Struggling with project. Not sure what to do.

[Jackster]

So I have been working on this electronics project for the past 6-8 months now and I am about 4 months behind shipping.

Not sure what my options are at this point and have sortof lost all will to live at this stage.


I have 2 boards designed that are basically the same but one breaks into 3 separate boards and the other is a single board. They have the same components other than the one that breaks up having a duplicates of some and added FFC parts.

The single board version works fine. Not really had any problems with it and by revision 3 is fully working and ready for P&P and shipping.
The other board that splits up into 3 I have not managed to get to work yet and I am on revision 5.
This time copying the single board in CircuitMaker and remaking it from the ground up.
Yet still in revision 5 prototyping I am unable to get it to work.

The problem looks to be around the FTDI FT232RL. When ever I plugin the USB I always get errors like "Device Descriptor Request Failed).

I'm not sure if it is the circuit or the fact that I am trying to P&P the prototypes by hand.
I've been using SMD stencils to improve the soldering and this has helped a lot but no matter what I do with this board it fails every time.

Not sure what my options are here. Guessing my best bet is to hire someone to take a look at it for me?

[tszaboo]

This is what I think: The FCC cables have resistance and inductance. It is generally required to use one GND connection every 4-5 digital line. So try connecting the GNDs together with extra cables, and see if this helps.
Is anything else connected to the boards, or is it just USB? With more than 1 connection, you might have ground loops, which isnt a problem with just one board, but becomes one with 3 boards.

[Jackster]

Don't have the FFC connected atm. I made the 3 parts of the boards into a "panel" and at the cutoff points added traces for power, ground and data.
Just USB. No other connections.

[tszaboo]

Can you post a picture? Schematic? Layout maybe? In jpg or PDF.

[Jackster]

Do you have Circuit Maker? Can just add you to the project. Might be better than static images?

[stmdude]

Do you have Circuit Maker? Can just add you to the project. Might be better than static images?

If you put static images on here, anyone could help you, not just the people with Circuit Maker. Just sayin'

[Jackster]

Top Layer

Bottom Layer

[RoGeorge]

Did you put 3xFT232 in parallel on the same USB cable?

If yes, this can not work.
You need 3 different USB cables from 3 different host USBs, one for each FT232 devices.

If you put them all 3 FTDIs in parallel, when the USB host is asking the 3xFT232 "Who and what are you?", then all at once will try to answer. It won't be an intelligible answer.

[Jackster]

Did you put 3xFT232 in parallel on the same USB cable?

If yes, this can not work.
You need 3 different USB cables for 3 FT232 devices.

USB is asking the 3xFT232 "Who and what are you?", then all at once will try to answer. It won't be an intelligible answer.

No, I only have the one FTDI chip. This board is split into 3, but is all one circuit being driven by a single FTDI.
The split just allows the displays and switches to all be angled from each other.

[stmdude]

I'm having a hard time figuring out what the three different sections on the PCB is doing, but I can tell you right now that the USB traces you have are _wierd_. They're forking off (seems terminated in two different headers, and the FT232), and seem pretty long.

You can't really do that with 12MHz differential signals. You'll get lots of reflection in the lines, completely messing up your signal integrity.

Unless you're doing something completely whacky (like RoGeorge suggests), I'm willing to bet that this is your issue

[Andy Watson]

What have you connected to pin 26 of the FTDI chip? The schematic appears to show no-connection but the data sheet says "Must be tied to GND for normal operation, otherwise the device will appear to fail."

[RoGeorge]

If you have only one FTDI chip, then why and where did you route the USB D+ and D- data lines. Those will add unnecessary reflections.

- first step, I will cut all ramifications of the USB data whires that are not necessary.
- if it still does the same, then check the FTDI chip is working and is correctly wired in respect to USB D+ and D-.

A last thing could be a fake FTDI chip that is bricked by the windows drivers (that was a problem a few years ago, it probably won't happen now).

