Eagle will not route small connector (QFN sized)

Good to hear you got it going, thanks for letting us know. Good luck with the remainder of your project!

The lib file I posted was the wrong file and had a lot of errors.

I did follow Rachael's advice and fixed the layer issue. Now it autoroutes.

I appreciate everyone's help!

Hi,

there are a lot of mistakes and logical errors between thinking and wishing and truth.

Truth:
The component is not a part of circuit diagrams and don't have circuit diagram names.
The names of the component have just pin names and, or pin numbers.
In the circuit diagram you can insert the component and then this component can get electrical names and electrical pin names.

In the library normally create the component without any board dimensions or electrical attributes (himself the component).
It's just a physical "device" that will be mounted into the board area.

/The grid in the schematic must have 0.1inch, not 0.01inch.
So you must create the symbol pins with this grid with.
Then the router (manually or automatic router) can catch the pin connections for routing the wires.

For further information read the tutorial, the hand book, or the help file.

/what i've seen in your posted lib file (is a script file), it have an error on the source line

182 (The number of opening elements does not match the number of closing elements.)
Also there are some other errors marked as warnings.
Well, i think this file is broken because this have TAG errors. (<tag> ... </tag>)

Please create a new lib of this connector because its the simplest way instead correcting the script file.

Gerald

---

When I tried looking at the library parts in Garrets.lbr, EAGLE v7.5 came up with lots of errors, and wouldn't display the library for me. I went into the schematic and ran "exp-lbrs.ulp", which re-created the library from the project and placed it in the same directory as the schematic and board. I was then able to look at the library parts. As Rachael said, the silkscreen for the SMD connector is the the dimension layer, when it should be in the tPlace layer. Only the overall board outline should be in the dimension layer. In the schematic, *all* parts must be on a 0.1" grid. If not, the nets may not get connected. Note that the schematic grid is totally *separate* from the board's grid.

-Dave P

I will take a look at that.

I modified an existing library, but forgot to look at those layers.

I was in a hurry this morning when I copied the project file. I apologize for that.

I'll give this a shot and report back this evening.

Thank you!

I've just taken a look and I think I know what the problem is. Your library part for that connector contains a bunch of stuff in the "dimension" layer including the large bounding rectangle. Eagle likely thinks this is defining a cut out in the board which clearly it then can't route through. So in order to get it to route first fix your connector library part. If you are unfamiliar with how library parts should be created and what layers should be used then google for library tutorials and maybe look at the Adafruit or dangerous prototypes ones as they are pretty good tutorials. Then you can start again with sensible grid choices and things placed nicely on the grid and a sensible routing grid and hopefully you should be sorted.

If this is a library you found elsewhere let this be a lesson on not trusting 3rd party libraries, they are inevitably more of a pain than just doing them yourself in the first place!

Also, I did note that ERC fails as it picks up two differences between the board and the schematic so back annotation is broken. This is caused by making changes in one when the other is closed. You should probably look at those and fix them too.

Best Regards,

Rachael