We can fabricate boards using PCB material that has copper only on one side, or material with copper on both sides. Boards with copper on only one side take less time to fabricate. If you can get all of your circuit onto one layer without using any vias, this is the simpler and faster way to make the board.
Due to the nature of the milling process, the vias and pads are not plated through the board, meaning the top and bottom sides are not initially connected. This has important consequences:
Big wide traces are good, up to a point. You should make the traces as wide as possible given the density of the circuit. That makes the board much easier for me to mill and much easier for you to solder.
To make a group of traces wider in Eagle:
These images give a general idea of what trace widths will work when running traces between pins:
If your board absolutely requires narrow traces, then use trace width >= 10 mil (10 mil = 1/100 inch = 0.254 mm). Separate tracks, pads, vias, etc. by spaces >= 10 mils wide.
In Eagle you use the "Polygon" command to create areas of solid copper on
the board. Unless you are using the background copper as a ground or power
plane, please do not submit boards with polygons drawn over the whole board.
In the past, some students have gotten the impression that we will always
remove all copper from the board that is not shown as copper in their files.
They will then put polygons on the board not connected to ground or power to
prevent it all from being removed, like this:
We would rather you submit a design like this:
Then, unless you specify otherwise, we will only remove a 1mm insulation channel around the outside of your traces, like this:
We can manufacture the boards more quickly if we define those empty channels rather than you.
But in cases where the background copper is to be used as a ground or power plane, use the Polygon function.
We often receive board submissions with Polygon areas that look like this, in which the Polygon's "Isolate" parameter is set to 8 mil = 0.008":
It is much better if you increase the "Isolate" parameter on your Polygon to something like 50 mil, producing something more like this:
This makes is a lot easier for us to fabricate the board and for you to solder on it without accidentally shorting pins to the background copper.
A common mistake is to make traces that are too narrow to handle the necessary current. These burn up spectacularly the first time you turn on the power, like this:
More current requires wider traces. Our FR4 board material has "1
ounce" copper on both sides, so your traces will be made of this. The
chart below shows the trace temperaures that will occur for different
currents on 1 ounce traces of different widths. Use it as your guide for
|Trace Width in Mil||Maximum Current in Amps|
You can also use this PCB Trace Width Calculator.
As discussed above, you must solder wires into all vias. These solder joints create a small bump on the board. If the bump is underneath a surface mount IC, it may be impossible to solder the IC down. So do not put vias under these chips.
If you are using the autorouter in Eagle, restricted zones can be defined to prevent placement of vias under these chips. These are defined by drawing shapes on the "vRestrict" layer.
Having vias underneath socketed DIP ICs is usually not a problem.
The not-so-great Autorouter function in Eagle can create absurdly complex routings with dozens or HUNDREDS of vias. Remember that you will have to solder a wire into each one, so you want to minimize the number. I recommend routing the board by hand if at all possible for a better design.
If you must use the Autorouter function in Eagle, then download this ZIP file and use the Autorouter Parameter and Design Rules files contained in it. Please DO NOT use the default Design Rules and Autorouter settings in Eagle. They will produce boards that are very difficult for me to make due to the very narrow traces and close spacing.
Instructions for using my files in Eagle Version 4.16r2:
When defining the outline of the board on the Dimension layer, please draw it with wires with width=0. This is especially important if you want traces to go right up to the edge of the board. Width=0 makes things a lot easier on this end.
I have no equipment for doing silk screens, and I remove text when it is included in the top or bottom layer Gerber files. It wastes time, wears out the mill bits, and generally causes me problems. So don't bother putting text in there because I will delete it.
|NOT GOOD - Top-layer traces go to relay pins (highlighted
in red) which are covered up when the relay is in place
If you want to run a top-layer trace to a component pin, make sure the pin will be visible from above the board when the component is in place. With our boards, soldering a pin on the bottom will not be sufficient to make a reliable connection to a trace on the top. So it is best to put all traces to these invisible pins on the bottom layer of the board.
If you absolutely must have traces on the top side going to pins obscured by the component (or if you forgot to follow the rules!), it is difficult but possible to solder the component on anyway.
Normally, our boards are made with a strip of copper removed around the outside of the traces and pads, and the rest of the copper left on the board, like on our main PCB page. But it's possible for me to remove all the copper on the board except for the traces, pads, etc. This takes longer, but some people need this done, especially if they have transmission lines on the board and the extra copper will cause interference. If you need all the excess copper removed from the board, specify this in your request email. BUT, due to the extra time and bit wear, I am reluctant to do this unless absolutely necessary. The regular channels are wide enough to make it easy to solder DIP and surface mount components down.
Very few people make a perfect working PCB on the first try. If there are wiring mistakes in your design, please try to modify the board yourself rather than ordering a new board. Traces can be cut with an XActo knife, and new connections can be made by soldering on jumper wires. If there are only minor problems on the board, please try to correct them this way if at all possible. In the few weeks before demos in Senior Project Lab, I get barraged with large numbers of board orders, and the turnaround time on boards increases. It may be much faster for you to modify the board yourself.
-Mark Smart firstname.lastname@example.org
Back to ECE Shop Index
ECE Shop Rooms 1041-1046 ECE Building 306 N. Wright Urbana, IL 61801 (217) 333-2173