[Jackster]

I'm having a hard time figuring out what the three different sections on the PCB is doing, but I can tell you right now that the USB traces you have are _wierd_. They're forking off (seems terminated in two different headers, and the FT232), and seem pretty long.

You can't really do that with 12MHz differential signals. You'll get lots of reflection in the lines, completely messing up your signal integrity.

Unless you're doing something completely whacky (like RoGeorge suggests), I'm willing to bet that this is your issue

The USB lines go to the FFC sockets and fork off directly to the FTDI as well. When I break the boards apart the direct connection breaks and can only go via the FFC.
Was told this wasn't too bad in terms of length. Could move the FTDI to the side with the USB but I would then need a much larger FFC to get to the main board where the ATMEGA is.

[fourtytwo42]

I'm having a hard time figuring out what the three different sections on the PCB is doing, but I can tell you right now that the USB traces you have are _wierd_. They're forking off (seems terminated in two different headers, and the FT232), and seem pretty long.

You can't really do that with 12MHz differential signals. You'll get lots of reflection in the lines, completely messing up your signal integrity.

Unless you're doing something completely whacky (like RoGeorge suggests), I'm willing to bet that this is your issue

Have to agree here never seen anything like it! USB is a point to point system, meaning the data lines from your FTDI chip should go straight to the connector as a PAIR and absolutely nothing else!! Checkout the apps notes, there are suggested layouts there

[Jackster]

Did you not closely read the note on pin #26 in the data sheet?  Looks like a  problem to me.

26 TEST Input Puts the device into IC test mode. Must be tied to GND for normal
operation, otherwise the device will appear to fail.

What have you connected to pin 26 of the FTDI chip? The schematic appears to show no-connection but the data sheet says "Must be tied to GND for normal operation, otherwise the device will appear to fail."

Hmm interesting. That might be it.
Sometimes the other board does not work too in the same manner...


Just tested it on the "working" board and looks like that was it.

[edit] I have tested this with the problematic board and still get the same error.
Guessing as suggested that the USB data lines being forked as such are not helping.

[Jackster]

Any suggestions on the USB data routes?
Will they be okay going over the FFC?

[ovnr]

On a completely different matter: I noticed that you're using a NRF24L01+ 1.27mm pitch module. There are two pinouts on the market - one with GND on pin 2, one with GND on pin 8. Suffice to say they're not compatible. Verify you've got the right one - it seems like GND on pin 2 (like the larger TH header versions) is more common, while you have it on pin 8.

[Jackster]

On a completely different matter: I noticed that you're using a NRF24L01+ 1.27mm pitch module. There are two pinouts on the market - one with GND on pin 2, one with GND on pin 8. Suffice to say they're not compatible. Verify you've got the right one - it seems like GND on pin 2 (like the larger TH header versions) is more common, while you have it on pin 8.

I based the pinout on the headers from the datasheet. Already tested and works fine. Thanks though I was not aware of this.

[stmdude]

Any suggestions on the USB data routes?
Will they be okay going over the FFC?

Well.. The first thing I would try is to cut the traces to the FFC connectors, and just leave the traces between the USB connector and FT232 to see if this really is your issue.

If it is, first, you need to read up on routing differential signals. Second, you should re-route your board with your new-found knowledge, and figure out a way to just have two things connected to the bus at the same time (FFC connectors count as a thing).
You could use solder-bridges or in-line 22ohm resistors to be able to swap between using the USB connector or the FFC as one end of the bus.

Oh, and when reading up on routing differential signals, you're "only" using full-speed USB, so you can most likely just ignore impedance matching for now.

[tszaboo]

USB can go through FCC connectors. They need to be routed deferentially, on the same layer, through the same amount of vias, and the GND has to be wide enough for them. No Y connections.
Your GND is also all over the place. It should be the widest trace. If possible, it is a layer, not a trace.

How many of these are you planning to make, and how much money do you loose because of the delays? Because maybe, you should really hire a consultant to finish it.

