Controlling the impedance (Z) of transmission-line signal traces is an important step in designing printed-wire boards for RF and high-speed digital circuits. Proper impedance matching minimizes unwanted reflections and maintains signal integrity. There are many tools available to the PWB designer to analyze the impedance of the standard PWB geometries. Unfortunately, most of these tools do not address the use of coplanar grounds when calculating impedance. But using numerical methods with the aid of an electromagnetic (EM) simulation tool, it is possible to account for coplanar grounds when they are used in the calculation of PWB trace impedance.

It is a relatively simple task to select the correct signal trace width and distance to the reference ground plane (stack-up) in order to achieve the desired trace impedance. The equations used by simulation tools are often included in the PWB layout tool suite of commercial computeraided- engineering (CAE) programs. These equations are based on standard microstrip and stripline geometries. The microstrip geometry features a signal trace on an outer PWB layer and a reference ground plane some distance below it. The stripline geometry features a signal trace that is on an "inner layer" and two reference planes, one above and one below it. The standard PWB analysis tools handle these two cases very well.

However, most real PWB designs do not fall neatly into these two ideal geometries. Most often, a microstrip signal trace will have not only a ground plane below it, but often will also have ground plane on the same layer next to it, called a coplanar ground. The stripline case may also have a coplanar ground. The coplanar ground is also known as "ground pour" or "ground fill" on the same layer as the signal trace.

Most PWB analysis tools do not account for coplanar grounds when they calculate trace Z. The proximity of this additional ground has the effect of increasing the capacitance of the signal trace to ground and therefore lowers the trace Z. To minimize the effect of a coplanar ground on trace Z, design "rules of thumb" have been applied. If the coplanar ground is kept at a sufficient distance away from the signal trace, the reduction in the trace Z will be within acceptable limits. A popular rule of thumb is to keep the coplanar ground at least one signal trace width away from the signal trace itself so that the reduction in the signal trace Z will be minimal.

One reason that most PWB analysis tools do not include the effects of coplanar grounds is that there are no closed-form solutions for these geometries. However, CAE simulation tools are now available that can calculate the trace Z for almost any geometry using numerical methods. To check the "rule of thumb," the well-known suite of EM simulation software tools from Sonnet Software (www. sonnetsoftware.com) were used for computer analysis. The Sonnet Suite of software tools are full-wave threedimensional (3D) software programs written for simulating the electrical behavior of a wide range of circuits and high-frequency designs. The 3D planar EM software is ideal for analyzing printed circuit boards (PCBs), filters, planar PCB antennas, lowtemperature- cofired-ceramic (LTCC) components, and even the transitions between an integrated circuit (IC) and its package. For those seeking a painless introduction to the world of EM simulation, Sonnet offers a free, feature-limited version of its Sonnet Suites software for EM simulation o high-frequency designs from 1 MHz through terahertz frequencies. The software is available for free download from the Sonnet web site.

As a test value of dielectric constant for the substrate material, a dielectric constant of 4.5 was used, which is representative of printedcircuit- board (PCB) laminates based on FR4 material.

The investigation began by calculating the signal trace Z for several microstrip and stripline cases without any coplanar grounds. As expected, these results agreed well with the results from PWB analysis tools. The study proceeded by adding coplanar grounds spaced at various distances from the signal trace and determined the trace Z reduction. The results for the coplanar stripline and microstrip configurations are shown in Figure 1 and Figure 2. As the edge of the coplanar ground is brought closer to the edge of the signal trace, the signal trace Z is reduced as expected. Parameter G/H is the measure of the coplanar edge to the signal trace edge spacing. Parameter G is the gap or spacing between the edge of the signal trace and the edge of the coplanar ground, while H is the height of the signal trace to the reference plane (*Fig. 3*). When performing calculations, both G and H must be in the same units, i.e., mils or in. For example, if the gap G between the edge of the signal trace and edge of the coplanar ground is 20 mils and the stackup dielectric thickness between the bottom surface or the signal trace and the underlying ground plane is 20 mils, then G/H = 1.

The results show that if the gap G between the coplanar ground and a microstrip signal trace is at least as large as the height H to the ground plane, i.e., if G/H is greater than 1, then the reduction in signal trace Z is under 5 percent. A stripline signal trace is even less sensitive to the presence of the coplanar ground and a G/H value greater than 0.7 will suffice. This agrees with the commonly accepted rule of thumb.

In some designs where space is limited, it may be necessary to reduce the gap below the rule of thumb value. The graphs can be used to determine the value of Z reduction required, with compensation provided to account for the reduction. For example, if space is limited and a gap G of 10 mils is needed around a 75-Ohm microstrip signal trace, a value of 20 mils for H will yield a G/H value of 0.5. The graph indicates the trace Z will be reduced to about 87 percent of the value without the coplanar ground. Knowing that the reduction value is 87 percent, a standard PWB calculation tool (which does not include the effect of the coplanar ground) can be used to design for a trace Z that is not 75 Ohms but equal to 75/0.87 which is equal to 86 Ohms. The presence of the coplanar ground will reduce the actual trace Z down approximately to the desired 75- Ohm value.

To further test the analysis approach, a microstrip trace with sublayer grounds was evaluated. Along with the coplanar ground, there is an extra ground layer between the bottom of the signal trace and the reference ground plane. The extra ground layer is gapped or open under the signal trace by the same horizontal amount as the coplanar trace. Figure 4 shows a 3D edge view created by the Sonnet EM software. The pink areas represent the copper signal trace on the top layer of a circuit board, the coplanar ground on the top layer and the sublayer ground. The grey bottom surface is the solid reference ground plane for that circuit board. The two lower dielectric areas have a dielectric constant equal to 4.5. The space above the top layer is free space with a dielectric constant assumed to be equal to 1. Comparing the coplanar data for microstrip 50 Ohms and the data for microstrip 50 Ohms plus the sub plane (the bold blue traces in Fig. 2) shows how the trace Z is further reduced by this extra sublayer ground. The additional effect is under 2 percent.

Armed with this information, it is possible to apply the commonly accepted rules of thumb for coplanar ground spacing and know that the trace Z will be reduced by less than 5 percent. For cases where we can't follow the rule of thumb, the indicated correction can still be applied.