Cheap to midrange autorouters are shit. People tell me that the ones from really expensive packages like cadence allegro are better but still can't do as well as a good PCB designer routing by hand. I've never used those packages myself so I can't say for sure.
first you need design rules fine enough that you can get a track between two pads. If you don't have that then you will never succeed. Since you haven't told us the pad size I can't say what those design rules would be but basically you need to take the pin pitch, subtract the pad size and then divide by 3. Some high density connectors will basically require a PCB process that is a step up from some of the cheapest hobbyist services. You also want to be on a grid that is an exact subdivision of half your pad pitch and have your pads aligned to that grid (yes this is a PITA when working with a mixture of metric and imperial components).
Looking at your board I notice the autorouter is putting tracks closer to each other than to the connector pads. You might want to check if your tool has some sort of "pad to track clearance" setting that is larger than the regular clearance setting.
Once you get a suitable set of design rules you can "escape" the connector by following a pattern. You can escape the first row straight out. The second row can use the gaps between the pins in the first row. The third row can use the gaps in the first and second row on the other side of the board. The remaining rows can route out the other side.
Unfortunately even once you have escaped the connector you still have to get the tracks to their destinations. How difficult this is depends on how rigid your circuit design is. If you can swap pins then life is much easier, if you can't swap pins and the pin arrangements on the two sides don't match up well then life gets very painful. Lots of vias, lots of time spent routing and re-routing. Sometimes you may have to make the board bigger or add more layers.
Speaking of vias your vias look as big as your connector pads. That seems weird to me. Once you have figured out your track and gap you might want to look at what PCB manufacturers can meet those specs and what their hole size/annular ring specs for vias are.