Strategies to the Design of Crosstalk between Two Parallel Micro-strip Lines on PCB Based on the Simulation Analysis

Crosstalk Theory

Based on electromagnetic theory, crosstalk refers to the electromagnetic decoupling between two signal lines. It is a type of noise caused by mutual capacity and mutual impedance between signal lines.


In Figure 1, among the two parallel lines, one line has signal source (VS) and internal impedance (ZOG) at one end of the line and load impedance (ZLG) at the other, forming a closed loop through ground. The other line only has resistance (ZOR and ZLR) with a structure of single wire to the ground. In this figure, the lead with signal source is called emission line or interference line while the other line is called receiving line or interfered line.



When driving signal (1) is passing the emission line, interference signal will be generated with contrary directions as a result of the parasitic capacitance between emission line and receiving line. Meanwhile, while passing the emission line, driving signal will generate a changing magnetic field that induces an interference current with a contrary direction to driving signal after crossing the receiving line. The interference current (2) and (3) are crosstalk signal decoupled from the emission line to the receiving line by the driving signal. This is how crosstalk is generated.


Crosstalk can be classified into capacitive crosstalk and inductance crosstalk based on different causes. Capacitive crosstalk refers to the decoupled voltage generated by mutual decoupled capacitance while inductance crosstalk refers to the decoupled current generated by mutual decoupled inductance.


Based on the places where crosstalk takes place, crosstalk can be classified into near-end crosstalk and far-end crosstalk. In Figure 1, near-end crosstalk is the interference signal generated by the driving signal (1) at the near end of the receiving line, adding capacitive crosstalk (3) and inductance crosstalk (2). Far-end crosstalk is the interference signal generated by the driving signal (1) at the far end of the receiving line, inversely adding capacitive crosstalk (3) and inductance crosstalk (2).


Crosstalk is generated between two leads because of electromagnetic decoupling. The analysis of crosstalk is to calculate the interference voltage from the driving signal inductance to both sides of the receiving line with the driving signal provided. VR(0) is set as the interference voltage on the receiving line when X is equal to 0 while VR(L) is the interference voltage on the receiving line when X is equal to L. Then two formulae can be obtained:


The Simulation Model of Crosstalk Analysis between Two Parallel Micro-strip Lines

In this article, the printed circuit board used in the simulation model has a size of 20x60mm (width x length) with epoxy laminated glass fiber FR-4 as the substrate material whose dielectric constant is 4.7. Figure 2 shows the sectional view of the simulation model.



In Figure 2, the upper layer is wiring plane (micro-strip line plane) while the lower layer is image plane. Micro-strip line is an ideal conductor while image plane is an ideal conducting plane. The parameters of two parallel micro-strip lines can be set as: L=40mm, W=0.5mm, H=0.3mm. According to the formula of the characteristic impedance of micro-strip line ( ), the characteristic impedance of micro-strip line is 50Ω.


Note: 0.38mm


In Figure 3, the first port (P1) of emission line is the interference source port. Each port of emission line and receiving line is connected by the characteristic impedance (50Ω), so crosstalk signal will be absorbed when it reaches the near end and far end of receiving line and it won't return to influence crosstalk. As a result, two micro-strip lines form a 4-port network whose parameters S13 and S14 can be calculated respectively: , .


TR0 refers to the crosstalk of emission line to the near end of the receiving line while TRL refers to the crosstalk of emission line to the far end of the receiving line.

Simulation Result and Discussion

• Crosstalk intensity with the change of frequency


Ordinary signals are a result of the adding of sine waves with different frequencies and ranges so it's meaningful to study how crosstalk of two micro-strip lines changes with the frequency of a single sine wave.


To better reflect the rules, Figure 4 is obtained with wiring distance (D) with values of 1mm and 3mm, displaying how crosstalk changes with the frequency.



It can be concluded that in the range of low frequency, the intensity of crosstalk has a linear relation to signal frequency, no matter far-end crosstalk or near-end crosstalk. In the range of high frequency, near-end crosstalk (S13) shows the strong periodical vibration with the increasing of frequency while far-end crosstalk behaves contrarily. This mainly relies on the different distances between capacitive crosstalk and near/far end, between inductance crosstalk and near/far end. In the range of low frequency, the phases are mostly the same from these two types of crosstalk and ports and the relative phases of the integrated signal have little influence on extent. However, in the range of high frequency, under different frequencies, the phases have large differentials from these two types of crosstalk signal and ports when the extent of these two types of interference integrated signal will change periodically with the change of phase, which leads to the obviously periodic vibration of extent by frequency.

