Can't Route Arduino

Question

I am using the standard edition of Eagle 7.5

I have grabbed an Arduino Micro from the Element 14 library (E14_Arduino_revB.lbr). I placed this device on a board expecting to have the board drilled out for the pins of the Micro to go into and to route traces from these holes to other device on the board. (This seemed like a simple enough thing to do).

BUT...

1) AutoRouter refused to route any air traces to the Arduino pins.

2) Manually attempting to route a trace to the Arduino pins refuses to obey

3) Routing any trace anywhere near the Arduino turns the cursor into a Do-Not-Enter sign (circle with line through it).

SO (BTW, if you haven't figured this out yet, I am new to Eagle)

Is this something wrong with the library object?

There don't appear to be any routing exclusion zones in the exclusion or restrict layers in the package.

WHAT do I do? How do I make this work?

rachaelp · Accepted Answer

Hi Kingsley, David's answer above is a clue but I think the underlying problem is the library part doesn't do what you (or I when I first looked at it) were expecting. If you load the library part into the library editor and examine it you'll see that: a) It's got its bounding box on the dimension layer (i.e. how you draw a board outline). b) It's got SMT pads where the USB connector is. So basically it's defining itself as a board and confusing the auto router. If you put components within the bounding box of the Arduino board then you will find the auto router will route to them (I have just tried and it does). Interestingly I can manually route the connections whereas you can't so you have another issue going on there. Have you loaded any design rules or anything? I'm not sure what the original purpose of this library is. It provides a symbol like it's defining a component but then provides things you couldn't route to if you put it on a board (you can't route to the SMT USB pads if you were to place an Arduino Micro on the board using the through hole pads provided) and it also provides a board outline rather than a placement outline so screws up routing to it (if you use the auto router at least). I guess if you are wanting to create your own variant of an Arduino Micro it might be useful but that's a very limited use case I would have thought. My personal opinion is it's not a particularly useful (or well designed) library and you should probably just create your own library for what you want to do. This is actually the best thing to do in most cases anyway as bundled "free" libraries (as with pretty much ALL schematic tools, not just Eagle) or ones downloaded from the internet are generally not ideal to use and you really need to thoroughly check anything you haven't created yourself anyway (or risk having to rework or worse scrap off a batch of boards if a library contains any errors) so you are better off just creating your own trusted libraries in the first place. Best Regards, Rachael -- Web access to CadSoft support forums at www.eaglecentral.ca. Where the CadSoft EAGLE community meets.