Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

MCU and USB Section Powering

Status
Not open for further replies.

tiwari.sachin

Full Member level 6
Joined
Aug 1, 2009
Messages
341
Helped
3
Reputation
6
Reaction score
3
Trophy points
1,298
Location
India
Activity points
4,447
I need some suggestion on how can the MCU Vcc and USB Vcc and Analog Vcc can be powered up

All the above voltages are 3.3V

I am connecting 3.3V regulator outputs to all the above said Vcc... MCU Vcc and USB Vcc with a 100nF cap

Analog Vcc with a ferrite and 100nF cap before ferrite on Vcc and 100nF and 1uF after ferrite that goes to AVcc


Now products are working fine but we have products being returned and i see that Vcc and GND are short.

I got the failure analysis done from the MCU vendor and they say it could be electrical stress (over voltage or current) due to which the wires are damaged

I have the X-ray report too

Could anyone suggest me on the precautions I need to take to power up the MCU.

I have been connecting Regulator output to MCU pins all this time but this is something of new issue and I really need some expert advice
 

USB device right now

There are some pins on mcu

USB vcc... Tied to 3.3v of regulator

Vbus... Connected to Vbus pin of mcu via voltage divider as it is 3.3v compatible

And of course D+ and D-
 

Check the current consumed by USB device which should be within the limits of your regulator
 

As I said. I have used a voltage divider and connected to mcu Vbus which needs 3.3V
 

I am connecting 3.3V regulator outputs to all the above said Vcc... MCU Vcc and USB Vcc
USB device right now
So you are USB slave, and the USB master (according to standard) will supply 5V on USB Vbus Pin1 of USB connector.
Is this pin connected to something else than the (hopefully hi-impedance) voltage divider connected to Vbus pin of the CPU?
Please provide a schematic
 

You say it's a self-powered USB device and you observe VCC to GND short of the MCU.

Possible reason is either VCC overvoltage or supply latch-up triggered by a CPU IO pin. I presume the chip analysis could tell more to narrow down the failure mechanism, but apparently there have been no significant results provided.

Apart from chip analysis, I would look for this points:
- possible ways how a VCC overvoltage can propagate to the CPU. Are there any protection means, e.g. TVS diodes?
- which CPU pins are exposed to external interfaces or possibly ESD events? Are they protected against overvoltage respective excessive clamp current?
- I presume the D+ and D- pins must be considered as possible target of ESD and other voltage surges in any case. Are they protected externally?
 

Usb sch

USB SECTION.png

mcu section

MCU Section.png

- - - Updated - - -

I have got the chip analysis done from the MCU vendors and it shows the xray and I can see that the internai wires D+, D- and some other IO pins are cut

It also shows that the internal diodes (TVS I think) are damaged and hence the short.

I too think it probably is the ESD but i have the protection

Below are the PCB Design section

TOP LAYER

TOP.png

On Top the series resistors are used on D+ and D-

BOTTOM LAYER

BOTTOM.png

On Bottom layer I have the ESD Chip and the fuse.

I understand that the ESD pins have to be connected without a Via, Preffered is always a direct connection but due to the PCB and placement constraint, I had to place it as given

- - - Updated - - -

SHIELD GND AND USB GND are saparted as given below

SAPARATION.png

- - - Updated - - -

My Power Supply Circuit. The voltages that I get are perfect and there is no fluctuation or ringing on DC to DC.

PS.png

The 3.3V from the regulator is directly connected to MCU Power. with some 0.1uF caps

- - - Updated - - -

Note: I am not using USB power to run the system. The device is powered by a battery

VBus is used only for USB Detection Purpose
 

First suggestion:
TVS Array SP1255 should be connected to USB_VSS, not the VSS_SH (as you have a Hi-Imp connection between VSS_SH and USB_VSS)
Second question:
How is the connection between USB_VSS and GND (of µC) realized? (should be a low-imp. connection...)
 

Check image for USB_Vss Connection

USB_VSS.png

I saw that the MCU_GND and USB_VSS GND was short in MCU and hence didnot connect it anywhere and have connected it directly to Pin 5 of USB Connector.
 

