JLCPCB Impedance Calculator can't get 100R or 90R - Page 1
Forum section: electronics / general

author: run_the_race
author_rank: Newbie
timestamp: June 27, 2021, 11:14:24 am
content: Here's a link to the JLCPCB impedance calculator:https://cart.jlcpcb.com/impedanceCalculationGoing to route the following signals:100R differential pair (Zo = 50R)90R differential pair (Zo = 45R)Planning to use the stack up JLC7628, with a 4 layer PCB, in total 1.6mm thick.Step 1 Calculate singled ended impedance for each:Use "impedance + trace space" from top drop down box:Set Z=50R, click single ened, gives a result of track width = 11.55milSet Z=45R, click single ened, gives a result of track width = 14.04milStep 2 Calculate differential impedance:Set Z=100R, with widest spacing in dropdown box of 8mil, gives track width = 8.08milSet Z=90R, with widest spacing in dropdown box of 8mil, gives track width = 10.28milAs you can see one can't reach the required singled ended impedance for the differential pair. To reach the required single ended Z one needs a wider spacing, which one can't specifiy.Surely 100R and 90R are the most common values? What am I missing here?

author: asmi
author_rank: Super Contributor
timestamp: June 28, 2021, 07:48:22 pm
content: Quote from: run_the_race on June 27, 2021, 11:14:24 amDon't do that. JLC2313 stackup is MUCH better for high-speed design, because it allows for thinner traces and easier layout.Also requirement for differential impedance Rd does not necessarily imply requirement for Rd/2 for single-ended trace. In most cases single-ended impedance doesn't matter as much if differential impedance is correct.

author: run_the_race
author_rank: Newbie
timestamp: July 02, 2021, 05:21:01 pm
content: Quote from: asmi on June 28, 2021, 07:48:22 pmBut their website says "Recommended impedance: 10 - 66 ohm !" for JLC2313 when I try do impedance calculations.

author: asmi
author_rank: Super Contributor
timestamp: July 02, 2021, 06:09:42 pm
content: Quote from: evb149 on July 02, 2021, 05:34:21 pmThat kind of defeats the purpose of differential pair IMHO.

author: Styno
author_rank: Regular Contributor
timestamp: July 02, 2021, 06:28:13 pm
content: You can route a differential pair any way you like on a pcb, as long as the time the signal needs to reach the receiver is about the same for both traces. They don’t have to be routed (closely) together, although that is often the easiest way. Route them on different layers or opposite ends, it doesn’t matter, on a pcb they are both single transmission lines.This is the case because the ground/reference plane captures almost all the fields, there is hardly any field interaction between the two traces. Provided you use a good stackup where the plane is only a thin prepreg away from the signal layer, of course.Edit: fix mobile autocorrect errors

author: asmi
author_rank: Super Contributor
timestamp: July 02, 2021, 07:15:26 pm
content: The coupling is what's allowing for the differential impedance of a pair to be lower than than of two of individual traces. I've seen many-many boards with differential traces, and can't remember a single case when they are routed far apart as to not allow any coupling. Typical distance between traces in a pair is 1H-2H, and that's the way they always are routed.Try routing two independent 45 Ohm traces, and then a diff pair of 90 Ohm diff impedance with traces 0.1-0.2 mm apart, and compare those two solutions. I think advantage of close-coupled diff. pair will become super-obvious.

author: asmi
author_rank: Super Contributor
timestamp: July 02, 2021, 11:45:31 pm
content: Quote from: evb149 on July 02, 2021, 07:35:20 pmThat's no longer the case for at least a couple of years now. JLCPCB offers 4 layer stackup JLC2313 with 0.1 mm prepregs and controlled impedanceat no extra cost. You can have five 10x10 cm 4 layer boards for ~$20 delivered. And they can make down to 3.5/3.5 mil traces and 0,2/0.4 mm vias. That is more than enough for a lot of cases. Check a project linked in my signature for one example of what kind of boards you can make with that process.One thing that really sucks is that a stackup JLCPCB offer for 6 layer boards sucks for high speed designs due to very thick cores. If they instead would've used thick prepreg in the middle with 0.1mm cores, it would be much better. As it is, 6 layer PCBs with controlled impedance and custom stackup goes for $150-$200 for ten at WellPCB. They are of much higher quality, but you pay for it.

author: HQ
author_rank: Newbie
timestamp: June 10, 2025, 06:30:31 am
content: Although this post is quite old, it’s still very helpful for beginners like me. I’m currently comparing results using different tools, and I’ve noticed that even with the same parameters, different manufacturers’ impedance calculators give different results. This might be because each tool reflects the manufacturer’s own production experience and assumptions. I have used:JLC calculatorhttps://jlcpcb.com/pcb-impedance-calculatorNextPCB impedence calculatorhttps://www.nextpcb.com/pcb-impedance-calculatorPCBway calculatorhttps://www.pcbway.com/pcb_prototype/impedance_calculator.html

author: thm_w
author_rank: Super Contributor
timestamp: June 10, 2025, 09:38:55 pm
content: Quote from: HQ on June 10, 2025, 06:30:31 amhttps://www.reddit.com/r/PrintedCircuitBoard/comments/18m1kqy/which_impedance_calculator_thats_available_for/