Connector suggestion for PCBs spaced ~40mm apart (USB & 5V@1.25A)

[SgtSiff]

I'm looking for suggestions for connectors to connect two PCBs that are 39.7mm apart. It needs to carry USB data lines, as well as power (5V, 1.25A).

Because of the odd spacing, I'm guessing a board to board connector is out of the question so it will have to be a cable of sorts. Researching this has led me down the path of ZIF connector + FFC cable.

If I used the Wurth 686606050001, I could use two conductors for 5V, two for GND, and the remaining two for the data lines which seems OK, but:

Is there something more suitable? I can find suitable 90 ohms impedance matched ZIF connectors (Panasonic Y5BH), albeit in 0.5mm pitch which is something I could work around by using more conductors to meet the current requirements, but I'm struggling to find 90ohm FFC cables. For such a short distance, do I need to worry at all? I got the idea from the RevPi connect, which seems to use a 100mm FFC cable to connect two PCBs with Wurth 687118182122 ZIF connectors, which don't seem to have any mention of impedance control. Picture of the assembly can be seen here: https://www.rs-online.com/designspark/revolution-pi-by-kunbus

Also an additional question, for those who have used these cable in a design before, where can I find information about minimum bend radius of the FFC cable? The datasheet doesn't seem to mention anything. I tried to model it with the 50mm long Wurth FFC and came up with this:



It's a bit crude, but gives a rough idea as to what the bend radius would look like.

[T3sl4co1l]

Could also do square-pin header, that's just over-long, and use thru-pin (stackable) sockets to mate it.  Heh, assuming the boards can be stacked axially, of course this wouldn't work so well if they're slid in separately or something...

What EMI environment is this like?  Is the surrounding structure just plastic, or does it provide any shielding/grounding?  Do both boards have cables attached or anything?

Putting USB over open, unshielded connections like these (ribbon, FFC, pin headers, etc.) is a bit iffy.  It may be desirable to add a ferrite bead or something, or shielding (which can be a foil backing, if it can be mated to both boards), or extra grounds (to the same end, just around the boards, rather than around the cable).  Or extra filtering if it only needs to be USB Full Speed (12Mbps), not High Speed; not really great, but it's a little something.

As for the cable, both for bend radius and for ease of assembly, I might suggest using horizontal connectors, preferably near the center of the boards if that space is available, so it's facing out and accessible.  Bend radius should be in the datasheet, if not it's typically 5mm or something like that?

Tim

[ajb]

Well, there's USB and then there's USB, so it makes a difference if you need Hi-Speed (480Mbps) versus Full-Speed (12Mbps) or Low-Speed (1.5Mbps).  It also makes a bit of a difference if this cable will be the continuation of an external connection (like, host PC -> regular USB cable -> PCB1 -> FFC -> device on PCB2) or strictly internal (host on PCB1 -> FFC -> device on PCB2).  In the latter case you can get away with more than in the former. 

In most cases, I think you'll be fine with full-speed or lower with a standard 0.5mm pitch FFC if this is a one-off, but it might be marginal if this is a commercial endeavor.  Here's a paper looking at impedances of off-the-shelf cables, differential impedance with 0.5mm unshielded polyester FFCs was measured at 100R: https://meritec.com/wp-content/uploads/2014/03/FFC-Impedance-Tests.pdf

Impedance controlled FFC are available, but probably expensive and/or with a substantial MOQ, but an alternative could be to design your own FPC with whatever impedance you want.  The same connectors you'd use for FFCs will work with FPC as well.

As far as bend radius, that depends on the specific FFC, and whether the bending is one-time or continuous.  Some cables are thicker than others, which means that they resist bending more but also are going to experience more strain when bent to a given radius than their thinner counterparts.  It's not terribly uncommon to see flat flex cables actually folded to fit in a tight space or to turn a corner, this is not really ideal but can be okay as long as it's folded once and left like that forever.  Something that needs to flex intermittently will need a larger radius, and continuous flex will need a larger radius still.  We have an Epilog laser engraver here that uses a long FFC to carry the encoder signals on the X-axis, so it flexes hundreds of times per job, and it has probably a 10mm radius with a 180° bend?

[SgtSiff]

What EMI environment is this like?  Is the surrounding structure just plastic, or does it provide any shielding/grounding?  Do both boards have cables attached or anything?

