Routing a PCB with no Netlist in Altium

Question

I want to route some tracks directly in the PCB file in Altium, So there is still no Netlist available.

So what rule/rules should I change to route pads directly, without applying the clearance rule between the track and the pad for the newly created nets?

Answer 1

Disable Online DRC.
Preferences -> PCB Editor -> General -> Editing Options -> Online DRC = unchecked.

You should really create a schematic, even if there's only two parts on your board. In the time it took to write this question, you could have made your schematic. It's amazing how a seemingly simple project can go awry. By creating a schematic, you don't need to compromise design rules which are there to help you create a board without spacing and wiring errors. Plus, when you revisit this project in a year, a schematic will make more sense than a routed PCB.

Answer 2

This is a couple of years old, but I came across this when searching for the same answer, I didn't find one, but I did come across a way of doing it that doesn't involve changing settings or creating rules that are in general not good.

1. place a trace from the first connection to somewhere between the connections.
2. place a trace from the second connection to somewhere between the connections.
3. drag the copper from one connection onto the other.

Answer 3

There are two ways:

1. Use Place - Line (or other shapes as you like) to draw arbitrary copper. It will be placed with Net = 'No Net'. Note that primitives will pick up nets when dragged or pasted onto other net objects (pads, existing traces, etc.), and will yield a shorted unconnected copper violation (with normal settings).

2. Design / Nets / Edit Nets, and add new custom nets. You can construct the netlist manually this way (or edit a plaintext netlist and import it, just as well). Assign pads to nets in the dialog, or via their Properties. Route as usual; design checks will be meaningful.

3. Add a schematic to the design, use generic symbols (headers say) if you have to, match up footprints and assign pins (you may need to create a PcbLib from the PcbDoc to be able to assign footprints), and continue as usual.

Note, if using schematic, once a synchonizable design is prepared, in PCB check Project / Component Links, and match up respective symbols/designators/footprints. This avoids renaming, swapping or deleting and re-adding that may occur with unsynchronized parts (part IDs not matched).