# Differential Trace Impedance

### High-Speed Digital Design Online Newsletter: Vol. 5 Issue 02

A last-minute cancellation has opened a window
in my schedule for private seminars. A private
seminar gives you and your co-workers a perfect
opportunity to learn the latest in high-speed
digital design within the context of *your* designs.

If you are located in the Southwest US and have 30 or more digital engineers at your site, please write to info03@sigcon.com by Feb 15, 2002 for more information about this opportunity.

## Differential Trace Impedance

Mitch Morey, San Diego, CA:

I'm working on a board with 100-ohm differential signaling that I would like to design for microstrip routing. I've used the Polar Instrument calc, the ADS LineCalc software, and have got two additional stackup constructions for our fab houses, and have talked to numerous people on this.

Here are the recommendations I have gathered so far. All configurations represent 100-ohm differential microstrips, operating at 2.4Ghz speeds, using a 5mil-thick FR4 dielectric, with an underlying solid copper reference plane.

- .005" lines with .005" edge to edge (fab shop 1)
- .004" lines with .008" edge to edge (fab shop 2)
- .005" lines with .008" edge to edge (ADS LineCalc)
- .006" lines with .0065" edge to edge (ADS LineCalc #2)
- .016" lines with .016" edge to edge (engineer #1)
- etc. etc.

???**!!*!???

Thanks for your interest in High-Speed Digital Design.

What you need is a piece of software called a two-dimensional E&M field solver. This program calculates the magnetic and electric fields surrounding your traces, and from that data extracts the impedance and delay. This is the best way to do impedance calculations. The good field solvers allow you to specify the trace width, height, spacing, thickness, dielectric constant, AND they allow you to overlay the trace with a solder-mask layer.

I'm not sure what ADSlinecalc uses, but if it's not a two-dimensional field solver you shouldn't trust its results. I have reason to distrust the accuracy of the examples you have provided.

First let me give you some general principles to help you understand what's happening and then I'll rule out a couple of the solutions below.

The first thing you need to know is that the
patterns of electric field lines in a dielectric
medium follow the same shapes as patterns of
current flow in solid conductors. This sounds
pretty obtuse, but it's going to help you in a
major way, because it will help you *see* what is
happening when you change the trace geometry.

Follow me for a minute on this mental experiment. Start with a microstrip trace of length X. I want you to mentally replace the dielectric medium surrounding this trace with a slightly conductive solid material. Now imagine that you connect an ordinary ohmmeter between the trace and the ground plane. The value of DC resistance you measure in this experiment will be exactly proportional to the IMPEDANCE of the trace. I hope you can now imagine what would happen if you press the trace closer to the ground plane. Can you see that the impedance must go DOWN, because there is now less material between the trace and the reference plane? If the trace is pressed down to the point where it nearly touches the reference plane, its resistance to ground (i.e., impedance) approaches zero.

What about doubling the width? This adjustment practically doubles the conductive surface area, substantially lowering the resistance to the reference plane (i.e., impedance). I like using this DC analogy because most engineers find it a lot easier to imagine simple patterns of DC current flow than they do high-frequency electromagnetic fields. The constant of proportionality isn't important—I just want you to see what's going to happen as you make various adjustments.

So far I've shown two things that decrease the impedance in microstrips:

- (1) Moving a trace closer to the reference plane decreases its impedance.
- (2) Fattening a trace (i.e., increasing its width) decreases its impedance.

And the converse statements are also true,

- (3) Moving a microstrip further away from the reference plane increases its impedance.
- (4) Shaving down the trace width increases its impedance.

Stripline traces are a little more complicated in that you must account for the distance from your trace to both top and bottom reference planes. The general result for offset striplines is that whichever plane lies closest to the trace has the most influence on the impedance. Smack in the middle the planes are both equally important.

Let's now imagine a differential configuration with TWO traces. Connect the ohmmeter BETWEEN the two traces (from one to the other). The resistance you read now will be proportional to the DIFFERENTIAL impedance of two-trace configuration. [NOTE: one- half the differential impedance is DEFINED as the odd-mode impedance.]

If your two traces are set far apart, and they have the same dimensions as in the first experiment, your new differential measurement will be exactly TWICE as great as before. If you draw out the patterns of DC current flow you can see why. For *widely* separated traces the current flows mostly from one trace straight down to the nearest reference plane, then it shoots across the plane to a position underneath the second trace, and from there it leaks back up to the second trace. As this current flows, it encounters a resistance R1 when leaving the first trace, practically zero resistance flowing across the plane, and then another amount R1 as it flows back up to the second trace. The total resistance encountered is 2*R1.

- (5) The differential impedance of two widely separated traces equals twice the impedance to ground of either trace alone.

Now let's see what happens to the differential impedance as you slide the two traces towards each other. When they get close enough, significant amounts of current begin to flow directly between the traces. You still get the same old currents going to and from the reference plane, but in addition to those currents you have now developed a new pathway for current, direct from trace-to- trace. This additional current pathway acts like a new resistance in *parallel* with the original, widely-spaced current pathways. The new parallel pathway lowers the differential impedance of the configuration. You may conclude:

- (6) The differential impedance of a tightly- spaced pair is less than twice the impedance to ground of either trace alone.