OK, so you have an internal starpoint in the cpu die (by bonding wires). Should be OK for a battery powered system.
Imho the major ESD problem is caused by wrong connection of the TVS protection array.
With current circuit you protect the incoming USB lines against host chassis GND (via cableShield), but you should protect your USB/cpu inputs against your localGND/cpuGND
 

Should I connect TVS to USB_VSS or GND of MCU.

Note there a star point in the CPU DIE between these grounds

- - - Updated - - -

I have changed as follows

BOT_ESD.png

As can be seen I have connected the TVS GND to GND of MCU (third layer in GND). Not connected to USB_Vss as there is no dedicated layer for the same

The Blue area (Hole is the mounting hole) for casing

TOP_ESD.png

This image is of the TOP layer. USB_VSS is connnected to the USB_Shield via resistor and cap.

I had a ESD tested at 8KV (The older board) and it failed. I am wondering if I am doing it right this time.


SUM UP

USB_VSS and GND (POWER, MCU etc) -----> Short in MCU (Star internal to chip)
GND dedicated Plane hence connected TVS GND to third layer (GND)
 

Better than before, but I would highly recommend to connect TVS to USB_VSS, to have a robust backpath to the USB GND wire (and not via bonding starpoint inside CPU).
So GND concept should look like:
Code:
                 TVS
                  |
VSS_SH---[RC]---VSS_USB---[CPU starpoint]---GND

Also TVS should be placed on topside close to connector pins (TVS pinout was designed to have straight connection to connector)
All signals should follow daisy-chain approach (connector-TVS-SeriesR-CPU, no stubs)
F3 is IMO useless, as you only do hi-imp. sensing on the line.
C59, do you really need 2µ2? I would suggest ~100n for noise filtering

- - - Updated - - -

Other question regarding your application:
You said its battery powered, and according schematic you use a Buck-SMPS for 5V.
Is the circuit working in Car environment?
And do you have additional circuits inside which need the 5V? (as CPU is 3V3 only)
 

F3 is a fuse... 500mA... Why is it useless

I will try to put the TVS on top but I would still need to have vias before the pin and connect to resistors of D+ and D-... Is that ok... I did it because of space constraint.

Its more of a handheld printer... 5V is needed for USB host IC... After DC to DC.... I have a LDO for 3.3v

Battery Li Ion 7.4V, 2 series →DC to DC 5V →LDO 1117 for 3.3V

- - - Updated - - -

Note... Right now... I am not using Host but I do have a option....


Whenever I use host... I will have DC to Dc 5V and LDO to generate 3.3V

For options where Host is not needed... The DC to DC is used to generate 3.3V

I do have option for this....
 

From schematic you showed, 5VUSB is only loaded by R56/R60 divider, which will drain less than 1mA. So what is F3 protecting?
If you fear the risk of short-circuit to your internal components, then 500mA is far too high. E.g. if R56 is shorted, CPU will be biased via clampdiode to 5V. Clamping diodes will usually burn up >~2mA, so your CPU is damaged, and F3 still working...

As you have bigger vias and traces, you may have to put them in front of the TVS, but place them as close as possible to the TVS pads.

So you are USB Slave & Host in one unit? We just talked up to now to the slave part.
Is the printer (which I think is connected to the Host side) Host-supplied? By your battery, or did you make a bypass to the slave interface? (in this case F3 makes sense...)

- - - Updated - - -

Your update describing placement variants makes it even more complicated...
So your design is either USB slave OR USB Host. Do you use different interfaces for this, or always the same connector?
 

This is what the entire USB Section is

USB.png

I am not using the HOST Section as of now.

I am right now using only device, maybe I will just short F3.
 

OK, this explains the need for F3.
So the need for F3 depends on the current capabilities of the 5V BuckSMPS.
If it can source 1.5A (Thermal shutdown of U16) you can skip the fuse.
If not, then F3 is a good solution.
I would suggest to connect the CPU voltage sensing to USB_5V, so CPU can sense if F3 opened, and you can unplace F3 in case you don't implement HOST mode ;-)
For U17 (TVS) I still recommend to connect it to USB_VSS.
 

I have changed the ESD as below

ESD_UVss.png

The ESD IC is on top and the signal lines routed at the bottom.

I have even removed F3, U16 does have the protection. I had missed it. Thanks for pointing that out.
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top