Copper pour for differential pairs - Page 1
Forum section: electronics / beginners

author: fabiodl
author_rank: Frequent Contributor
timestamp: November 19, 2023, 02:07:35 pm
content: I just finished watchingIt was immensely informative. But there was one aspect was not mentioned. If we have signal plane and a ground plane below, should I do a copper (GND) pour on the signal plane or is it better not to?I imagine there will be additional coupling between the copper pour and the traces.Intuition would suggest that it is then better to leave a gap between the pair and the copper pour. How much should this be? For instance x times H (the distance between the signal and ground layer). How much is this x?

author: tooki
author_rank: Super Contributor
timestamp: November 19, 2023, 03:29:50 pm
content: First of all, the key thing is that if your differential signals are fast (which is often part of why they’re differential to begin with), they’ll require impedance-controlled conductors, (cables, connectors, and traces).Forget the differential aspect for the moment, as this applies whether it’s single-ended or differential:There are numerous types ofplanar (flat) transmission lines. Here are the ones you’re basically describing:- If you have a ground plane, and your signal trace above it on the signal plane without a ground pour, it’s called a microstrip.- If you have your signal trace on the signal plane, with a ground pour (but without a ground plane below it!) it’s called a coplanar waveguide (CPW).- If you have a ground plane, and your signal trace above it on the signal plane with a ground pour, it’s called a coplanar waveguide with ground (CPWG).In every case, the dimensions are intimately tied to the impedance control. The dimension over which you have the least control is the thickness of the dielectric (the PCB substrate between your signal and ground planes). You have some choices from your PCB manufacturer, but the available thicknesses are what you have to work with. Similarly, the thickness of the PCB trace is something over which you have only limited control. You have no control over the thickness of solder mask and silkscreening, other than whether you have your traces covered or not,What you have full control over is the width of the trace and the width of the gap between the trace and a ground pour, and between the traces in a differential pair.IIRC, the thicker the dielectric, the wider the signal traces and the wider the gaps between differential traces, and the wider the gap between signs all traces and ground pours.Altium has a quite good impedance control calculator that uses a field solver to calculate these quite accurately. First, set your PCB layer stack correctly, since this is key to getting accurate impedance calculations. Then you create an impedance profile for your required impedance (e.g. 90 ohms for USB, 50 ohms single-ended or 100 ohm differential for typical RF stuff, etc). It’ll calculate something for you, and you can either use it as-is, or you can manually set a value and have it adjust the others to match. Alternatively, your PCB house may provide you with optimized values for their impedance-controlled PCB services. (But beware, they may not be accurate: at my previous job we did some testing, and discovered that the PCB house’s values were wrong, and Altium’s were practically perfect). Then you use parameter sets and rules to assign the impedance profile to the relevant nets.KiCad has an impedance calculator as a separate tool, and there are numerous online tools too. These aren’t as advanced as Altium’s but will be close enough for almost all purposes.As for your original question of whether to pour ground around a differential pair or not (in other words, whether to use a microstrip or a CPWG): microstrip (no ground pour) is usually better. If you need a ground pour for other reasons, you may have no choice. But there’s no one-size-fits-all answer, and sometimes you’ll need a different transmission line type altogether.

author: twospoons
author_rank: Frequent Contributor
timestamp: November 19, 2023, 11:04:28 pm
content: What you are describing would be a differential coplanar waveguide with ground, I don't think I've ever found a formula for that one. Best to keep the signal layer ground pour clear of the diff pair. Rule of thumb for the ground pour on your signal layer is to make a clearance at least five times the dielectric thickness. That should minimise the impact on your differential pair. But as always with any rule of thumb: use with caution.

author: fabiodl
author_rank: Frequent Contributor
timestamp: November 19, 2023, 11:34:38 pm
content: Quote from: twospoons on November 19, 2023, 11:04:28 pmThank you. Would you suggest actually putting the copper pour, with a 5H clearance, or leave it out altogether?In the specific case, I am dealing with HDMI signals. I plan to use JLC04161H-7628https://jlcpcb.com/impedanceas a stack layout

author: tooki
author_rank: Super Contributor
timestamp: November 20, 2023, 04:50:51 pm
content: There are plenty of concrete requirements and recommendations for HDMI layout. Beyond impedance control, length matching is important too.https://ez.analog.com/video/w/documents/687/hdmi-layout-guidelinehttps://e2e.ti.com/cfs-file/__key/telligent-evolution-components-attachments/00-138-01-00-00-10-65-80/Texas-Instruments-HDMI-Design-Guide.pdfIt looks like HDMI is 100 ohm differential. Given the high clock speeds, you’ll want the ground plane close, so you want a PCB stack up with a thick core and thin prepreg between outer layers. (If I recall correctly.)TI says to use “shield traces”, ideally ground, with a “scattering” of vias to the ground plane below. They say to make the gap between signal trace and shield (d) greater than 3x the gap between the signal traces (s). The TI document even includes the formulas for calculating reasonable approximations of the geometry. However, I’d just let your PCB layout software do it.I’ll add that it’s super important that the ground plane below the signal traces be unbroken. Do not run other traces through it. At high frequencies like this, the signal return wants to occur directly below the signal traces, so any breaks create a loop you don’t want.

author: twospoons
author_rank: Frequent Contributor
timestamp: November 21, 2023, 04:18:01 am
content: This is a section of LVDS routing on a board I am currently working on - quite similar to HDMI in that it uses 100 ohm diff pairs, requires length matching and runs at a bit rate of ~500Mb/s. The board is four layers - this bit has two ground layers as I have LVDS routing both sides. Note the outer layer ground pour is pulled well back from the signals and via stitched around the edges. The sexy curves are not really necessary but I like them.This is from a working, tested design.Note that those two chunks of ground pour (blue layer), that look like blobs on a stick, should really be via stitched into the ground planes or removed, as they have the potential to act like patch antennas and radiate noise. But the are small, and so far they have not proved to be a problem.

author: fabiodl
author_rank: Frequent Contributor
timestamp: November 22, 2023, 08:23:32 am
content: Quote from: twospoons on November 21, 2023, 04:18:01 amThank you, this is exactly what I am looking for.By the way, using jlcpcb calculatorhttps://jlcpcb.com/pcb-impedance-calculator/and the standard stackup JLC04161H-7628single ended impedance of 50 ohms gives 13.75 mils (0.3493 mm). Isn't it very thick? Your pcb traces do not seem to be that thick

author: twospoons
author_rank: Frequent Contributor
timestamp: November 22, 2023, 11:08:24 pm
content: We're not using JLPCB, so our stackup will be different to yours. The example I've shown uses the recommended width and gap from our PCB supplier (0.29mm trace, 0.41mm gap). Dielectric thickness and dielectric constant can make a huge difference to trace and gap widths.

author: fabiodl
author_rank: Frequent Contributor
timestamp: November 28, 2023, 08:42:47 am
content: Got it, thank you!