EMI nightmare Both PCBs have nice long dangly extraneous wires in the form of ethernet, ModBus and DI/DO. However all of the interfaces are fully isolated with their own properly filtered isolated supplies. I don't know what effect this will have, if any, I need to do more research on this before it goes for testing, but it's just me working on this project

Putting USB over open, unshielded connections like these (ribbon, FFC, pin headers, etc.) is a bit iffy.  It may be desirable to add a ferrite bead or something, or shielding (which can be a foil backing, if it can be mated to both boards), or extra grounds (to the same end, just around the boards, rather than around the cable).  Or extra filtering if it only needs to be USB Full Speed (12Mbps), not High Speed; not really great, but it's a little something.

Well, there's USB and then there's USB, so it makes a difference if you need Hi-Speed (480Mbps) versus Full-Speed (12Mbps) or Low-Speed (1.5Mbps).  It also makes a bit of a difference if this cable will be the continuation of an external connection (like, host PC -> regular USB cable -> PCB1 -> FFC -> device on PCB2) or strictly internal (host on PCB1 -> FFC -> device on PCB2).  In the latter case you can get away with more than in the former. 

Shielding is a concern, especially as this will be in an industrial environment. The USB connection is Hi-Speed 480MBps and it is strictly internal.

Taking a step back, do you think a reasonable approach would be to use a standard two layer PCB with a vertical USB connector on each end? I've got a RPi LCD that uses one of these:



But instead of HDMI, I could use USB A or even C.

[JohnnyMalaria]

For fear of missing something, what about:

[SgtSiff]

Think I'm going to go with this setup, can anyone see any potential problems?

Can get them manufactured for $0.40 (100 qty) each. $1 including all of the connectors. This will need to pass EMC btw.

1mm 2 Layer PCB. Diff traces are 0.865mm wide, 0.254mm spacing. Solid ground plane on back.

[Mecanix]

Vibration and user handling considerations required, otherwise I can't see why this wouldn't work, logically anyway.

Also an additional question, for those who have used these cable in a design before, where can I find information about minimum bend radius of the FFC cable? The datasheet doesn't seem to mention anything. I tried to model it with the 50mm long Wurth FFC and came up with this:

Normally/easily carried with a simple Nastran SOL101 (linear static), I see from the visuals that you have a seat of SW... solver should be included? Ensure stress/strain does not exceed the core material given yield (+ a good 10% safety), and that's your bent max.

[Mecanix]

Sure I'll be flamed beyond all hells for saying this; if data integrity isn't of paramount importance a 100mm fpc set-up will(should) work just fine for usb. Completely different story for e.g. mil, aerospace or medical obviously. Good set of series termination resistors tweaked at both ends and off you go

[T3sl4co1l]

Yeah, that's probably fine.  At worst you could add some bypass caps (+5V/GND), one at each connector say.  Pop option if it fails EMC, perhaps.

Or kinda more likely a CMC might be something to put in there, a bit harder to configure though.  Best way for that I think, two data line chokes, with one winding each common to GND, the other to USB_DP/M, and just a ferrite bead in series with +5.  Annoying to jumper out, because you need jumpers in that case (0 ohm resistors), it's a BOM adder either way.  Perhaps more of an alternative design option, in case you find the thing needs a ferrite bead (see if you can clip a ribbon cable style FB around it, or just a big enough round or square FB, to test this possibility).

Tim

[KE5FX]

USB is differential.  You have to try hard to screw it up (and believe me, the PC OEMs do.)  A few centimeters of FFC at Zo=90 or 100 ohms will be fine.   Just surround the D+/D- pair with ground traces. 

Source: Lots of experience doing just this, at 480 Mb/sec. 

With respect to EMC testing, the real threat is the external cable back to the PC, where manufacturers like to cut corners with shielding.  Bring a few different ones to the test lab. 

[SgtSiff]

USB is differential.  You have to try hard to screw it up (and believe me, the PC OEMs do.)  A few centimeters of FFC at Zo=90 or 100 ohms will be fine.   Just surround the D+/D- pair with ground traces. 

The FFC in the RevPi is almost 100mm long and it seems to have passed all EMC tests so I can certainly believe this. In your experience, do you think I would need to go with something like the Molex 15021-0215, which is shielded and has controlled 100R impedance, or would a standard 0.5mm FFC be OK? By the way, there is no external cable, it connects to a USB hub on the second PCB.

Frustratingly, in the doc it seems to imply there is a 90R option , but there is no part number or anything that I can find:

[Mecanix]

I think you'll need a 1.00mm pitch (minimum) for 1.25A

[SgtSiff]

I think you'll need a 1.00mm pitch (minimum) for 1.25A

I was planning to use more than one conductor, so like:

5V 5V GND GND D+ D- GND GND 5V 5V

I forgot to reply to you earlier btw, It's Fusion 360 now SW, and I have zero experience with FEA unfortunately.

[Mecanix]

oh I see, yep that will work plenty.

