Controlled Impedance Traces

[Northy]

Hi all,

As my boards get more complicated, I find myself struggling with controlled impedance traces and reaching the limit of my understanding.
Does anyone know of any good reference materials where I can learn more about doing it correctly?

Up until now I've relied on the board house to tweak my designs to achieve the correct impedance on certain traces, I'd like to understand things better to try to reduce the back and forth with them.

Many thanks,

G

[Northy]

I'm trying to do:

100 ohm differential
50 ohm single ended
and 75 ohm single ended

All on the same internal layer. Is that a good idea? Or not physically possible with the same stack-up?

G

[asmi]

I'm trying to do:

100 ohm differential
50 ohm single ended
and 75 ohm single ended

All on the same internal layer. Is that a good idea? Or not physically possible with the same stack-up?

Theoretically it's possible. In practice depending on stackup and manufacturing limits it may or may not be possible. Two rules you should memorize for single-ended traces:
1) As trace width increases, it's impedance decreases
2) As dielectric thickness increases, impedance increases.

Since you can not vary thickness of dielectric in different parts of the same layer pair, the only "knob" you have to control impedance is trace width. So if you use a typical high-speed stackup with thin dielectrics designed so that you can achieve impedances of 40-45-50 Ohms (which are most commonly used) with reasonably narrow traces, achieving 75 Ohms on the same layer might require traces too narrow for your PCB manufacturer. If you design your stackup such that you can reach 75 Ohm, achieving 50 Ohm on the same layer will require unreasonably wide traces, and so while technically possible, is not very practical.

For differential impedance situation is a bit more complicated as you now have two "knobs" instead of one:
1. If you increase trace width, differential impedance decreases because single-ended impedance of individual traces decreases.
2. If you decrease spacing between traces on a pair, differential impedance decreases due to coupling between traces.

[tridac]

A book from Motorola, "Strip Line Design", or similar, used to be the goto book years ago. Probably find a copy on the abe books site...

[rfclown]

A number of free calculators are available. Some I use:

txline 2003: no installation, just exe and dll file. came from AWR
appCAD: was free HP tool. still available
Saturn PCB Design.
Rogers has one.

I also put some equations into a spreadsheet that I use. Don't have that with me right now or I'd attach it. I got the formulas from an online calculator (that published the formulas used).

Even when the board house gives their calculated widths, I double check with the free tools I have. You want to download the PCB material datasheets to get the correct properties. The 3 examples you give an be done on the same layer. 50 ohm single ended stripline and 100 ohm differential stripline will have about the same line width. 75 ohm single ended will be narrower.

[Northy]

Thank you all very much.

I'm starting to make sense of it all now.

G