Abstract:
A two-layer printed circuit board (PCB) having impedance control is provided. The two-layer PCB includes: a substrate; a plurality of transmission lines laid on the substrate for transmitting high-speed signals, each of the transmission lines having a standard impedance; and at least one ground trace laid on the substrate adjacent each of the transmission lines, for controlling a characteristic impedance of each of the transmission lines to equal or approach the standard impedance.

Description:
BACKGROUND OF THE INVENTION  
       [0001]     1. Field of the Invention  
         [0002]     The present invention relates to a printed circuit board, and particularly to a two-layer printed circuit board achieving impedance control and a method of achieving impedance control when high-speed signal transmission lines are laid on the two-layer printed circuit board.  
         [0003]     2. Background  
         [0004]     Signal integrity is an important factor to be taken into account when a printed circuit board (PCB) is designed. A well-designed PCB has an elevated on-off switching speed of integrated circuits, and a high density, compact layout of components. Parameters of the components and of the PCB substrate, a layout of the components on the PCB, and a layout of high-speed signal transmission lines all have an impact on signal integrity. In turn, proper signal integrity helps the PCB and an associated computer system to achieve stable performance. Impedance matching is considered as an important part of signal integrity. Therefore a characteristic impedance of a transmission line is designed to match an impedance of a load associated with the transmission line. If the characteristic impedance of the transmission line is mismatched with the impedance of the load, signals arriving at a receiving terminal are apt to be partially reflected, causing a waveform of the signals to distort, overshoot, or undershoot. Signals that reflect back and forth along the transmission line causing “ringing.” 
         [0005]     Parameters that have an impact on the impedance of the transmission line include a width and a thickness of a copper wire or trace of the transmission line, a dielectric constant and a thickness of a substrate of the PCB, and a thickness of each of a bonding pad, a trace of a ground wire, and other peripheral traces. An experiential formula used to calculate the impedance of a transmission line is as follows:  
         Z   0     ≈       87         ɛ   r     +   1.41         ⁢   ln   ⁢           ⁢       5.98   ⁢   H         0.8   ⁢   W     +   t             
 
 Where Z 0  is the characteristic impedance of the transmission line, ε r  is the dielectric constant of an associated PCB substrate, W is the width of the transmission line, t is the thickness of the transmission line, and H is the thickness of the substrate. A four-layer PCB achieves impedance control via a framework that includes the transmission line and a reference ground plane adjacent the transmission line. Referring to  FIG. 1 , the four-layer PCB includes transmission lines  100 , substrates  110 ,  130 , and two ground layers  120 . According to the standard dimensions of PCB manufacturing, H is 4.4 mil, t is 2.1 mil, and ε r  is 4 for a standard 4 layer structure. If a width of the transmission line is 5 mil, the impedance of the transmission line is 54.7 ohms. This figure approaches a standard value for achieving impedance matching; that is, 60 ohms. In addition, simulation software is also available to calculate the impedance of the transmission line. A section plan of the transmission line, the substrates, and the ground layers are inputted to simulation software. Then simulation software analyses an electromagnetic field caused by the transmission line and the ground layers, and calculates the impedance of the transmission line. 
 
         [0006]     A two-layer PCB used for an input/output card is manufactured without ground layers in the substrate, in order to achieve reduced costs. However, a layout of the conventional two-layer PCB is not standardized. Generally a relatively large unused area of the PCB has copper applied thereto, which serves as ground. Therefore impedance matching is hard to achieve.  FIG. 2  shows the conventional two-layer PCB. The two-layer PCB includes a transmission line  150 , a ground layer  160 , and a substrate  170 . A thickness of the substrate  150  is 56 mil. If a width of the transmission line  150  is 5 mil, a value of a characteristic impedance of the transmission line  150  is calculated to be 150 ohms. If the characteristic impedance of the transmission line  150  is to approach a standard impedance of 60 ohms, the width of the transmission line  150  would need to be 82 mil, which is a most unreasonable requirement. When using simulation software, it is hard to control the characteristic impedance of each of the transmission lines  150 , because the section plan includes a plurality of transmission lines  150  and only one ground layer  160  to refer thereto.  
         [0007]     What is needed, therefore, is a two-layer PCB which is able to achieve impedance control with a reasonable layout. What is also needed is a method for achieving such impedance control.  
       SUMMARY  
       [0008]     A two-layer printed circuit board (PCB) having impedance control is provided. In a preferred embodiment, the two-layer PCB includes: a substrate; a plurality of transmission lines laid on the substrate for transmitting high-speed signals, each of the transmission lines having a standard impedance; and at least one ground trace laid on the substrate adjacent each of the transmission lines, for controlling a characteristic impedance of each of the transmission lines to equal or approach the standard impedance. Hence, the impedance of the transmission lines is calculable without any necessary integral metal plane (grounded or powered) forming in the PCB.  
         [0009]     A method of providing impedance control for a two-layer printed circuit board is also disclosed. The two-layer PCB includes a substrate and a plurality of transmission lines laid on the substrate for transmitting high-speed signals. The method comprises the steps of: (a) laying at least one ground trace on the substrate adjacent each of the transmission lines; (b) inputting a section plan of the two-layer PCB to simulation software; (c) calculating a characteristic impedance of each of the transmission lines via the simulation software; (d) comparing the characteristic impedance calculated in step (c) with a standard impedance; (e) if the characteristic impedance calculated in step (c) does not equal or approach the standard impedance, adjusting any one or more of parameters of the section plan, and returning to step (b); and (f) if the characteristic impedance calculated in step (c) equals or approaches the standard impedance, performing a layout of each of the transmission lines and the ground trace according to the last-input parameters.  
         [0010]     The two-layer PCB is capable of achieving impedance control of each of the transmission lines, so as to achieve signal integrity for the two-layer PCB.  
         [0011]     Other advantages and novel features will become more apparent from the following detailed description of preferred embodiments when taken in conjunction with the accompanying drawings, in which: 
     
