# Impedance matching routes in Eagle board

I am making my second board using Eagle CAD. I have different components with a set of different sizes. I set the minimum width for lines to be x. That way, the autorouter creates EVERY line in that width. The problem is that other components are wider, so I think I'd need to somehow widen the lines on the connections to that component (or probably not, the highest frequency in my circuit is of 16 MHz).

How may I do that?

• First step: Don't use the Eagle autorouter. It's appalling, even amongst autorouters. – Nick Johnson Jun 19 '15 at 8:50

Your wavelength at 16 MHz is 18.75 meters. Unless the traces are very long, you shouldn't have impedance matching problems (rule of thumb is wavelength/10)

• Hmmm... explain how frequency would matter for a digital signal? What frequency are you talking about? Clock? Or 3rd harmonic? or 5th? or 7th? or? – Rolf Ostergaard Jun 19 '15 at 5:57
• Yes, I was expecting to get called for that, @RolfOstergaard. I figure he's good to past the tenth on a board of "normal" size and care to keep traces short--but he didnt spec digital. – Scott Seidman Jun 19 '15 at 10:25
• @ScottSeidman to find this result you supposed the speed of current will be the speed of light. But this, for copper, it's not true. Shouldn't so, the lenght, be 1.875m (since on copper the speed is about 10% of the speed of light)? – Pedro Quadros Jun 19 '15 at 11:09

Though the other answers already said that you don't have to care about impedance matching in your case, the time will come where you may need it. More often, you may want to specify wider tracks for higher currents or more clearance for high voltage.

Eagle supports this, and it's called net class.

In the schematic or layout editor, goto menu Edit > Net classes... and define sets of wire width, via drill size and clearance. By Rightclick > Properties... on a wire / net you can assign one of the defined net classes.

This way, the auto router automatically uses these different settings for different nets. Unfortunately, there seems to be no difference when routing the board by hand. At least, the DRC throws an error when you used the wrong size somewhere. When you pour a ground plane, the clearance is taken into account.

Here is an example. The first wire is of the standard net class, the second from a net class with 36mil trace width and the third from a net class with 36mil clearance:

• Thanks for your answer, very helpful for a future in which I will definetely need this. – DogTag Jun 23 '15 at 14:33

If you are doing a digital circuit, the frequency of the (clock) signal is irrelevant for impedance matching.

Rise/fall time is the interesting parameter. If electrical lenght of traces are more than 1/5-1/3 of the rise/fall time, you will see reflections. No matter the frequency. And this can cause issues.

If I read your question right, you wonder if you should taper the trace width out to match wider component pins. That would normally not be required for the type of digital stuff you do today.