About Track Impedance in High Frequency Applications

This is the space to ask all your burning tech questions and discuss the Skills Bright Sparks competition. We are here to help!
timchpi
Posts: 31
Joined: Wed Aug 01, 2018 11:19 am

About Track Impedance in High Frequency Applications

Post by timchpi » Sat Nov 17, 2018 6:31 pm

Hey guys Tim here
So I am working on another controller board for my 3D printer.
I am now working with raspberry pi CM module cus well it have a real good processing power and guess what Atmega644P on 8 MHz just couldn't cut it.
So anyway I came to the design of USB cus well I need wifi and what I found on datasheet that is real sad is:

Code: Select all

The USB port (Pins USB DP and USB DM) must be routed as 90 ohm differential PCB traces.
So I did some googling and it turns up to be related to something called ... Track Impedance?
And I am now completely lost.

Can anyone with experience on working with High-Frequency Applications with Specific Track Impedance required give me a hand on this?
Much Appreciated.

Thanks
Regards
Tim Here

Microman171
Posts: 7
Joined: Fri Aug 29, 2008 4:50 pm

Re: About Track Impedance in High Frequency Applications

Post by Microman171 » Mon Nov 19, 2018 8:38 am

Hi Tim,

I work for a company that specialises in wireless electronics - and I have plenty of experience with controlled impedance! The fastest signal you will see on USB 2.0 is 480 Mbps - which isn't all that fast in the grand scheme of things. This is fortunate, because the slower the signal the easier it is to control - you don't need to be so careful on length matching. Routing D+ and D- next to each other would be enough to get the length right.

To control the impedance of these USB tracks, you need to control the spacing between them the spacing to the ground plane (on the same layer) and the height above the ground plane (on the layer below). I'll assume you will be using standard FR4 PCB material - and there's no reason not to for USB 2.0! The other critical thing is that your USB signals do not cross plane boundaries - i.e. you don't route anything on the layer directly below. This can be tricky in two layer designs, but it can certainly be done.

I'm happy to review your board layout when you're ready.

Kind regards,
Dan

timchpi
Posts: 31
Joined: Wed Aug 01, 2018 11:19 am

Re: About Track Impedance in High Frequency Applications

Post by timchpi » Mon Nov 19, 2018 8:41 pm

Hey dan:
Glad to hear from you.
Yeah I see you point. Comparing with Wi-Fi running at 5800MHz the 480Mbps on USB2.0 is really not that fast.
However I am I'm high school NCEA Level 2 if it starts to explain a little why is it really hard on my behalf - I don't have the basic knowledge to cut it.
Ok so there are a few points you made if I get it right:
Route them close to each other, and make sure that their length match up as much as possible;
Control the distance between track, from track to ground, and from track to back of the board, which is fixed 1.6mm norm isnt it?
And not to route anything below USB line, so it shall be plain ground with nothing on it.

So I have a few questions:
1. Does it matter to have a DC line(like VCC) instead of GND under the data line?
2. Does it matter to not have copper pour under the data line or do I have to have copper pour?
3. Do I need to add caps to the D+ and D-?
4. I see that on datasheet of RPi-CM3, USB is required to be 90 ohm differential PCB traces. However, nothing has been stated on DSI(Display Serial Interface) and CSI(Camera Serial Interface). On the other hand, on the schematic of the official CMIO v1.1, DSI and CSI are declared to be

Code: Select all

matched length 100R differential pairs
which got me confused: When datasheet doesn't say anything but reference design does, do I need need to take that into account? Plus, on behalf of DSI and CSI itself, should I use matched length track with controlled impedance or do I not need to care at all? Especially the I^2C port inside DSI and CSI is also declared as matched length track with controlled impedance, which I have seen no where else. By contrast, interestingly, the SD seems to not have any requirement relates to length matching and impedance control at all.

Thanks
Regards
Tim

Microman171
Posts: 7
Joined: Fri Aug 29, 2008 4:50 pm

Re: About Track Impedance in High Frequency Applications

Post by Microman171 » Tue Nov 20, 2018 11:06 am

Hi Tim,

I'm not familiar with the DSI and CSI interfaces specifically. Are you planning on using them in your end application? If so, I'll try to do a bit of research to make sure I don't give you bad advice!

What tool are you using to design your board? I use Altium, and that makes differential impedance control pretty easy. CircuitMaker is a free version that might suit your needs - it may not control impedance for you but you should be able to set routing rules to control the trace spacing. EAGLE, on the other hand, makes this a bit tricky - but certainly achievable for something like USB 2.0.

To answer your questions:
1. You can use any potential (GND, VCC, etc) under your bus as long as it doesn't cross boundaries (i.e. traces over GND for the first half and VCC for the second would be bad practice).
2. I think you could get away without the pour under the tracks (just remember to account for this in your impedance calculation), but you will need to keep all other high-speed signals further away to avoid interference. I recommend just putting a ground pour on the layer below, and adjacent to the tracks.
3. No. You also don't need to add series resistors usually - these are to reduce the slew rate and I don't remember these being necessary for USB high-speed. If the reference design has them, add them!
4. See above. I'm not familiar with DSI/CSI, but I'll look into it if you're planning on using this in your design.

If there's one piece of advice I could have had early on, it would be "stick to the reference design as far as practicable"! This is especially true for the high-speed areas of the design (which includes the power supply decoupling caps). I've been bitten on some 5 GHz designs where they didn't perform as well as I had expected due to deviations!

For I2C, this is typically only going as fast as 1 MHz. 1 MHz isn't super fast so as long as you don't have cross talk, and as long as there isn't too much capacitance, you should be fine. Worst case, you can usually turn the speed down because it's a control interface (normally, anyway). Your traces would need to be really long before you had issues at 1 MHz!