    
     BRIEF DESCRIPTION OF THE DRAWINGS  
       [0012]      FIG. 1  is a section plan of a conventional four-layer PCB;  
         [0013]      FIG. 2  is a section plan of a conventional two-layer PCB;  
         [0014]      FIG. 3  is a section plan of a two-layer PCB in accordance with a first preferred embodiment of the present invention; and  
         [0015]      FIG. 4  is a section plan of a two-layer PCB in accordance with a second preferred embodiment of the present invention. 
     
    
     DETAILED DESCRIPTION OF THE EMBODIMENTS  
       [0016]      FIG. 3  shows a section plan of a two-layer PCB in accordance with a first preferred embodiment of the present invention. The two-layer PCB  3  includes a plurality of single transmission lines for transmitting high-speed signals. The two-layer PCB  3  includes a single transmission line  10 , a substrate  20 , two ground traces  30 , and a plurality of low-speed signal transmission lines  40 . The ground traces  30  and the single transmission line  10  are laid on a same plane level of the substrate  20  side by side, with the ground traces  30  being adjacent opposite sides of the single transmission line  10  respectively. A thickness of the ground traces is equal to a thickness of the single transmission line  10 , the thicknesses generally being 2.1 mil. In order to control the impedance of the single transmission line  10 , the section plan as shown in  FIG. 3  is inputted to simulation software, such as a 2D Extractor. Simulation software analyses an electromagnetic field caused by components of the section plan, and calculates a value of the characteristic impedance of the single transmission line  10 . If the calculated value does not equal or approach a required standard value for the two-layer PCB  3 , one or more of the following parameters are adjusted: a width w and a thickness t of the single transmission line  10 , and a spacing s between the single transmission line  10  and each of the ground traces  30 . Then another section plan defined by the adjusted parameters is inputted to simulation software, and the characteristic impedance of the single transmission line  10  is recalculated. Such processes are repeated if necessary until the calculated value equals or approaches the standard value, thus obtaining a group of proper parameters including w, s, and t, which achieve the desired impedance matching. Then the layout of the single transmission line  10  and the two ground traces  30  is performed according to the proper parameters.  
         [0017]     If only one ground trace  30  is laid adjacent only one side of the single transmission line  10 , parameters achieving the desired impedance matching can also be obtained via simulation software. Using only one ground trace  30  is simple and inexpensive. However, in the first preferred embodiment using two ground traces  30  respectively laid adjacent opposite sides of the single transmission line  10 , the single transmission line  10  is more effectively insulated from other transmission lines. Besides, the impedance of the transmission lines is calculable without any necessary integral metal plane (grounded or powered) forming in the PCB.  
         [0018]      FIG. 4  shows a section plan of a two-layer PCB in accordance with a second preferred embodiment of the present invention. The two-layer PCB  5 , applied to transmit USB (Universal Serial Bus) 2.0 signals, includes a differential transmission line  50  for transmitting high-speed signals, a substrate  60 , two ground traces  70 , and a plurality of low-speed signal transmission lines  80 . The differential transmission line  50  includes two componential transmission lines  52  and  54 . The transmission lines  52  and  54  are uniformly spaced apart, have a same length, and transmit signals in mutually opposite directions. The ground traces  70  and the differential transmission line  50  are laid on the substrate  60  side by side, with the ground traces  70  being adjacent opposite sides of the differential transmission line  50  respectively. A thickness of the ground traces  70  is equal to a thickness of the differential transmission line  50 , the thicknesses generally being 2.1 mil. In order to control the impedance of the differential transmission line  50 , the section plan as shown in  FIG. 4  is inputted to simulation software. Simulation software analyses an electromagnetic field caused by components of the section plan, and calculates a value of the characteristic impedance of the differential transmission line  50 . If the calculated value does not equal or approach a required standard value for the two-layer PCB  5 , one or more of the following parameters are adjusted: a width W and a thickness T of the differential transmission line  50 , a spacing K between the transmission lines  52  and  54 , and a spacing S between the differential transmission line  50  and each ground trace  30 . Then another section plan defined by the adjusted parameters is inputted to simulation software, and the characteristic impedance of the differential transmission line  50  is recalculated. Such processes are repeated if necessary until the calculated value equals or approaches the standard value, thus obtaining a group of proper parameters including W, S, K, and T, which achieve the desired impedance matching. Then the layout of the differential transmission line  50  and the two ground traces  70  is performed according to the proper parameters.  
         [0019]     It is believed that the present embodiments and their advantages will be understood from the foregoing description, and it will be apparent that various changes may be made thereto without departing from the spirit and scope of the invention or sacrificing all of its material advantages, the examples hereinbefore described merely being preferred or exemplary embodiments of the invention.