Advice on a custom USB device

[xylo04]

Hi folks! I'm a software engineer by day and a radio amateur, but I dabble in electronics. I'm working on a OSHW project right now which is basically meant to cram several USB devices into one.

The project is published at https://github.com/k0swe/tx500-data-interface.

To interface a ham radio with a computer for digital modes, you generally need two things:

• a serial UART for controlling frequency, mode, transmit/receive, etc, and
• a duplex audio signal for received and transmitted digital data (very similar to a modem).

Right now I accomplish this with an FTDI cable and a cheap USB sound card plugged into a hub. I want to make a rugged device that has a USB hub controller, UART and audio chip integrated on one PCB. The closest consumer device to compare this to is the Yaesu SCU-17.

I have a design started in KiCad, but this is only my second custom PCB, and it's the first design I've done with ICs and USB buses. I'm eager to get advice on anything that can be improved, but I have a couple of specific concerns:

• Are my uses of power regulation, decoupling caps, signal filtering, etc appropriate? I followed the application notes for my hub controller and UART, but I'm not an EE and don't actually know what I'm doing.
• The audio chip I'm using, the Cmedia HS-100, doesn't have application notes in its datasheet. I currently have minimal supporting circuitry around it. Do I need to add anything obvious? There's some debate in the amateur radio community in general about adding transformers to audio lines like this.

If it helps, I'm trying to optimize for simplicity, small size and ruggedness. This is meant to be in use near RF, but right now I'm only targeting low power operation (QRP), which is 10 W or less of transmitted RF. This is not a consumer device, so I'm currently dispensing with overcurrent and ESD protection. Let me know if I'm going to regret that!

[teksturi]

Usually it helps if you give us pdf or jpg straight to this site. People are lazy and do not bother to open someone else project files especially when they do not even know if they are interested. This way you will get more input. 

I look your schematic a little bit, but it was too hard to check because it was 6 pages. This would probably fit one A4. That will make it more readable. You can still split one A4 to sections and write headers to thous. Of course this is little bit personal preference but I think no one puts just one usb connector to one A4 page.

[xylo04]

Thanks for the meta-advice. Bad habits from programming.

I've restructured the schematic and attached it here. I couldn't quite fit everything on one page, but it's down to two.

[teksturi]

Thanks for the meta-advice. Bad habits from programming.

I've restructured the schematic and attached it here. I couldn't quite fit everything on one page, but it's down to two.

I try it and it will fit. How does this look? I still leave it upto you if you wanna do this. But still very good start   

[xylo04]

Thank you, that looks very good!

Any advice on structural changes?

[elias]

The design looks fine to me, I'm just a bit concerned about the way you are mixing the Left and Right channel outputs. I would either expose both channels individually or mix them using a pair of resistors, if not a an OP-Amp.

But I'm no expert in this matter, what you are doing may be perfectly fine, just pointing it out so maybe somebody with greater knowledge can comment.

[teksturi]

These are just best of my understanding and can be totally false claiming.

U1 needs decoupling capacitor.

USB hub port needs 120uF as it is minimum required (USB specification)
100uF was reference design but thous where low ESR tantalums.

You didn't have datasheet for TPS76333

You do not have capacitor at VOUT at TPS76333 (Check datasheet)

You might even change design that you do not have TPS76333 at all.
FT232 can make 3V3 so you can use that to power TUSB2036.
Datasheet says you can draw 50mA from that and TUSB2036 use 40mA.
I do not know how much J2 other end draws.

It will be close and is up to you to decide if you wanna use this.
If this is my design. I would design it so that I can use both ways.
Just add 0ohm resistor from FT232 output to 3V3 rail. If this not
work then populate TPS76333. Remember to still add needed caps.

I think usb shields should be connected together. Other wise when
you connect some random device with long cable it.

I really like idea that FT232 external supply voltage can be
selectable. See datasheet section 6.4. You can use 0ohm resistor
to jumper. Of course this is just idea and I would probably do
this this way. Also if you have room in your pcb add leds for tx
and rx. You do not even have to populate these but if something is
not working you can populate them.