• Crosstalk intensity with the change of wiring distance


When the wiring distance (L) is 40mm, substrate thickness (H) 0.3mm and signal frequency 2GHz and 5GHz, the simulation result of the crosstalk intensity with the change of wiring distance is shown in Figure 5.



In this figure, both near-end crosstalk and far-end crosstalk decrease as the wiring distance becomes larger. When wiring distance starts to increase from 1mm, the crosstalk decreases quickly but with the increasing of the distance, the decrease of crosstalk becomes slow. Obviously, when the distance is larger than three times of the width, the crosstalk between lines can't be improved by enlarging the distance between lines. This is because when two micro-strip lines get too close, both mutual capacitance and inductance will become so prominent that crosstalk will substantially rise.

• Crosstalk intensity with the change of wiring length

When the wiring distance (D) is 2.0mm, substrate thickness (H) 0.3mm and signal frequency 1GHz and 5GHz, the simulated result of the crosstalk intensity with the change of length is shown in Figure 6.



According to Figure 6, when the signal frequency is 1GHz, the intensity of both near-end crosstalk and far-end crosstalk increase with the extension of parallel length. When the signal frequency reaches 5GHz, the intensity of near-end crosstalk increases with the extension of parallel length and the intensity of far-end crosstalk vibrates with the extension of the parallel length. This is because the electrical length of wiring is larger at the frequency of 5GHz than that at the frequency of 1GHz and phases of capacitive crosstalk and inductance crosstalk are substantially differential at the far-end port.

• Crosstalk intensity with the change of the distance between micro-strip line and image plane

In order to maintain the micro-strip line characteristic impedance at 50Ω, the value of W/H must be kept 1.82. Therefore, in the simulation model, the ratio between line width and the height of image plane is kept 1.82 as well.


a. When the wiring length (L) is 40mm, the distance between the two lines and their edges 1.0mm and signal frequency 2GHz and 5GHz, the crosstalk intensity with the change of image plane thickness is shown in Figure 7.



According to Figure 7, crosstalk intensity increases with the extension of the distance, especially when the distance is in the range of 0 to 0.4mm, the crosstalk intensity goes up so quickly and the speed tends to slow down with the continual extension of the height. When H is more than 0.5mm, crosstalk intensity basically remains still. This is because when micro-strip line is too near to image plane, decoupling between wiring and image plane becomes so integrated while decoupling between wiring is so small. When the distance between micro-strip line and the image plane increases, the decoupling between wiring and image plane becomes weak while decoupling between wiring rises. However, with the increasing of the distance between micro-strip line and the image plane, the decoupling between wiring and image plane has become so weak that it has little influence to the decoupling between wiring. Based on the analysis above, the distance between transmission line and image plane should be shrinked as much as possible so as to decrease the crosstalk better.


b. When the wiring length (L) is 40mm, distance between lines two times line width and signal frequency 2GHz and 5GHz, the crosstalk intensity with the change of image plane thickness is shown in Figure 8.



According to Figure 8, crosstalk intensity changes little with the distance between two lines multiple of the line width.


Based on the comparison between the two circumstances, it can be concluded that with the increase of the distance between micro-strip line and image plane, if the distance between lines remains unchanged, crosstalk intensity will be magnified and if the distance is the stable multiple of line width, crosstalk intensity almost remains unchanged.

Strategies of PCB Design

According to the analysis result above, some strategies are displayed below in order to decrease the crosstalk between transmission lines:
a. For high-speed digital PCBs, components whose clock rising edge and falling edge speed is relatively slow should be picked up so that the signal frequency can be decreased.
b. Long-distance parallel layout should be avoided.
c. The distance between two lines should be enlarged.
d. Multilayer PCB design should be used so that the height between transmission line and image plane can be decreased. If PCBs with higher image plane have to be used, the distance between transmission lines should be enlarged.


Helpful Resources
3 Routing Techniques on PCB High-speed Signal Circuit Design
High-Speed PCB Routing Techniques to Reduce the Influence of EMI
Suppression Method of Signal Reflection in High-Speed PCB Layout
Misunderstandings and Strategies on High-Speed PCB Design
7 Common Problems of High-Frequency and High-Speed Multilayer PCB Fabrication and Their Solutions
Full Feature PCB Manufacturing Service from PCBCart - Multiple Value-added options
Advanced PCB Assembly Service from PCBCart - Start from 1 piece

Default titleform PCBCart
default content

PCB successfully added to your shopping cart

Thanks for your support! We'll go over your feedback in detail to optimize our service. Once your suggestion is picked up as the most valuable, we'll instantly contact you in email with a $100 coupon contained.

After 10seconds Back Home