So what does 'Impedance controlled PCB' mean from a manufacturing point of view? - Page 1
Forum section: electronics / general

author: TheUnnamedNewbie
author_rank: Super Contributor
timestamp: April 15, 2020, 05:02:08 pm
content: So, I'm not all that familiar with PCB manufacturing past simple PCBs. I come from a circuit design background, and I am starting to think that PCB manufacturing might not work the way I thought it did.A lot of manufacturers will offer something along the lines of 'Impedance controlled PCB'. What exactly do they mean by this?I always assumed you would get the exact stackup (up to the letter - decide on manufacturer and weave type and thickness), and then use your calculator or simulator to decide what the trace width/gap should be for your impedance.But today I have chatted with some people who work on the more mass-manufacturing/production side of things, and they seemed to imply (but there was no time to go into this) that they just told the manufacturer 'Here be 50 ohm transmission line' and the manufacturer would adapt the width to the specific dielectric thickness/type they happened to use.So what does 'Impedance control' mean in this context?

author: jmelson
author_rank: Super Contributor
timestamp: April 15, 2020, 05:29:38 pm
content: Quote from: TheUnnamedNewbie on April 15, 2020, 05:02:08 pmWell, they need to tightly control layer thickness and Er (dielectric constant) and give you those numbers.Also, as frequencies move higher, they have to worry about the fiberglass fill ratio and the way the weave is laid down.QuoteIf you hand off the rough design to a design house to layout the board, that will work. I don't know any PCB fabricator that will go in and tweak the thickness and width to get specific impedances, but maybe with everything going to higher freq. there are outfits that will do that.Jon

author: free_electron
author_rank: Super Contributor
timestamp: April 15, 2020, 05:36:07 pm
content: impedance control means you work cosely with the board fab to define a stackup , material selection , copper foil selection and then you do you part of the work : using the provided information you set trace width and spacing.During manufacturing they do tight control to make sure the layer thickness is respected. They nject coupins ( test structures) in the border of the panel where they verify that a panel is indeed yieldeing the desired impedance. if something were to go 'off' in the process ( overetching / underetching , via plating abnormality , surface plating abnormality , layer mismatch , too much butter ( yes, that's a term .. ) on the prepregs , problems during hot press )they can trap this and scrap the panel. The coupons are inserted at various locations and they test those before they ship the boards. if the coupons pass , the boards will be correct ( provided you did the trace/space correct )

author: Alex Eisenhut
author_rank: Super Contributor
timestamp: April 27, 2020, 05:26:49 pm
content: I was going to write a book-length reply but free_electron nailed it succinctly.Basically let the shop decide what they need to do to achieve your goal and follow it.I can even take a picture of such a panel with test coupons in my private reserve, if you want.

author: GerardG
author_rank: Regular Contributor
timestamp: April 28, 2020, 07:43:00 am
content: As already been written above.PCB factory will change your trace width, if needed. This means you already need to be pretty close to the design.Per production panel a coupon is placed and measured. This is an optimal designed trace and coupling as per your design.The coupon will tell the manufacturing company if etching and plating are correct.Your requested copper thickness will always have a tolerance, same to the copper width. Top of the trace has a other width as the bottom has.What you need to do in your design.1. talk with the PCB company and discuss the stackup.2. Calculate the trace width for the impedance's you need.3. Let the PCB company look at your trace calculations and comment to this.4. Finalize your design. Keep copper away from your impedance traces, otherwise you get edge coupling. Most of the time >0.3mm will be enough to have minimum influence.This will be a big task because sometimes you have to cross traces or go between some pads.Expect your trace not to be optimal on Impedance, just be smart about it.