Electromagnetism and Controlled Impedances

Jared L. Crum

Department of Electrical & Computer Engineering

Youngstown State University

ABSTRACT: Stripline and mictrostrip calculations were performed to compute the desired thickness between layers in a circuit board design. After the calculations were completed the conclusion was that the inner layers should have 8.09 mils of dielectric between layers, and that between the surface layers and adjacent layers there should be 6.38 mils of dielectric. Finally, the differential impedance for our design was calculated to be 96.4W. Though these numbers have been calculated, the real test comes after the circuit boards are produced. Circuit boards are tested with coupons and Time Domain Reflectometry.

1. Introduction

Design of a circuit involves much more than knowledge of electronics. Often impedance must be controlled for impedance matching. Much high frequency behavior of a circuit is controlled by electromagnetism. Therefore, an understanding of electromagnetic fields is necessary to comprehend this. It turns out that an adjacent plane layer of a circuit board will cause impedances on a signal or trace layer. This impedance is often controlled when a circuit board is designed so that a desired result can be obtained. What is the purpose of controlled impedance? Maximum power is transferred when impedances are matched. A television aerial has characteristic impedance, and a coaxial cable is designed to match this impedance. The input impedance of a television is also designed to match the coaxial cable. Designers of printed circuit boards also have to match impedance of some critical high frequency traces so that one circuit couples the maximum energy into another circuit. The longer a trace is, the greater the need is for controlled impedance. Some of the undesirable effects of an impedance mismatch include low gain in an amplifier, excessive noise, and random errors in digital systems.

The assignment that we received from Sovereign Circuits was to design how the layers of a circuit board should be put together to get desired impedances in signal layers. This assignment is shown in appendix 1. A signal layer is a layer of copper traces, whereas a plane layer is a layer of all copper. The plane layers are either ground or power, and they will cause impedances on the traces of an adjacent layer. The parameter that we need to determine is the distance (H) between layers. All the other data that is needed to make the calculations has been given to us. The width (W) and thickness (T) of the trace, and the relative permittivity (e_r) or dielectric constant of the substrate, and the desired impedance (z) are the parameters that the unknown distance (H) is dependant on. The length of the trace could also enter into the calculations; however, traces that are within the limits of a normal circuit board will generally be between two and seven inches. In this range, the impedance does not vary much with distance; therefore, even computer simulation programs do not take the length of the trace into consideration. Another point to consider regarding this is that all the circuits that are designed for controlled impedances have their traces precisely defined to be a certain length. In the circuit design we were given to work on, for example, certain traces take unusual detours so that all the traces will be of the desired length. Therefore, even with respect to the length of the traces, the impedance is well controlled.

The objective of this assignment is to find a proper distance between circuit board layers. How is a circuit board fabricated? There is a dielectric adhesive that is placed between the layers. An accurate thickness of this layer is obviously important. After the layers have been glued together, there is absolutely no conductance between layers. How is the circuit completed then? Holes are drilled through the board and coded with copper to connect layers together at desired locations. If a circuit board is held up to the light, these conduction holes can be seen through the solder mask. The solder mask is the green layer on the top and bottom of the circuit board that keeps solder from running over and shorting into neighboring contacts. Of course, the contacts are the places that the solder mask does not cover to allow for an electrical connection. Often these contacts are also drilled through to allow for a component to be mounted through the board. This is a brief description of how a circuit board is put together to help us see what is involved in the design of a circuit board.

2. Testing Impedances

After a circuit board is designed and produced, the real test of the numbers shows up. The calculated dimensions generally get close to the desired impedance, but this is not an exact science. How are the boards tested to make sure the impedance is correct? When a printed circuit board is produced, it is generally made in a sheet with about five other identical boards. The sheet is then cut up into individual circuit boards. Each sheet has what is called a coupon on it. The purpose of the coupon is to test for appropriate impedance values. Simply put, a coupon is made of contacts that are easily accessible. These contacts have traces in between them that have nothing to do with the circuit. Their sole purpose is to test the circuit.

Often, after the circuit board is tested, the coupon is cut off and disposed of. Once again, the coupon is a set of contacts with traces in-between that simulate traces inside the actual circuitry of the board. These coupons can be checked quickly since they are designed so that a robot, which automatically probes the contacts and gets the readings, can test them. Often, after readings are taken, adjustments are made to tweak the circuit boards to be made at a later time. This sort of trial and error is necessary since calculations can't take everything into account. Obviously, if the readings are not within the customer's specifications the circuit boards are discarded. At times the coupon is kept on the circuit board so that a concerned customer can check the specifications again. Values for controlled impedances can be computed by hand. They can also be computed with computer simulators. However, the real test is performed with the coupon.

3. TDR

After a circuit board has been produced it can be checked with TDR or Time Domain Reflectometry. Time Domain Reflectometry is the analysis of a conductor by sending a pulsed signal into the conductor and then examining the reflection of that pulse. By examining the polarity, amplitude, frequencies and other electrical signatures of all reflections, errors may be precisely located. If the conductors are manufactured with exact spacing and the dielectric is exactly constant, then the impedance through the trace will be constant. If the conductors are randomly spaced or the dielectric changes along the cable, then the impedance will also vary along the cable. A TDR sends electrical pulses down the cable and samples the reflected energy. Any impedance change will cause some energy to reflect back toward the TDR and will be displayed. How much the impedance changes determines the amplitude of the reflection.

4. Calculations and Conclusions

There are three kinds of calculations that were performed in this project. On layers one and eight of the board, surface microstrip calculations will be employed. On layers three and six of the board, symmetrical stripline calculations will be used. For layer three, differential impedance calculations will the used.

With surface microstrip the traces are on the surface of the board, only surrounded by a plane layer on one side. With symmetrical stripline the traces are right in between two plane layers. With these two kinds of calculations the board can be designed. Also, differential impedance for the traces with 0.015 inch spacing on layer three has to be computed for this project. These traces are easy to recognize in the board design (appendix 5) since they have another trace running parallel to them 15 mils away. This pair of traces has equal magnitude, but opposite polarity signals. The closer the traces are, the greater the field effect will be. Typically, their individual dimensions would result in about 50 ohms, but when they are brought together they produce a differential impedance of around 100 ohms.

The calculations for stripline and microstrip are shown in appendix 2 and appendix 3. These appendices along with appendix 4 clearly depict the dimensions T, W, and H. They also show the difference between stripline and mictrostrip. The circuit design is shown in table 2 on the next page.

The data used to compute the distances between layers are shown below along with the calculated results in table 1.

Table 1: Design Results _

T= Thickness of trace W= Width of trace

e_r= Relative permittivity of dielectric Z= Impedance

H= Height or distance between layers

Microstrip Layers 1 and 8:

T= 1.7 mils W= 6.0 mils e_r= 4.2 Z= 65 W

Calculated H = 6.4 mils

Stripline Layers 3 and 6:

T= 1.2 mils W= 6.0 mils e_r= 4.2 Z= 50 W

Calculated H = 8.1 mils

________________________________________________________________

Table 2: Project Design Diagram _

The circuit board design was to be 62 mils +/- 7 mils.

The design based on the previous calculations is shown below.

Layer 1 ® ---------------- 1.7 mils --------- Not To Scale

Dielectric Layer ® ÀÀÀÀÀÀ 6.38 mils ÀÀÀÀ

Layer 2 ® ---------------- 1.2 mils ---------