As per KE5FX's recommendation:
12P 0.5mm: 5V 5V GND GND D+ GND GND D- GND GND 5V 5V
6P 1.0mm: 5V GND D+ GND D- GND
Same phy size both option anyway... all down to how much micro-management we all comply too

And my god, that strangely look like a version of SW... those identical shadows and edges smoothing effects lead me to this confusion.
RE exp: if you model and create assemblies you'll eventually need to find the time to get training on for at least linear static (mass/force, stress & strains), and safety factors in considerations of the tolerances of your manufacturer(s). Bare minimum man. Plan a good month or two in advance... all good fun (not)!

[SgtSiff]

Thanks Mecanix, I guess I jsut have to decide which path to take now that I have two options

Being an EE i've always been a little scared of dipping my toe into FEA.. but you're right, I moved to F360 from just Eagle as I have been finding myself doing more and more Mechanical design in projects now and the integration is nice.. I guess learning FEA and CAM is the next step.

[Mecanix]

Cool stuff. Hope it all works out, post the grand finals so we can all confirm that's the way to go (advantages!)

Side note; I'm nothing short of a beginner in EE being in my third year only. ME (by profession) and flooding in EE capabilities as much as I humanly can, not easy and a pretty steep learning curve I tell ya. (sincere respect to the knowledgeable guys here).

FEA mandatory for prod design, unfortunately (e.g. bolt preloading, material thermal expansion and relevant stresses aka prevent premature cracks and other failures). Nothing worst than a prod recall and/or losses by warranty claims. CAM will greatly help you to design-for-manufacturing and machinability. Also mandatory I'll add.

All the best, Sergeant! 🥂🥂

[KE5FX]

USB is differential.  You have to try hard to screw it up (and believe me, the PC OEMs do.)  A few centimeters of FFC at Zo=90 or 100 ohms will be fine.   Just surround the D+/D- pair with ground traces. 

The FFC in the RevPi is almost 100mm long and it seems to have passed all EMC tests so I can certainly believe this. In your experience, do you think I would need to go with something like the Molex 15021-0215, which is shielded and has controlled 100R impedance, or would a standard 0.5mm FFC be OK? By the way, there is no external cable, it connects to a USB hub on the second PCB.

Frustratingly, in the doc it seems to imply there is a 90R option , but there is no part number or anything that I can find:

I use standard 0.5mm FFC.  It looks like the parts you mentioned are qualified for USB 3 SuperSpeed operation at 5 Gbps, so they would certainly be fine for any USB 2 applications.  The distinction between 90 and 100 ohms is unlikely to matter except in situations that are already so marginal that they could be hosed by any number of other factors.  The USB 2 impedance tolerance appears to be +/- 15% according to a quick Google search, so either 90 or 100 would be permissible as long as the cable itself lives up to its specs.

Edit: another pedantic point to bring up is that some manufacturers discourage circumvention of their conductor current limit specs by paralleling multiple conductors.  There is often a separate spec for total current carried by all conductors in the cable, and it's usually surprisingly low.  If/when one of the paralleled conductors starts to get flaky, the others have to shoulder its load, which of course is likely to cause the rest of them to fail in succession. 

You can bend the rules as long as you know what to expect, but I wouldn't go as far as to simply multiply the cable's max current rating by the number of conductors.  I'd set it up so that if half of your the conductors open up completely, the remaining ones are still at or below their rated current limit.  It sounds like your 4x 5V scheme complies with that, if the cable spec is 500 mA per conductor as is common.  If the current spec is less than 500 mA/conductor, then 4x power+4x ground might be a little aggressive.

As per KE5FX's recommendation:
12P 0.5mm: 5V 5V GND GND D+ GND GND D- GND GND 5V 5V
6P 1.0mm: 5V GND D+ GND D- GND
Same phy size both option anyway... all down to how much micro-management we all comply too

I don't personally put a ground trace between the D+ and D- lines since they're supposed to be referenced to each other differentially.  If you wanted to look into the whole even- versus odd-mode impedance topic, you could start here, but the bottom line is that they don't expect you to use a central ground.  The main idea behind putting the traces next to each other is common-mode immunity, and running a ground line down the middle certainly won't help there.

[T3sl4co1l]

http://www.ediss-electric.com/SI-TDR_investigations/fleximpedance.pdf

It's probably better without the ground: GSG giving ~80 ohms (~40 CM, ~160 DM -- in reality these will be closer together as the middle ground makes a poor shield) versus GS+S-G giving 116 ohms diff and unstated CM (probably not very far below 80).

Neither is a great match, so there would be some benefit to a custom cable, at least over longer lengths or where greater signal quality is required.

I'd stick with GSSG.

Tim