# Bert Simonovich's Design Notes

Innovative Signal Integrity & Backplane Solutions

## PCB Cross-sectional Geometries

PCB cross-sectional geometries describe the details of the dielectric substrates, traces and reference planes within a PCB stack-up.  Their physical relationship with one another can then be used to predict the characteristic impedance of the respective traces. There are only three generic cross-sectional geometries with variations within each. They are:

• Coplanar
• Microstripline
• Stripline

Coplanar:

Coplanar geometry, or sometimes called coplanar waveguide (CPW), is a signal conductor sandwiched between two coplanar reference conductors or planes. These reference planes are usually ground. The characteristic impedance is controlled by the signal trace width and the gap between it and reference planes. This is a common transmission line structure for RF and microwave designs using single-sided printed circuit board technology. As a rule of thumb, the width of the reference plane on each side of the signal trace should be at least five times the distance between the left and right plane.

Microstrip line:

The microstrip line is the most popular transmission line geometry used in two or four layer printed circuit boards. The characteristic impedance is controlled by the signal trace width, on one side of the substrate, and the thickness of the substrate to the reference plane below it. The embedded microstrip line has the signal trace covered with prepreg or other dielectric material.

Cross section views below showing Microstrip line (left) and embedded microstrip line (right).

Stripline:

Cross section views below shows an example of single stripline (left) and dual stripline (right) geometries. These are geometries are typically found in multi-layer PCBs of 6 layers or more.  The characteristic impedance is controlled by the trace width, thickness and its proximity to the reference planes above and below.

Single stripline has one signal layer sandwiched between two reference planes. If the signal layer is exactly spaced between the two reference planes, the geometry is called a symmetrical stripline; as opposed to an asymmetrical stripline, where the signal trace is offset from the center of the cross-section.

Dual stripline geometries have two signal layers sandwiched between reference planes, and are mainly used to save layers; caveat is a trace on one layer is routed orthogonal to the trace on the other  to mitigate crosstalk.

Differential Pair Geometry:

Differential signaling is when a signal and its complement are transmitted on two separate conductors. These conductors are called a differential pair. In a PCB, both traces are routed together with a constant space between them as edge-coupled or broadside-coupled.

Edge-coupled routes the traces side-by-side on the same layer as microstrip or stripline. The advantage is that any noise on the reference plane(s) is common to both traces and thus cancelled at the receiver. Most differential pairs are routed this way.

Broadside-coupled routes one trace exactly over the other on 2 separate layers as dual stripline. Since each trace is more tightly coupled to its adjacent reference plane than the opposite reference plane, any noise on the planes will not be common to both traces and thus, will not be cancelled at the receiver. Because of this, and the fact that it usually results in a thicker PCB, this geometry is rarely used.

Odd-Mode Impedance:

Consider a pair of equal width microstrip line traces, labeled 1 and 2, with a constant spacing between them. Each individual trace, when driven in isolation, will have a characteristic impedance Zo, defined by the self-loop inductance and self-capacitance of the trace with respect to the reference plane.

When a pair of traces are driven differentially, the mode of propagation is odd. If the spacing between the transmission lines is close, there will be electromagnetic coupling between the two traces. This coupling is defined by the mutual inductance and capacitance.

The proximity of the traces to a reference plane(s) influences the amount of electromagnetic coupling between traces. The closer the traces are to the reference plane(s), the lower the self-loop inductance and stronger self-capacitance to the plane(s); resulting in a lower mutual inductance, and weaker mutual capacitance between traces. The result is a lower differential impedance.

A 2D field solver is usually used to extract the parameters for a given geometry. Once the RLGC parameters are extracted, an L C matrix can be set up as follows:

The self-loop inductance and self-capacitance for trace 1 and 2 are L11, C11, L22, C22 respectively. The off diagonal terms in each matrix, L12, L21, C12, C21, are the mutual inductance and mutual capacitance. We use the LC matrix to determine the odd-mode impedance.

The odd-mode impedance is the impedance of one trace, of a differential pair, when driven differentially. It can be calculated by the following equation:

Where:

Zodd = odd mode impedance

Lo = self-loop inductance = L11 = L22

Co = self-capacitance = C11 = C22

Lm = mutual inductance = L12 = L21

Cm = mutual capacitance = |C12 |=|C21|

Even Mode Impedance:

When current flows down both traces, of the same polarity, the mode of propagation is even and the coupling is positive. The even mode impedance can be calculated using the following equation:

Differential Impedance:

The differential impedance is twice the odd-mode impedance:

Average Impedance:

When current flows down two traces randomly, as if they were single-ended, the mode of propagation is a combination of odd and even. The average impedance of each trace is affected by its proximity to the adjacent trace(s); calculated by the following equation:

Coupling Coefficient:

The coupling coefficient, Kcc, is a number that conveys the amount of electromagnetic coupling between two traces. Knowing the odd and even mode impedance, Kcc can be calculated by the following equation:

Backward Crosstalk Coefficient:

Two traces near one another will couple a portion of its own signal to the other. If we consider one trace as the aggressor, and the other as the victim, the amount of coupled noise travelling backwards on the victim’s trace, opposite to the aggressor’s direction, is called Near-End crosstalk (NEXT) or backwards crosstalk. The amount of coupled noise, travelling in the same direction as the aggressor’s direction, is called Far-End crosstalk (FEXT).

In stripline, there is little to no FEXT, but backwards crosstalk will saturate to a fraction of the amplitude of the aggressor’s voltage for the length of time the traces are coupled. This fraction of the aggressor’s voltage is  called the backward crosstalk coupling coefficient Kb. It is equal to one half of the coupling coefficient Kcc :

Example:

A 8-9-8 mil differential pair; with 12mil core; 12 mil prepreg; Dk=4; stripline geometry; 1/2 oz copper; has the following R L G C matrix extracted from a 2D field solver:

If the two traces are driven differentially, then the differential impedance is 100 Ohms and there is 13% coupling of the two traces. On the other hand, if the traces are driven single-ended then the characteristic impedance of each trace is 53 Ohms. With 9 mils of space between them, the backward crosstalk is 7%.

If you increase the spacing between traces until Zodd equals approximately Zeven, the coupling will reduce to near zero, and there will be little backward crosstalk. Depending on your design and your noise budget, you may be able to live with a certain amount of backwards crosstalk. The only way to know the spacing between traces to achieve the budget is to plug in the numbers.

Acknowledgment:

I would like to thank my old Nortel colleague, the late Dick Goulette, for sharing these equations many years ago. They have served me well over the years.

Written by Bert Simonovich

February 7, 2011 at 8:52 pm

Tagged with ,

This site uses Akismet to reduce spam. Learn how your comment data is processed.