I check these quickly. Check them again
MUTEP should be pulled low
VOLUP should be pulled low
VOLDN should be pulled low
DR maybe pull up? Good idea to make it easy to change after.
MUTER should be pulled low

Add led also for this. I think you have much room in your pcb.

I also think that XREGXX pins may need caps. Else they can even
oscillate. Good idea to be safe and caps there. No need to populate
right away. If you know you do not need them please leave them away
put it wasn't sure to me.

Add test point for 3V3.

Example U2 cap between trace and pins are super low. You have room so
make it bigger. Same thing with many places. No need to use minimum
what your pcb manufacturer say. That is minimum for reason. When you
do it like this (minimum caps) you are playing game which you can
ether draw or lose. Do not play that game

You have lot of room in your pcb. Redo your designators. Maybe every
text can be even right way. Maybe also add better pin 1 indicator for
ic's.

Be careful with your mounting holes. Right now they are in F.mask layer.

There might be lot of other things. But this was just small checking hope
it helps.

[mon2]

My 2 bits:

1) the ESD protection devices on the USB lines is missing - review the TI ESDS312 - amazing device with high levels of protection.

2) when the time comes to the PCB layout, be sure to note that you must apply impedance controlled traces for the USB 2.0 HS lines. Many articles on the internet on this subject. Your PCB shop should be able to support this requirement of 90 ohms and validate with a TDR report.

3) Why are there caps on the D+ and D- lines? This may be a violation of the USB spec. Have never used them in any of our designs for USB 1.1 / 2.0 / 3.1 to date.

4) Consider to insert an EMI filter on the USB lines like from Littlefuse, etc. You can source them locally to get started and migrate to offshore when the  volume picks up at a fraction of the cost.

Here are some (dated) offers on these filters:

We like to offer below

KC p/n.WCM-2012-900T
Price USD0.04/pc FOB Taiwan
SPQ=3000pcs/reel
MOQ=36000pcs per shipment
LT=30days
 
Above p/n. is for USB 2.0 application

If you need USB 3.0 common mode choke, we will suggest to use KC p/n.WCM-2012HS-900T   spec as attached file fyr


Rex Chen
Your Best EMI Solution Partner

鈞寶電子工業股份有限公司／King Core Electronics Inc.
O.Phone: +886-3-4698855#201
e-mail: rex@mail.kingcore.com.tw
Address: 台灣桃園市平鎮區南豐路269號／No.269, Nanfong Road, Pingjhen City, Taoyuan County 324, Taiwan

Above is from Kingcore (Taiwan).

5) As you are using only the TX & RX lines for the USB serial port - you could reduce this chip down to the very low cost device from WCH.

Review CH340N (8 pin SOIC; no xtal required) @ $0.50 USD or less in single qty.

http://wch-ic.com/products/CH340.html

If you select the USB to Serial bridge properly, then it will be possible to install on Windows 10 / MAC, etc. without a driver if the bridge is a 'CDC Class' device. Best to review the datasheet for this confirmation. You can also check Maxlinear (aka Exar) USB Uarts.

Cannot recall if the WCH CH340N is CDC or not at this time but they offer a mix of such solutions.

6) U4 LDO is not enabled as the EN pin is floating. It should connect to VIN to enable.

7) TI is a good company but there are other competitive and more mature options like Microchip who purchased SMSC and SMSC was a great and pioneering company for the USB markets. Do review their USB hub offerings as well. You can also consider offshore brands but did not really find the savings to be great so better to stay with Microchip, etc. brands.

[xylo04]

Many thanks to those who responded!

I'm just a bit concerned about the way you are mixing the Left and Right channel outputs...

I'm doing this currently by tying L and R inside the audio and it does work, but I don't actually know that this is a good way to do it. Looking for further input here.

U1 needs decoupling capacitor.

