How to get proper impedance specifications from PCB manufacturer.  - Page 1
Forum section: electronics / beginners

author: ziggyfish
author_rank: Regular Contributor
timestamp: May 17, 2017, 12:45:41 pm
content: HiI am trying to workout the correct trace width i need to use for my 50 ohm 915Mhz RF circuit. I tried contacting PCBCart and didn't get any useful information. Only that the constant is 4.2. When i chuck that number into an online co-planer calculator i get a track width of 0.25mm (pad size of chip) and a gap of around 0.1mm and a dielectric height of 0.195. I get an impedance of 56.21This pcb manufacturer doesn't support a smaller gap than 0.1 (0.052 would give me an exact 50 ohm impedance). What am i doing wrong?

author: AndyC_772
author_rank: Super Contributor
timestamp: May 17, 2017, 01:11:54 pm
content: Poor choice of PCB manufacturer, perhaps?You should be able to use a software tool to calculate the board stack-up and trace geometry you need. Prescribe the stack-up and dielectric materials as part of your drill drawing, specify clearly in your notes that the board must be controlled impedance, then find a PCB manufacturer with the capability to make it.A good supplier will be entirely familiar with this process. Controlled impedance boards are totally routine.

author: 8086
author_rank: Super Contributor
timestamp: May 17, 2017, 01:23:41 pm
content: Which online calculator are you using?TXLine says you have 50 ohms already.

author: dmills
author_rank: Super Contributor
timestamp: May 17, 2017, 01:35:37 pm
content: The usual issue with a lot of the budget fabs is that they are cagey about the layer spacing, because I think they tend to run with whatever cores and prepregs are cheap this month, so getting real information about what the stackup is that they are going to use is hard.This is IMHO a good enough reason to use the slightly more expensive sort of fab, and also to put a length of 50 ohm line on the panel with a footprint for an end launch SMA on each end, makes finding out what they have actually built somewhat easier, just hook up a VNA and measure.Regards, Dan.

author: AlfBaz
author_rank: Super Contributor
timestamp: May 17, 2017, 01:56:17 pm
content: Quote from: ziggyfish on May 17, 2017, 12:45:41 pmThat's a little weird. On their site they claim to be able to do high frequency boards and show you can use rogers ro3000 and ro4000 series laminates, not that they're needed here.My guess is their "standard" pcb manufacturing processes using fr4 haven't been characterized or, most likely, are inconsistent so even if you do a successful test coupon there may be no guarantee it will be the same for the next batch

author: T3sl4co1l
author_rank: Super Contributor
timestamp: May 17, 2017, 08:50:25 pm
content: You can't get 50 ohm traces, on 1.6mm PCB stock, with trace widths that will route into SMT pads.Typical trace width is about 30 mils.An SMT pin itself isn't a pure 50 ohms anyway. A little trace necking won't hurt anything.At ~1GHz, you have maybe 30mm of length before you care about impedance matching. Who cares?Alternately, you can change your system impedance to a higher impedance, like 100-150 ohms, and add matching where necessary.Tim

author: ziggyfish
author_rank: Regular Contributor
timestamp: May 18, 2017, 03:48:35 am
content: Quote from: 8086 on May 17, 2017, 01:23:41 pmI used:http://chemandy.com/calculators/coplanar-waveguide-with-ground-calculator.htm

author: ziggyfish
author_rank: Regular Contributor
timestamp: May 18, 2017, 04:24:02 am
content: Quote from: dmills on May 17, 2017, 01:35:37 pmWhat PCB Fab would you recommend?

author: dmills
author_rank: Super Contributor
timestamp: May 18, 2017, 10:29:58 am
content: Depends a lot on what I am doing, for prototype non critical boards with easy track and gap up to 4 layers or so, I just use the same Chinese fabs as everyone else.For prototypes boards with critical stackups or fine pitch/filled via/hard gold/small geometry I bite the bullet and use Wurth, expensive but they do make a very nice board, and at the end of the day knowing I can trust the board is worth something when trying to bring up a complicated prototype.Once I get to reasonable production runs it gets more complicated as I am usually trying to keep the bare board cost reasonable in relation to the rest of the BOM, if it has £600 of bits on it then who cares what the per board PCB cost is? If the board has only a few quids worth of parts however then you can tolerate a higher failure rate (And the thing probably does not have anything tricky) and whichever Chinese fab has not pissed you off recently becomes reasonable.It is always worth getting a 50 ohm line with a pair of footprints for SMA put on the panel somewhere if the board has any RF lines, so you can use a VNA to quickly verify the stackup is what you thought it was.Regards, Dan.