High speed differential pairs (impedance) - Page 1
Forum section: electronics / projects

author: sw_guy
author_rank: Regular Contributor
timestamp: February 09, 2024, 06:17:35 am
content: hi,I am experimenting 1G lan design (=adding 1G LAN interface to a processor). How much I need to consider impedance matching? Based on typical rules, the impedance between signal layer and ground layer below is 100R. To make that happen software suggest to have 4mils trace width and about 4 mils distance. That is pretty small - and taking into account PCB manufacturers economical dimensions, I would like to stay min 6mils.I have done pair length matching, but traces are not even near as close as 4 mils.sw guy

author: ch_scr
author_rank: Frequent Contributor
timestamp: February 09, 2024, 07:19:21 am
content: See if you have a groundplane "further down". The traces will grow wider the further the distance to gnd. You might have to via-stitch the "trench".

author: selcuk
author_rank: Frequent Contributor
timestamp: February 09, 2024, 07:50:01 am
content: It should be 100 ohm differential impedance. It is not from a single signal trace to ground layer as in microstrip line. What is the height between the signal layer and ground plane below it? If you calculate 4mil + 4mil, the height should be 6mils. I think you can design with 6 mil track spacing.

author: sw_guy
author_rank: Regular Contributor
timestamp: February 09, 2024, 11:02:18 am
content: PCB is 4 layer and I have set the thickness between signal and ground layer to 2.8 mils. Based on calculation 6/6 routing gives 79R impedance.Now when I think this further, 2.8 mils is probably too small. I contacted to the PCB manufacturer and the (default) thickness is as much as 14.1 mils. Using that, trace width and clearance are ~6-7 mils. That sounds like realistic, right?I think that for impedance matching PCBs, the thickness of dielectric is somewhere between 6-9 mils (?)sw guy

author: selcuk
author_rank: Frequent Contributor
timestamp: February 09, 2024, 12:31:31 pm
content: I've calculated your values in Saturn PCB Toolkit. 2.8 mil height, 6/6 mil tracks, 1oz pcb with 4.4 er. Differential impedance is about 67 ohms. You need to make the calculations according to the manufacturer's data. If they don't have 2.8 mil prepreg thickness, you may try to design with 14.1 mils.Let's assume this is the manufacturer's impedance data (jlcpcb.com/impedance) :https://jlcpcb.com/impedanceAnd let's choose basic 4-layer setup (1st one). There is a prepreg layer 7628*1 between top layer and inner layer 1. Er is 4.4, thickness is 0.2104mm (~8.3mil). From the calculator, track width is 8 mils and spacing is 6 mils and the differential impedance becomes 101.5 ohms.You can match the impedance with a 2-layer board having a thickness of 1.6mm but the tracks become very wide so that you may not prefer to use.

author: sw_guy
author_rank: Regular Contributor
timestamp: February 09, 2024, 01:51:30 pm
content: Thanks. I get the same answer using values you mentioned.Now the remaining problem is to understand how to wire 1Gb RJ45 connector with magnets...I am not sure how to connect J1 and J10...sw guy

author: coromonadalix
author_rank: Super Contributor
timestamp: February 09, 2024, 05:39:44 pm
content: why double posting ? you end up showing the same picture on your other thread ?

author: sw_guy
author_rank: Regular Contributor
timestamp: February 09, 2024, 07:16:32 pm
content: Quote from: coromonadalix on February 09, 2024, 05:39:44 pmReally? Same image on two messages.