Assume you mean on USB port 0? Added C19

USB hub port needs 120uF as it is minimum required (USB specification)
100uF was reference design but thous where low ESR tantalums.

Modified C11, C16 and C17 from 100 to 120.

You didn't have datasheet for TPS76333

Added to repo

You do not have capacitor at VOUT at TPS76333 (Check datasheet)

Added C18

You might even change design that you do not have TPS76333 at all.
FT232 can make 3V3 so you can use that to power TUSB2036.
Datasheet says you can draw 50mA from that and TUSB2036 use 40mA.
I do not know how much J2 other end draws.

It will be close and is up to you to decide if you wanna use this.
If this is my design. I would design it so that I can use both ways.
Just add 0ohm resistor from FT232 output to 3V3 rail. If this not
work then populate TPS76333. Remember to still add needed caps.

Interesting idea! I think for now I'll stick with using the TPS76333, but I'll make a note to try this in the future. https://github.com/k0swe/tx500-data-interface/issues/6

I think usb shields should be connected together. Other wise when
you connect some random device with long cable it.

Added GND1 as a case ground. On the PCB this includes an exposed strip that should contact with the enclosure.

I really like idea that FT232 external supply voltage can be
selectable. See datasheet section 6.4. You can use 0ohm resistor
to jumper. Of course this is just idea and I would probably do
this this way.

Added https://github.com/k0swe/tx500-data-interface/issues/7 to track this suggestion, thanks!

Also if you have room in your pcb add leds for tx
and rx. You do not even have to populate these but if something is
not working you can populate them.

Added https://github.com/k0swe/tx500-data-interface/issues/8 to add LED footprints for both FT232R and HS-100B.

Add test point for 3V3. ... Maybe every text can be even right way. Maybe also add better pin 1 indicator for ic's.

Fixed designator directions and pin 1 indicators

Be careful with your mounting holes. Right now they are in F.mask layer.

Actually, I don't have mounting holes since I'm using a slide-in enclosure. I think you're seeing the fiducials for aligning the solder paste stencil.

Many thanks! I'll keep working on these suggestions!

[xylo04]

1) the ESD protection devices on the USB lines is missing - review the TI ESDS312 - amazing device with high levels of protection.

Added U6 and U7. I was going to go without them and still might mark them as "optional" but at least having pads for ESD protection makes sense. I added them to the two USB ports as well as the UART TX/RX and audio SPKR/MIC, hopefully that's appropriate.

2) when the time comes to the PCB layout, be sure to note that you must apply impedance controlled traces for the USB 2.0 HS lines. Many articles on the internet on this subject. Your PCB shop should be able to support this requirement of 90 ohms and validate with a TDR report.

I will try to follow this if possible. I'm using KiCad's differential traces which seem to try to do this.

3) Why are there caps on the D+ and D- lines? This may be a violation of the USB spec. Have never used them in any of our designs for USB 1.1 / 2.0 / 3.1 to date.

They're shown in the TUSB2036 application notes. If I can get away without those that would be great; I'm using larger parts and they take up a lot of real estate.

4) Consider to insert an EMI filter on the USB lines like from Littlefuse, etc. You can source them locally to get started and migrate to offshore when the  volume picks up at a fraction of the cost...

Thanks for the tip. I might skip this for V1, but assuming this works for my low-power radio application, I will probably need to harden it for use in high-RF environments.

5) As you are using only the TX & RX lines for the USB serial port - you could reduce this chip down to the very low cost device from WCH. Review CH340N (8 pin SOIC; no xtal required) @ $0.50 USD or less in single qty....

Thanks again for the part recommendation. I am concerned about having this install with as little friction as possible. Again, I'll probably stick with FTDI for V1 since I know it's a high-quality part but I'll have to circle back on that.

6) U4 LDO is not enabled as the EN pin is floating. It should connect to VIN to enable.

Fixed.

