quick question regarding desgin guide - Page 1
Forum section: electronics / beginners

author: Write_to_Smokegenerator
author_rank: Regular Contributor
timestamp: June 28, 2012, 07:37:14 am
content: Hello everyoneI just read a PDF regarding high speed design:http://www.altera.com/literature/an/an224.pdfat page 12:"Use the following steps to reduce crosstalk in either microstrip or stripline layouts:?Widen spacing between signal lines as much as routing restrictions will allow. Try not to bring traces closer than three times the dielectric height."And that's what bothering me. If i recall it correctly on a 2 layer board the height is about 1.5mm and on a 4 layer board it is 0.45 mm.So on a 2 layer board the traces should be ca. 4.5mm away from each other (eurocard).On a 4 layer board the traces should be 1.5mm away from each other.That seems impossible.I happen to like this guide, allthough I knew most of the things before i read it.Would be nice if anyone can clear this up.cheers.

author: Electr0nicus
author_rank: Regular Contributor
timestamp: June 29, 2012, 12:44:20 am
content: HiI've searched some time on the internet and found some interesting info.First of all:Yes the calculations, that you need almost 4.5mm of trace distance for a proper crosstalk suppression on a 1.5mm FR4 PCB seem to be ok. There are some neat calculators on the web which show you.For example:http://www.eeweb.com/toolbox/microstrip-crosstalk/Also check out the other calculators they have:http://www.eeweb.com/toolbox/The thing is, that all these calculators do not take termination resistors into account. There are actually two types of crosstalk: forward crosstalk (as the signal travels from source to sink) and backward crosstalk (as the signal will be reflected from sink backwards to the source). As you can read in this PDFhttp://www.ultracad.com/articles/crosstlk.pdfon page 4 chapter "Termination"the Backward crosstalk is the part of crosstalk you have to worry about. If you terminate the signal line with a proper termination resistor, you can nearly eliminate the backward crosstalk which gives you a very improved crosstalk behavior of your circuit.To calculate the crosstalk, considering termination resistors, use this tool:http://www.ultracad.com/calculators/ultra_ct.zipFor example:A 100mm trace pair with 10mil (0.254mm) distance between each otherand a 1ns signal rise time on a standard FR4 PCB gives me with propertermination resistors a crosstalk coefficient of -30.7dB = 0.02916.This is for 5% Z0 and 1% Rt tolerance.If you have a signal voltage of 3.3V this means you get 3.3V*0.02916=0.09603Vcoupled in voltage. Which is quite down in the noise for a digital circuit.

author: free_electron
author_rank: Super Contributor
timestamp: June 29, 2012, 03:39:09 am
content: Quote from: Write_to_Smokegenerator on June 28, 2012, 07:37:14 amthose rules are correct. Your layer stack and width calcs are not ...nobody says the spacing needs to be even...for high frequency designs we typically use a 6 mils prepreg with a 45 mil core material and 1 ounce copper inner plus 1/2 ounce copper outer that gets grown to 1 ounce.so17+17 micron (1/1000 mm ) copper . 17 to start with , 17 grown during plating to end up with 35 microns post-plating6 mils prepreg35 micron copper45 mils core35 micron copper6 mils prepreg17+17 micon copper.Some factories can drop to 4 mils prepreg so then you can route denser.or you need to switch to a material with a different dielectric constant.you start with a doublesisded core that has thick copper. etching here is minima as these are the planes.laminate with prepreg and foil , drill , plate , dryfilm , imaging , developing , tinflash . filmstrip . etch . tinstrip -> post processing.nothing special. standard process.Your distance calcs are wrong too:if you route 4 mil tracks the distance between two tracks needs to be 12 mils ( 16 mils center to center ) in metric :you route a 100 micron track width so the gap needs to be 300 micron ( 400 center to center of the tracks )to get good couppling between a 4 mil track and the plane that pre-preg can't be thicker than 6 to 8 mils. a prepreg like you said ( even spacing from layer to layer ) doesn't do anything. you have no plane in that case ...as for a two layer board .. you can;t do this kind of stuff doublesided .. there's no coupling at all , or you need extremely thin substrates like in flex boards.You are reading or interpreting what is said in that document wrong:- to AVOID coupling ( so to avoid crosstalk ) the distance BETWEEN TRACES ( not the plane and the trace ! ) needs to be 3x the width of the trace ( 4x if you measure center to center ). the thickness of the dielectricum has notinhg to do with this...- to COUPLE to the PLANE you need to get below 1.5x the trace WIDTH. So for a trace of 4 mils you can not go above 6 mils pre-preg thickness. 8 mils is the limit ... beyon that there is no coupling and you have no transmission line.

author: Write_to_Smokegenerator
author_rank: Regular Contributor
timestamp: June 29, 2012, 07:50:36 am
content: Argh I'm an idot.... I now see my mistake -.-Thx for clearing that up.