple bent traces where I don’t want them,

That is very likely the “walkaround mode” of the Interactive router, and is what der.ule mentioned.

Klick on: Pcbnew / Route / Interactive Router Settings, and then set the Mode to Highlight collisions

When you draw tracks in KiCad that are not connected to a pad, then the segments get assigned to “No Net”. If you set the interactive router into the Highlight collisions mode, then it should let you draw a track from a pad (so that new track is part of the same net as that pad) to connect to a track segment that is in the "No Net** part of the netlist.

I experimented (again) a bit with it. I can draw a track segment that connects a named net to a “No Net” track segment, but not from a “No Net” to a “Named Net” track.

If that does not work satisfactory, you can also turn on Options / Allow DRC Violations (der.ule put a red line through it, which is a bit unfortunate). If you combine these two settings, then KiCad lets you make any connection you like.