[pigrew]

My understanding is that a USB device can have a max of 10 uF directly on Vbus. With this schematic, it has 125 uF. The way around this is some sort of soft-start. I'd suggest adding a load switch for the "extra" USB port (which would implement soft-start itself, and also over-current protection)  (Oh... seems you did this on the GitHub schematic)

One datasheet for the HS-100B says to connect the Vref pin to an external capacitor (10nF is a wild guess). I can't find any sort of documentation for which value to use... I'd imagine that each of the regulator outputs also should have a decoupling capacitor (2.2uF is a wild guess). Is there a reference design schematic? (I see there is an evaluation board available, but I can't find the schematic for it... You could buy it and reverse engineer it.)

2) when the time comes to the PCB layout, be sure to note that you must apply impedance controlled traces for the USB 2.0 HS lines. Many articles on the internet on this subject. Your PCB shop should be able to support this requirement of 90 ohms and validate with a TDR report.

3) Why are there caps on the D+ and D- lines? This may be a violation of the USB spec. Have never used them in any of our designs for USB 1.1 / 2.0 / 3.1 to date.

For HS, I think impedance control probably doesn't matter, as long as the USB tracks are short (like less than 4cm, which is feasible.). The rise time is ~500ps. Guestimate 15 cm/ns prop velocity. So, you might want the track to be less than 250ps long, so 3.75cm max length. That being said, you should try to target 90 ohm. The spec allows +/-10%. The skew is probably more important. Try to length-match to within a few mm.

However, the hub is only full speed, so it'll be fine, up to quite a few cm.

The USB data-line capacitors are for EMI reduction and also ESD immunity. I would not populate them for the on-board USB devices, but I would use the one going to the USB port.

The hub's BUSPWR should be low, since you are provide current from the upstream USB connection.

It's very debatable if the USB shield should be shorted to the USB GND, or not. I recently went through my pile of USB cables and most of them had open shields, so it probably doesn't matter.

[teksturi]

So have you check that almost everything can really left floating with audio ic?
I say about that in my previous post.

I also notice that you still have some unconnected ground in pcb design. Maybe
you are still working with it? When you make new post here you can also add
new picture for schematic. Also you can add image(s) for layout also.

You have made good progress with this one. Nice to notice that you take input
and not just say that you have already do the layout and do not want to do it
again. Nice job. 

[xylo04]

My understanding is that a USB device can have a max of 10 uF directly on Vbus. With this schematic, it has 125 uF.

The 120 uF value is coming out of the TUSB2036 datasheet, as well as mon2's advice above. However, I did find that I need to change the package type as that value doesn't come in 1210.

One datasheet for the HS-100B says to connect the Vref pin to an external capacitor (10nF is a wild guess). I can't find any sort of documentation for which value to use... I'd imagine that each of the regulator outputs also should have a decoupling capacitor (2.2uF is a wild guess). Is there a reference design schematic? (I see there is an evaluation board available, but I can't find the schematic for it... You could buy it and reverse engineer it.)

This is one of my biggest problems at the moment, the HS-100B doesn't have good application notes or eval board schematics. CMedia sells a slightly more expensive USB audio chip, the CM108, which does have decent documentation: http://rats.fi/wp-content/uploads/2016/04/CM108_DataSheet_v1.6.pdf. I'm considering switching to that chipset.

The USB data-line capacitors are for EMI reduction and also ESD immunity. I would not populate them for the on-board USB devices, but I would use the one going to the USB port.

If this is the case, maybe I can move those caps to the TX/RX and SPKR/MIC lines since those are at the edge of the board?

So have you check that almost everything can really left floating with audio ic?
I say about that in my previous post.

You did mention it. I'm hesitating to add a bunch of pull-ups for everything because my board is starting to get a bit crowded. The application note for the CM108 (linked above) suggests that those probably have internal pull-ups. However, that doesn't mean I'm going to ignore your advice.

