Printed Circuit Design & Fab - May 2008 - (Page 22)

FIGURE 5. The resonant frequency occurs when the reflected signal from the end of the stub is 180 degrees delayed and cancels out the signal through the via barrel. FIGURE 4. SPICE simulation of a simple via stub model. Blue trace is the long via, with no stub, and red trace is the short via with long via stub. There are no losses in the model. the most common answer offered in signal integrity, “it depends” – on the barrel diameter, clearance hole size, presence of non-functional pads, and spacing between the planes. However, for most typical design rules, the via impedance will range from 30 to 70 ohms. Given its short length, typically less than 200 mils, even this wide range of impedance has only a small impact on a signal. The signal degradation introduced at a via is not from the via barrel path, but from the stubs connected to the ends of the via barrel. Add a 30-Ohm stub that is 200 mils long to a short via and the insertion loss can drop by more than 30 dB, dramatically affecting transmitted signal quality. FIGURE 4 compares the simulated insertion loss of a 200 mil long, 30 ohm via with no stubs, to a short via (from layer 1 to layer 4) with a 200 mil long via stub. There is a huge reso- nant dip at the frequency where the length of the stub is one quarter of a wavelength. Any frequency components of a signal near this resonant frequency will be completely blocked by the via stub. Stub Length and Resonant Frequency The high frequency behavior of a via is dominated by the interference caused by the transmitted signal, along with the signal that reflects off the bottom of the stub. This is illustrated in FIGURE 5. The signal incident to the via is traveling down the 50 ohm impedance of the top signal line. The signal enters the via and hits the ‘T’ intersection where the signal splits. About half the signal travels down to the second signal layer, following in the wake of the initial signal heading to the receiver. The two signals traveling in the forward direction to the receiver will interact with each other. If the extra path length the signal took in going down the via stub, reflecting and coming back up the via stub (a round trip delay) is half a cycle, then the two signals traveling to the receiver will be out of phase and they will subtract. The frequency where this first resonance occurs is when the round trip delay of the stub is half a cycle. This corresponds to a resonant frequency of f = 1.5/Len, with the frequency in GHz and the via stub length in inches. If the resonant absorption from the via is to have little impact on the transmitted signal, then its resonant frequency must be much higher than the bandwidth of the signal in the data stream. The bandwidth of the signal is the Nyquist frequency, which is roughly one-half times the bit rate. For the via stub to have no affect on the transmitted signal, the resonant frequency of the stub should be much higher than the signal bandwidth. As a rough rule of thumb, if BR equals the bit rate in Gbps, this means f > ~ 10 x ½ x BR, or via stub length, in mils < 300/BR. A 10 Gbps data stream should have all stubs of less than about 30 mils in its signal path. Optimizing Stubs The first step in minimizing the impact from stubs is to keep their length as short as possible. In a multilayer board, one way of keeping stub lengths short is by limiting the signal layer transitions. In an extreme case, high-speed signals will only be routed on the top and bottom layers so that any via between these layers will have no stub at all. 22 PRINTED CIRCUIT DESIGN & FAB MAY 2008 http://www.pcb-pool.com/ppus/info.html?PHPSESSID=7df48fa7c977776045ff8d4b24a70fc7 http://www.pcb-pool.com/ppus/info.html?PHPSESSID=7df48fa7c977776045ff8d4b24a70fc7

Table of Contents Feed for the Digital Edition of Printed Circuit Design & Fab - May 2008

Printed Circuit Design & Fab - May 2008 Contents Our Line Market Watch Around the World Happenings ROI EMC For the Real World PCB East Conference Brochure Positive Plating Don't Let your Signals Stub Their Toes Improve PCB Layout With Skill Utility Programs The Next Generation Design Tool Challenge Thermally Conductive Microwave Materials PCB Dielectric Degradation in Lead-Free Assembly Applications A Tale of Two Trade Shows Eliminating Board Defects Off the Shelf Marketplace Ad Index BGA Bulletin

Printed Circuit Design & Fab - May 2008

For optimal viewing of this digital publication, please enable JavaScript and then refresh the page. If you would like to try to load the digital publication without using Flash Player detection, please click here.