[dmills]

I really don't think I would have tried this on a two layer job, a solid ground plane is really, really helpful when trying to pass EMC apart from anything else, and it will make high speed things like USB altogether better behaved.

My starting point these days is 4 layers, unless it is something utterly trivial with nothing at all fast edged on it, and moving to 6 does not take much convincing, anything with RF on the board really needs a plane, but see the datasheet for the RF module for details around the aerial.

The premium for 4 layers in reasonable production quantities is very small now, so unless this is incredibly price sensitive (In which case there are cheaper options then FTDI), I would start by burying a ground and 3V3 plane, fixing the pin 26 issue and sorting out the USB routing.

Regards, Dan.

[Jackster]

USB can go through FCC connectors. They need to be routed deferentially, on the same layer, through the same amount of vias, and the GND has to be wide enough for them. No Y connections.
Your GND is also all over the place. It should be the widest trace. If possible, it is a layer, not a trace.

How many of these are you planning to make, and how much money do you loose because of the delays? Because maybe, you should really hire a consultant to finish it.

Ill remove the fixed routes then and just go via the FFC.
Ill look into flooding GND? I can only really do 2 layer. 4 layers double PCB cost and I am already nearing my limit with component choice (FTDI over cheaper CH360).

I need to make around 50 of these, 75-100 of the other board. Not lost any delay but it is not a good image.
Tempted to hire someone at this point.

I really don't think I would have tried this on a two layer job, a solid ground plane is really, really helpful when trying to pass EMC apart from anything else, and it will make high speed things like USB altogether better behaved.

My starting point these days is 4 layers, unless it is something utterly trivial with nothing at all fast edged on it, and moving to 6 does not take much convincing, anything with RF on the board really needs a plane, but see the datasheet for the RF module for details around the aerial.

The premium for 4 layers in reasonable production quantities is very small now, so unless this is incredibly price sensitive (In which case there are cheaper options then FTDI), I would start by burying a ground and 3V3 plane, fixing the pin 26 issue and sorting out the USB routing.

Regards, Dan.

4 layers double my PCB cost. I am already at my limit. Would flooding/pouring GND be okay on one or both of my layers?
I don't think I can do 4 layer on Circuit Maker too...

Any suggestions on the USB data routes?
Will they be okay going over the FFC?

Well.. The first thing I would try is to cut the traces to the FFC connectors, and just leave the traces between the USB connector and FT232 to see if this really is your issue.

If it is, first, you need to read up on routing differential signals. Second, you should re-route your board with your new-found knowledge, and figure out a way to just have two things connected to the bus at the same time (FFC connectors count as a thing).
You could use solder-bridges or in-line 22ohm resistors to be able to swap between using the USB connector or the FFC as one end of the bus.

Oh, and when reading up on routing differential signals, you're "only" using full-speed USB, so you can most likely just ignore impedance matching for now.

I have cut the traces just above the USB connector going to the FFC connector. Did not improve anything.

Ill look into differential signals. I did keep the routes the same on my other board, but was told by a few people that it does not matter at these lengths.


Thank you all btw.

[tszaboo]

I draw a signal's current, and the return GND current for it. That area will act like an antenna, sending EMC everywhere and collecting noise. It should be better than this.

[Jackster]

I draw a signal's current, and the return GND current for it. That area will act like an antenna, sending EMC everywhere and collecting noise. It should be better than this.

Once I break the boards apart that should not be a problem? The ground will go via the FFC cable.

[stmdude]

I have cut the traces just above the USB connector going to the FFC connector. Did not improve anything.

Ill look into differential signals. I did keep the routes the same on my other board, but was told by a few people that it does not matter at these lengths.

There's a few things that matter _less_ when you have a small board and "only" run 12Mbps, such as impedance matching and to a certain extent, skew.  However, you absolutely need to route it as a differential signal. D+ and D- needs to run parallel to each other the entire way with a fixed distance between them. Use as few vias as possible, but if you need to use them, always use them in pairs. Everything one line does, the other one needs to do.