I'm starting to feel like I don't understand these chips well enough to make a super tiny PCB with all three immediately. I'm going to take a step back and basically build my own eval boards for each of the three major functions and make sure each works separately. That should give me a chance to test each in isolation and give me confidence to know that I understand what each chip needs, without the pressure of fitting my desired form factor. That way, I can experiment with 0-ohm resistors and test points galore on a larger surface.

Thank you all again, I'm excited that this project is moving forward!

[pigrew]

My understanding is that a USB device can have a max of 10 uF directly on Vbus. With this schematic, it has 125 uF.

The 120 uF value is coming out of the TUSB2036 datasheet, as well as mon2's advice above. However, I did find that I need to change the package type as that value doesn't come in 1210.

The distinction is device-side or host-side. The device should have betwen 1 and 10uF, but the host should have larger.  The host must have >=120uF. These values are from the USB 2.0 spec, table 7-7 on page 179.

One datasheet for the HS-100B says to connect the Vref pin to an external capacitor (10nF is a wild guess). I can't find any sort of documentation for which value to use... I'd imagine that each of the regulator outputs also should have a decoupling capacitor (2.2uF is a wild guess). Is there a reference design schematic? (I see there is an evaluation board available, but I can't find the schematic for it... You could buy it and reverse engineer it.)

This is one of my biggest problems at the moment, the HS-100B doesn't have good application notes or eval board schematics. CMedia sells a slightly more expensive USB audio chip, the CM108, which does have decent documentation: http://rats.fi/wp-content/uploads/2016/04/CM108_DataSheet_v1.6.pdf. I'm considering switching to that chipset.

https://www.cirmall.com/circuit/13967 shows a schematic with the IC.  They let you download the files, if you login with QQ or Weibo (which I don't really want to do....). You likely could email CMedia and ask for the schematic for their demo board. You can also order the demo board, and then reverse-engineer it (measure capacitor values).

The USB data-line capacitors are for EMI reduction and also ESD immunity. I would not populate them for the on-board USB devices, but I would use the one going to the USB port.

If this is the case, maybe I can move those caps to the TX/RX and SPKR/MIC lines since those are at the edge of the board?

I'd just get rid of them. Although, adding ESD protection for the analog audio pins wouldn't be a bad idea. The implementation would be different (maybe TVS diodes and series resistance).

[xylo04]

The distinction is device-side or host-side. The device should have betwen 1 and 10uF, but the host should have larger.  The host must have >=120uF. These values are from the USB 2.0 spec, table 7-7 on page 179.

Ok, so I think you're saying in the current version of the schematic, C19 should not be on the upstream port, that C3 and C4 are ok because they are <10uF combined, and that C11, C16 and C17 are in-spec for the downstream ports. Do I want to keep C11 and C16 on the hardwired devices, or can I remove them and only keep C17 for the downstream socket?

With regards to trying to break up the project to verify that I know how to use the ICs individually, I've attached two schematics, one for the TUSB2036 hub, and the other for the HS-100B's cousin, the CM108B USB audio controller. Both of these match reasonably well to their application notes, and should have enough room and jumpers and test points to let me verify that each individually is working. I'll make one for the FT232 as well, although that one is well-documented enough that I probably don't have to bore you all with that.

I did have to do a little bit of guesswork on the CM108B board. The datasheet for the B version of the chip doesn't have application notes, so I'm relying on application notes from the original CM108 (datasheet). I removed the crystal, SPDIF, EEPROM and some other things that were unnecessary. Unfortunately, I'm confused by the way some of the capacitors are marked. Several caps are marked "101", "104", "105", and "475". I thought those might be in pF, but they're not common values. Maybe they refer to a BOM that's not provided?

[pigrew]

The distinction is device-side or host-side. The device should have betwen 1 and 10uF, but the host should have larger.  The host must have >=120uF. These values are from the USB 2.0 spec, table 7-7 on page 179.

Ok, so I think you're saying in the current version of the schematic, C19 should not be on the upstream port, that C3 and C4 are ok because they are <10uF combined, and that C11, C16 and C17 are in-spec for the downstream ports. Do I want to keep C11 and C16 on the hardwired devices, or can I remove them and only keep C17 for the downstream socket?