From memory, SDIO can go up to 60 MHz, but SD was more like 25 MHz. 60 MHz is "reasonably" fast, but 25 MHz isn't really anything to worry about. Especially for the point-to-point wiring you'll probably be using. Even in 4bit mode, the clock rate is only 25 MHz (but the data rate is x4, as you have a 4 bit bus).

Kind regards,
Dan

timchpi
Posts: 31
Joined: Wed Aug 01, 2018 11:19 am

Re: About Track Impedance in High Frequency Applications

Post by timchpi » Tue Nov 20, 2018 2:10 pm

Hey dan:
Thanks a lot for that.
So uh, yeah. I will probably do a bit of research on myself about CSI and DSI, but i would definitely appreciate it if you could look it up as well - i guess there would be a lot of stuff that you will have a way more solid understanding comparing to me.
Uh ... the CAD I'm using is KiCAD, actually. Its free its open source its great in general. I have never heard of circuitmaker before? I do know Eagle and Altium though ... and proteus ... but uh ... circuitmaker definitely sounds like a excellence choice ... its just I still do not understand why did they make a free version available ... and what are the restrictions and license and stuff ...
And for number 3 i mean capacitors by cap ... I see a few design that have them on high speed rails.
And uh ... If I am using 1oz 1.6mm FR-4, plain GNDREF on other side, what would the preferred track width and space between them be?
And how much does the soldering joint effect the impedance?

Anyway I really really really apperciate your help. Thanks a lot.

Regards
Tim

Microman171
Posts: 7
Joined: Fri Aug 29, 2008 4:50 pm

Re: About Track Impedance in High Frequency Applications

Post by Microman171 » Tue Nov 20, 2018 3:38 pm

Hi Tim,

If you're happy using KiCAD then there's nothing wrong with that! From what I understand, KiCAD has push/shove routing which makes life easy (because you can route the first track, then drag the second close to the first). In EAGLE, this is a bit annoying to do. I'm not a huge fan of CircuitMaker, but the routing is better than when I used EAGLE.

For question number three, there's no need to add series/shunt caps to your USB data traces. These are probably also for EMI reduction or slew rate control. If the reference design has them then add them :)

I'll assume you're using a two layer FR4 board with 1.6 mm between 1 oz copper layers and a dielectric constant of 4.6 - which is what you get unless you ask for something special. My calculator says to use 1 mm wide tracks with a 0.2 mm gap between them! Normally you'd want to use a 4 layer board (which also makes the ground plane a bit easier) and have 0.25 mm between top layer and the next layer down. This gets your width down to 0.3 mm with a gap of 0.2 mm.

I wouldn't worry about the solder joints. Any effect here is going to be negligible. If you need series/shunt components on the data lines, you'll want to look at using 0603 or smaller (1608 in metric terms).

Kind regards,
Dan

timchpi
Posts: 31
Joined: Wed Aug 01, 2018 11:19 am

Re: About Track Impedance in High Frequency Applications

Post by timchpi » Thu Nov 22, 2018 5:00 pm

Hey Dan:
So uh ... what would happen if the impedance is too high or too low?

Thanks
Regards

Microman171
Posts: 7
Joined: Fri Aug 29, 2008 4:50 pm

Re: About Track Impedance in High Frequency Applications

Post by Microman171 » Fri Nov 23, 2018 11:51 am

For the RF signals I deal with, it acts as a big attenuator (i.e. we waste a bunch of power). For high-speed digital signals it will reduce your signal-to-noise ratio by reducing your signal level (a.k.a. attenuation) and increasing your noise level (from reflections). The general term you could research is "signal integrity" issues. The other affect you will probably observe, and maybe not care about, is EMC issues and EMI susceptibility. Your transmission lines will radiate in a way that prevents you from selling the design as a product (legally), and other devices may interfer and stop your product from working as expected.

For USB full-speed (12 Mbps), you would probably get away without controlling impedance because the data rate is too low to be affected. For USB high-speed (i.e. USB 2.0), it really does need to be carefully controlled (within 15%). You'll observe reduced data rates in the best case, and you'll see an unstable connection (where it works some of the time) in the worst case. Unfortunately you don't get much control over the choice of high speed or full speed. If the USB host and device both support high speed, they will attempt to make use of it.

My recommendation would be to use a 4 layer board if you want USB high-speed.

timchpi
Posts: 31
Joined: Wed Aug 01, 2018 11:19 am

Re: About Track Impedance in High Frequency Applications

Post by timchpi » Fri Nov 23, 2018 7:01 pm

Hey microman:
Ok so ...
1. How do i know if my design is valid enough so it does not radiate illegally?
2. Is the effect of having a lower than expected impedance same as higher than expected?
3. Will it have a better effect if I have a piece of ground in middle of the two data line or will it make it not work at all?

Thanks

Microman171
Posts: 7
Joined: Fri Aug 29, 2008 4:50 pm

Re: About Track Impedance in High Frequency Applications

Post by Microman171 » Sun Nov 25, 2018 3:16 pm

Hi Tim,

1. Follow best practices and hope for the best. The only way to know is to get a test lab to measure it for you. If I were you, I would only worry about this if you're making a product. Nobody is going to beat down your door unless you make a large number of them with the intention of selling.
2. Yes - the mismatch will cause you problems when it's too low or too high.
3. You could probably calculate what would happen with a ground plane between the traces, but I would recommend not doing so. USB is a differential bus and relies on having both traces next to each other for better common-mode noise rejection. In simpler terms, you get a better quality signal when they're adjacent.

I recommend biting the bullet and going for a 4 layer design. Managing the ground plane will be easier, the trace widths will be manageable, and you'll probably find routing everything else will be much easier too.

Post Reply