The problem is I want to use a socket for ICs, but by default EAGLE will put traces on both layers. So you would have to solder the top layer traces to the IC, and the bottom layer. But with a socket you can only really reach the bottom ones.
Any idea how to connect a part to only 1 layer?
Thanks.
Just hand route? Or if you have boards professionally made, the holes will be plated all the way through, so you don’t need to worry about which side you solder on.
Cheers,
–David Carne
Ah I see. If I were to send in a quote to make boards, does an eagle board file specify that the holes are to be plated?
cfinger:
Ah I see. If I were to send in a quote to make boards, does an eagle board file specify that the holes are to be plated?
Greetings cfinger,
Professionally made PCBs have all holes plated unless specified otherwise. The BatchPCB service only offers plated through holes.
If you make the PCB yourself it’s unlikely you’ll have plated through holes which requires a much more involved multi-step process.
Back to your original question, in EAGLE you can build a library part for your IC socket that has a keep out zone on the top layer. This will prevent the auto-router from placing traces under the body of the socket.
Comments Welcome!
@bigglez and busonerd: Thanks for the info. It makes sense that they would plate all the holes…
I usually build my own prototypes, perhaps I’ll put vias close to the pins of the IC so I can use the socket. Will clutter the board a bit, but it works.
Thanks.
I make my own boards and I have a tendency to use Eagle’s autorouter whenever I can. One way to get it to do what you want is to draw polygons on the tRestrict, bRestrict, and vRestrict layers. tRestrict and bRestrict will prevent eagle from allowing any traces on the top or bottom side of the board in that area. If you draw a rectangle on the tRestrict layer that completely surrounds your socket and its pads, eagle won’t be able to connect anything to them so it will route to the pads on the bottom side of the board. For DIP sockets, you could do two rectangles, one surrounding each row of pins, with a gap in between. This would let eagle route a few traces down the center of the DIP chip on the top layer. I’m usually too lazy and just draw a big box around the whole thing. I use this trick for polarized headers, LEDs, electrolytics, anything I can’t solder on the top.
Note that this will restrict some of the things you’d actually want eagle to be able to do, like route top layer traces across the DIP socket going between pins. It’s usually not a problem for me.
I sometimes put a vRestrict around resistors & diodes to keep eagle from putting a via under them. Just as a matter of preference, I don’t like having components sitting on top of my bumpy vias. It still lets eagle connect to the top or bottom side of the pins.
The restrict rectangles will cut holes in your power/gnd polygons if you use them. If this happens to you, get everything routed, save off a copy, then delete all of your restricts and run ratsnest to fill in the polygons.
ah… good call emf. Thats perfect for what I’m doing. Now if only it didn’t create so many pesky vias 
I route by hand - the eagle router is pretty close to a joke.
to do home made double sided boards you need to apply what I call non-plated-through-hole design rules. They are basically just a bunch of fairly obvious things to avoid or do. Primarily, look at each component lead and decide if you can solder top and/or bottom. Then when you place a part, be aware of which side of each pin is solderable and route accordingly. It may seem hard based on my description but it really isn’t. It’s pretty easy to pass a signal from one side of the board to the other via a resistor, capacitor, transistor switch, etc… When all else fails, make a via. drill it out and solder a piece of wire in the hole. typically, I only have to make a few vias. One thing you need to remember is to make sure that you leave enough room next to the leads to solder on the top side.
overall, it’s really quite easy once you get the hang of it.
Philba:
I route by hand - the eagle router is pretty close to a joke.
If only the router in my head were less of a joke than Eagle’s… sigh
you should try it. It’s really not that bad. especially if you put polygons on both sides and name them GND. That will significantly reduce the numbers of airwires. Start small and work up. It took me a few boards to get comfortable with it but it’s not that hard.