Autoroute or not?

I think the placing of the parts is your biggest problem.

Look at U6 and the U13, U14, and U15.

U6 has multiple connections to U13, but those connections have to cross all the connections to U11 and U12 to get there.

U14 and U15 are similar - all the connections to them have to cross connections to other ICs to get to U6.

You've placed your parts in a nice, neat, numerical order. That makes it easy to find the parts on the board, but makes the routing more complicated.

  • Ignore the part designators.
  • Place your parts strictly by function and minimizing cross overs in the rats nest.
  • Place any connector that has to physically be in a particular place first.
  • Move components connected to the connectors to minimize crossings in the rats nest.
  • Place the rest of the parts so as to minimize crossings in the rats nest.

I think your circuit can be managed on a double sided board, but you're going to have to be more flexible in where you place the parts.

Mmmpf. I didn't actually answer your question.

Don't bother with the autorouter. As most folks, I've tried them and found that I can route my boards faster and better by hand.

Autorouters might work alright if you have time to tune the parameters for best performance. That will take a lot of time and patience.

About the only time that would make sense is if you are doing large multi layer PCBs with thousands of nodes where you will expect a lot of changes. Manually re-routing that kind of thing would be a lot of work, so tuning the autorouter would be worthwhile.

Additional suggestions:

Look at your schematic.

  • Try drawing the schematic somewhat like your PCB layout, and group the multiplexers by function and IC.

  • Try to minimize crossovers in the schematic by grouping which signals go through which ICs and which multiplexers.

  • The simpler it is to draw the schematic, the easier it will be to lay out the PCB.
  • Draw your circuit using wires for all connections rather than using signal flags.
  • Your goal is a simple, readable schematic with (nearly) all connections as wires and very few crossed connections. That will translate into a PCB layout with fewer crossed connections.
  • Keep crosstalk in mind since you are working with audio.
  • You'll want to use separate multiplexer ICs for certain signals to reduce crosstalk between channels. You'll have to keep that in mind while simplifying the circuit.

If you have a two layer board, and dedicate one to ground, then it's unlikely you can route everything on the other layer.

With a board this complex, you need a policy. Simply dropping wires here and there is not going to work. I notice it's mostly DIL ICs, which means it's not an RF board. So while you still need a competent ground, you do not need a ground plane.

Choose a gridded ground. Lay out a series of ground tracks East-West on one layer, and North-South on the other layer. Connect them into a grid with vias, preferrably at the ground pins of the ICs.

Now place your other tracks. Follow the same orientation on each layer, via through when you change direction, and you will always have a systematic method for getting from A to B, without topologically blocking any other connection. You may still run into crowding problems, which means you need to backtrack and change your placements.

This two layer EW/NS routing is called 'Manhattan Routing'.

Most/some? autorouters have an option for you to restrict tracks on certain layers, so you may be able to set up yours to follow this orientation pattern. However, working with a Manhattan layout means that manual routing is quite straightforward.

I would not recommend leaving the ground until last, and then 'filling the empty areas with copper, using vias to bridge connections between isolated polygons'. The board is so busy that you will miss something, and there is no guarantee that you can actually get ground connectivity at all. Better to start with a complete ground grid (easy to place and check), and then place a track at a time (easy to place and check).

While a two layer board is probably appropriate here, when doing one off designs the cost to go from 2 to 4 layers is often less than shipping. If your goal was to have a dedicated ground plane, and you don't want to spend a lot of time routing efficiently, using a 4 layer board would allow you to have a dedicated ground plane while greatly simplifying routing.

Things are a little up in the air right now due to corona virus, but I just punched in a 4 layer 100x100 mm board into a cheap prototyping service and it came back less than $30. I used to spend hours trying to fit parts onto 2 layers to save on 4 layer boards when they were hundreds of dollars extra, but costs have come down so far it's often not worth the time.