If the traces are moved so close that they nearly touch, the differential resistance (impedance) approaches zero. In general, the differential impedance is a monotonic function of the trace separation.

- (7) All other factors being equal, the tighter the inter-trace spacing, the less the differential impedance.

I view any decrease in impedance as an annoying side-effect of close spacing. If I could re-design the universe, I'd try to make it not happen. Fortunately, you can counteract the annoying drop in impedance by shaving down the width of your traces. If you shave off just enough width you can push the impedance back up to where it belongs. In this way, the trace separation and trace width can be made somewhat interchangeable.

- (8) To maintain constant impedance, a reduction in spacing must be accompanied by a reduction in trace width (or an increase in trace height).

With these eight rules in mind, let's now look at the specific recommendations you have been given.

With your 5-mil dielectric, the individual impedance of a 16-mil trace on FR-4 already falls below 50 ohms, so the differential impedance will be less than 100 ohms regardless of what spacing you use. You can there rule out the 16-mil configuration. I suspect your engineer #1 may have been thinking about using a thicker dielectric than what you propose.

The two ADSlinecalc results conflict with each other. Staring from a pair 5-mil wide with an 8-mil space, INCREASING the trace width to 6 mils will lower the impedance, and DECREASING the spacing to 6.5 mils will lower it even further. Therefore, one of these results must be wrong. They cannot both be 100-ohm solutions. Therefore, I suspect something is either wrong with your copy of ADSlinecalc, or (dare I say it) your use of the tool.

Here's some data from a commercial 2-D field solver (HyperLynx). All these combinations should give you a 100-ohm differential microstrip impedance under the following conditions:

- Dielectric thickness = 5 mil
- Relative permittivity at 1 GHz = 4.3
- Trace thickness = 1/2-oz cu + 1-oz plating (1.5-oz total)
- No solder mask (***when your vendor adds solder mask he or she will somewhat reduce the trace width to compensate for the extra dielectric material above the traces.

Each combination in Table 1 is listed as a pair [w, s], where w is the finished, plated trace width in mils, and s is the finished, plated edge-to-edge separation in mils.

w | s |
---|---|

8 | 14 |

7 | 11 |

6 | 7 |

5 | 5 |

Whatever you choose to do, insist that your board fabrication shop place differential impedance test coupons on your panels and test each one to verify that you are getting the correct impedance.

Below I have attached a listing of 100-ohm stripline configurations. Obviously, this is just a small sampling of all possible combinations. In the chart, dimension "b" is the interplane separation, "h" the height of the trace above the nearest plane, "w" the trace width, and "s" the edge-to- edge separation, all in mils. Parameter rSKIN is the effective AC skin-effect resistance at 1 GHz, Z0 is the (high-frequency value of) characteristic impedance, and the column marked "dB/in. @1GHz" is the trace attenuation due to the skin effect, in dB/in., at a frequency of 1 GHz. Don't forget to also consider dielectric losses. All the stripline configurations assume 1/2-oz Copper on an FR-4 substrate with Er=4.3 at 1GHz.

I hope this information is useful to you.

Best Regards,

Dr. Howard Johnson

b h w s rSKIN Z0 (dB/in.@1GHz) 10 3 3 40 3.501 99.03 0.1522 10 4 3 7 3.235 100.4 0.1389 10 5 3 7 3.218 101.2 0.1371 10 5 4 40 2.76 94.59 0.1258 14 4 3 5.5 3.191 101 0.1361 14 4 4 12 2.738 100.3 0.1177 14 5 3 4.5 3.136 100.1 0.135 14 5 4 7.5 2.599 100.5 0.1116 14 5 5 40 2.329 99.51 0.1011 14 7 3 4.5 3.112 101.8 0.1317 14 7 4 6.5 2.556 100.6 0.1096 14 7 5 13 2.236 100.9 0.09574 14 7 6 40 2.006 94.98 0.09126 20 5 3 4.4 3.141 101 0.134 20 5 4 6.5 2.592 100.7 0.1111 20 5 5 11 2.271 100.6 0.09746 20 5 6 40 2.087 98.41 0.0916 20 7 3 3.9 3.132 101.1 0.1336 20 7 4 5.2 2.547 100.9 0.1089 20 7 5 7 2.165 100.7 0.0929 20 7 6 10 1.908 100.3 0.08218 20 7 7 19 1.75 100.7 0.0751 20 7 8 40 1.613 96.34 0.07242 20 10 3 3.7 3.143 100.6 0.1347 20 10 4 5 2.54 101.6 0.1079 20 10 5 6.5 2.148 101.4 0.0915 20 10 6 8.5 1.876 100.7 0.08054 20 10 7 12 1.682 100.5 0.07236 20 10 8 25 1.562 100.3 0.06735 30 5 3 4.3 3.147 100.7 0.1347 30 5 4 6.3 2.595 100.7 0.1112 30 5 5 10 2.268 100.7 0.09729 30 5 6 22 2.087 100.2 0.08996 30 6 3 4 3.139 101 0.1339 30 6 4 5.4 2.564 100.7 0.1099 30 6 5 7.5 2.195 100.7 0.09415 30 6 6 11.2 1.955 100.6 0.08399 30 6 7 20 1.81 100.4 0.07795 |