The auto router routes 49% of my board. Any tip how to make it route more? Should I route some wires first myself , try to rotate the parts, move them etc. How can u remove the auto routing. How I solve this at the moment is that I save just before i press auto route and then close it and reopen it if I want to try it again when I have moved a part a bit… This seems like a hard way to do it…
Kim
Proper part placment is key to good routing, if the parts are in the optimal places to start with then it makes a world of difference to routing.
Just about everyone here will tell you to try and route your board manually, rather than using the autorouter. The autorouter has merit but not much, and only with simple boards, it just makes a mess of bigger boards.
Start with small boards first and with practice you will be able to route bigger boards, but still, remember that part placement is everything.
To remove the “auto routing” type
ripup
That will tear all the signal traces up in your board. You can also use the ripup tool if you want to just rip up particular traces.
Proper placement is key, as well as having a board that’s big enough. If you are trying to route 100 traces on a top layer only 1"x1" board, with .1mm spacing, you aren’t going to do it no matter what.
You can also rip up some traces, move some components around, and start the auto router again, it will pick up where it left off.
But, I’ll go with what I’ve learned…
Nothing replaces good hand-routing, the autorouter in Eagle isn’t the best.
Hand routing is the only way to go. Especially with the brain-dead autorouter in eagle.
To get good placement, I play with the parts. Rotate them, move them to see when the air wires have the cleanest (least tangled) look. Don’t forget to hit “ratsnest” after you move a part as it will change where the airwires go. Try clustering parts that are related. For examples: put the bypass caps close to where they connect to the chip, put pull-ups next to the pins they pull up and so on.
It helps to define ground planes - polygons on both the top and bottom layers, name them GND. That will clean up a bunch of airwires and give you a start. Hit ratsnest and all your GND airwires will vanish.
If you are having trouble, make the board larger and increase the space between components for the first few boards you do. You will pretty quickly see how to do a better job. I still do that sometimes to get a better sense of how the layout will work. Then I squeeze it all back down once I have a workable design.
Phil
Philba:
It helps to define ground planes - polygons on both the top and bottom layers, name them GND. That will clean up a bunch of airwires and give you a start. Hit ratsnest and all your GND airwires will vanish.
I forgot that one, good tip Phil 
All my simple boards usually have a GND and a VCC pour on bottom/top. SFE advises to only use GND on both layers, but this is mainly due to past experience when boards were cut with sheers.
All the boards I get do not have the copper going right to the edge and are cut cleanly by the board house.
Adding a simple VCC and GND pour can sometimes even half the amount of airwires.
If you want to stick with the auto-router (AR), try making the AR’s grid smaller than the display grid. For example, if your display grid is > 10 mils, make the AR’s grid 5 mil. Reduce the trace widths - EAGLE’s default width is 16 mils (0.016" = .4064mm). 10 mils is good for signal traces, 16 - 24 mils is usually good for power. Most prototype board houses will go down to 8 mils (BatchPCB, Olimex,etc). For signals, I use vias with a 20 mil drill. For power runs I use 24 mill drills, or I use multiple 20 mil vias.
As almost “everyone knows”, EAGLE’s auto-router isn’t very good. However, there’s one on the internet that works with EAGLE and is better than EAGLE’s AR and is free: http://freerouting.net/
HTH
So how do i make the GND plane in eagle, and i will have a look around in the auto router setup to set grid and trace width
Thanks
skatun:
So how do i make the GND plane in eagle, and i will have a look around in the auto router setup to set grid and trace width
Use the polygon tool (not rectangle). Draw a box (4 points) around your board (assuming it has 4 corners). Then you will be able to rename the polygon using the Name tool. Change it to the net you wish it to be a plane for, for ground its usually GND.
For the autorouter, try a grid of 0.05".
I’d go for a much finer grid. The AR makes a mess of off grid pads. A great example of this is the db9 footprint which is hard to route “pretty” even by hand. I have to resort to .0125 alt grid to make it look ok by hand. If all you have is 100 mil pitch stuff, it will do ok but toss in a bunch of 805s and TSOPs to get a totally ugly board.
I work in mm grids usually so the suggestion of 0.05" could be out a bit.
Usually my grid is 0.125mm with an alternate grid of 0.0625mm.