With regards to trying to break up the project to verify that I know how to use the ICs individually, I've attached two schematics, one for the TUSB2036 hub, and the other for the HS-100B's cousin, the CM108B USB audio controller. Both of these match reasonably well to their application notes, and should have enough room and jumpers and test points to let me verify that each individually is working. I'll make one for the FT232 as well, although that one is well-documented enough that I probably don't have to bore you all with that.

I did have to do a little bit of guesswork on the CM108B board. The datasheet for the B version of the chip doesn't have application notes, so I'm relying on application notes from the original CM108 (datasheet). I removed the crystal, SPDIF, EEPROM and some other things that were unnecessary. Unfortunately, I'm confused by the way some of the capacitors are marked. Several caps are marked "101", "104", "105", and "475". I thought those might be in pF, but they're not common values. Maybe they refer to a BOM that's not provided?

Right... (C19+C3+C4+C20) (device-side) must sum to less than 10 uF, unless you add a soft-start circuit (<10uF would be on the bus side, and you could have as much capacitance as you want on the load side). Your load switch should count as soft-start, so you likely could use its fourth channel as a soft-start for other bits of your circuit.

Load switch U5B's enable pin probably shouldn't be floating. Connect it to VDD through a pull-up resistor to VBUS.

Those cap values should be in exponential notation of pF. 101 would be 10*10^0 pF = 10 pF. 104 would be 10*10^4 pF = 100nF, 105 = 1 uF.

[xylo04]

Time for an update! I decided there were enough unknowns that I should take a step back and play with the three major sections of the project separately: the USB hub, UART and audio. In that way, I figured I could validate each independently and make sure I understood the individual pieces before putting them together.

I've published 4 additional repos:

• UART: https://github.com/k0swe/ft232r-eval
• Two versions of the sound card, https://github.com/k0swe/hs100b-eval and https://github.com/k0swe/cm108b-eval
• USB hub: https://github.com/k0swe/tusb2036-eval

So far the FT232R and the CM108B work flawlessly according to expectation. I haven't built the HS100B version, but I'm starting to lean toward the CM108B anyway since it has GPIO pins I can use for a push-to-talk (PTT) circuit.

However, I'm having trouble with the TUSB2036 hub I built. When I attach it to a host, it doesn't enumerate. I've checked voltages in several places and it seems to be getting power, it's just not talking to the host. I think my next step is to stop by my makerspace and get comfy with the oscilloscope to see what I can learn, maybe starting by verifying the 6 MHz crystal is running as expected. Maybe I inadvertently fried the chip? I'm not quite sure what I'm looking for at this point.

One part that confused me about the TUSB2036 datasheet is that the application notes all include a placeholder "System Power-On Reset" on the RESET pin. Do I need something extra to pull this up or down after an initial timer? I don't know what to do with that placeholder. I have a push-button on it now, but that's not doing much to help.

I'll keep muddling along, but I would be glad for advice. Thanks to those who have already helped me out!

[pigrew]

One part that confused me about the TUSB2036 datasheet is that the application notes all include a placeholder "System Power-On Reset" on the RESET pin. Do I need something extra to pull this up or down after an initial timer? I don't know what to do with that placeholder. I have a push-button on it now, but that's not doing much to help.

Based on the datasheet, there is no internal pull-up, so your reset pin is being left floating.

You probably can get away with a RC filter as a reset (capacitor to GND, resistor to 3.3V, time constant of a millisecond or so). Otherwise, you buy a power supply supervisor IC with a suitable time delay.

TI has reference schematics downloadable from their product page ("design tools & simulation" category). They use a RC filter for reset (15k + 1uF).

[xylo04]

That's very helpful, thank you!

[xylo04]

Probably final update on this: it's working! https://github.com/k0swe/mountaineer

Thanks to all of the advice here, it was an enormous help!