Differential impedance calculation - Page 1
Forum section: electronics / general

author: Vilius
author_rank: Contributor
timestamp: April 16, 2023, 09:15:04 am
content: Hi,I am doing my first PCB design on USB 1.0/1.1, thus first time dealing with the differential impedance. I did my research on what the differential impedance is and how should I approach it. I have a 2 layer 1.6 mm board that I want to create a 90 Ohm profile on. I used the Altium`s impedance profile calculator and got the parameters, but then I double checked with a Saturn PCB tool - the results were significantly different. I may be missing something as it is my first time dealing with it, but which program should I really trust? Is there any other solution to get reliable results? Thank you in advance.

author: hanakp
author_rank: Regular Contributor
timestamp: April 19, 2023, 01:42:43 pm
content: Yes, this is normal. Vast majority of calculators like Saturn PCB use simple equations from 1960s which can't account for edge effects etc. I don't know what algorithm Altium employs internally, but when I compare results from Saturn and professional tools like ANSYS Designer TRL or AWR TXline, I routinely get >10% difference. And the smaller S and H, the worse Saturn results get.Having said that, I think you have Saturn configured wrong, you set 35 um base copper thickness and another 35 um of plating on top of that?

author: thm_w
author_rank: Super Contributor
timestamp: April 19, 2023, 09:15:19 pm
content: Do you have Altium setup for single or differential?https://www.altium.com/documentation/altium-designer/configuring-layer-stack-controlled-impedance-routing?version=21I'm not sure which Z it is giving you. If it is Zo (single), its not far off from the Saturn value of ~99 ohms.Either way, USB1.1 is forgiving enough that either value used should work fine.

author: Vilius
author_rank: Contributor
timestamp: April 19, 2023, 09:38:29 pm
content: Saturn gives me 2 numbers: Zdifferential and Zo (they are different.) Do you know what is the difference between those? Also I removed the plating cooper setting (made it 0) Saturn`s result changed only by 1.5 Ohm...

author: thm_w
author_rank: Super Contributor
timestamp: April 19, 2023, 09:57:31 pm
content: Zdiff is differential impedance between two traces.Zo is single ended impedance, just the one trace and your ground plane.You'll need to specify in Altium which one you are looking at, as per the link above.https://resources.altium.com/p/differential-pair-impedance-using-calculator-design-your-pcb

author: Vilius
author_rank: Contributor
timestamp: April 19, 2023, 10:22:23 pm
content: Zo is really the sign for single ended impedance? I know what single ended impedance is, but ideally, single ended impedance should be 45 Ohms is my goal is to have Zdiff of 90 Ohm, this Saturn thing keeps getting worse and worse xd

author: thm_w
author_rank: Super Contributor
timestamp: April 19, 2023, 10:45:04 pm
content: Please read the links above, and use the tooltips in Saturn.Your goal is Zdiff 90, not Zo 45

author: nctnico
author_rank: Super Contributor
timestamp: April 21, 2023, 03:42:36 pm
content: Ideally you'd need 2 lines with Zo =45 Ohms. On a 1.6mm PCB you are looking at traces nearly 3mm wide and then you'll need distance between them to make differential pair... It will be hard to get this PCB designed and likely the rule-of,thumb formulas used by Saturn are way outside their usefull limits. A better option is to use a 4 layer pcb with thin dielectrics between the outer and inner layers.

author: Damperhead
author_rank: Contributor
timestamp: May 29, 2023, 06:45:10 am
content: I wouldn't worry too much about the impedance. I would try to keep the differential wiring as short and clear as possible and the return current path as good as possible. It can be challenging with 2-layer PCB. However, you will probably have to add protection components between the differential pair, so the impedance will hardly be the desired 100 Ohm +/-10% on the transmission lines.

author: Sagar
author_rank: Contributor
timestamp: July 23, 2024, 04:48:04 pm
content: various impedance calcualtors are there but I will always recommend to use the one given by the PCB manufacturer because they know the quality, core, prepag much more then a random tool. You can find the listed one in the capabilities section, or on web listed by them.example:https://jlcpcb.com/pcb-impedance-calculator