• State TI Thinks Resolved
  • Locked Locked
  • Replies 15 replies
  • Answers 1 answer
  • Subscribers 63 subscribers
  • Views 6467 views
  • Users 0 members are here
Support feedback
Options
Options
Related

This thread has been locked.

If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.

TPS61090: short circuits at SW pin 3,4 after working for some time

Macjan Camilo Fernandes
Prodigy 180 points
Part Number: TPS61090
Other Parts Discussed in Thread: , TPS61092

Hello TI,

Brief description:

Our circuit contains 5V input adapter source given to MCP73871 (U8) charger IC with 3.7V Lithium Ion battery for backup. So during power fails battery takes in charge. This output is given to TPS61090RSARG4 (U7) IC which then boost the voltage to 5V and max load is only 500mA. I've attached our circuit diagram below including gerber view and placements. We have used these components for the first time in our designs and hoping to use it in future a lot.

Test Setup:

1. CRO Probe connected to TPS61090 VOUT at R69

2. Input voltage 5V Bench Supply given at R55 ( Not SMPS based) excluding rest of circuit with no LOAD's connected. (Input will be 7V 3A SMPS adapter in actual application)

3. Battery Not connected to charger circuit. (When battery is not connected the Input voltage at R55 is given as VBAT)

4. R67 = 1.8MOhms, R68= 200kOhms. (on CRO here it shows 0.540mV) (Correction done on Resistor divider)

5. The dot on 6.8uH power inductor is connected to VBAT,

6. PI_EN Pin is open in the circuit and going only to external connector.

Problem:

1. Circuit works fine for some time. Gives 5V output perfectly with no Load. After some time or sometimes immediately the TPS61090 IC gets short circuited pulling lot of current through Charger IC disabling output of Charger IC itself. So we put a 500mA PTC fuse which also doesn't help and still destroys the TPS61090 IC. CRO just shows low voltage at the output side and no way to debug what just happened.

2. We have also noticed after removing the IC, pins 3,4 which is SW is getting shorted to PGND pins. 

SCHEMATIC:

GERBER VIEW:

PCB TOP VIEW:

I have gone though some forum articles and found a similar issue on this post

https://e2e.ti.com/support/power_management/non-isolated_dcdc/f/196/t/435455

So we tried putting a Schottky diode of 100V rating which we had in stock to see if there was any protection needed for the FET on the gate control. So we kept it as close as to the SW pin. Which can be noticed on above picture of PCB view.

Then after connecting Schottky diode on SW pins 3,4. We turned on the Power supply and got 5V output very stable. But the below some drops in voltages were noticed. We think that these were creating problem and destroying the SW pin. Output voltage totally drops to 0V at some time intervals and some are steady. 

The article in previous link also mentioned to use RC snubber circuit across SW pins to PGND which we have not tried yet. The critical 2.2uF capacitor is right below C24 highlighted in Green in Gerber View.


Please also help us selecting the right RC values for snubber circuit.???

 

Our team will be really appreciated if you help us out sorting this Issue. 

Thanking you,

Macjan C. Fernandes

(EME Automation, Goa - India)

  • 0
    TI__Mastermind 46905 points
    the location and routing of C22 is not good, which could cause high voltage spike in SW and damage the IC.
    You can refer to this application note www.ti.com/.../slva773.pdf to revise the layout.
    in current board, you can try to add RC snubber, the location of the snubber is also important, which can also be found the this application note
  • 0 in reply to Jasper Li
    Prodigy 180 points

    Jasper Li,

    Since there was no time manufacturing another board and reply you as soon as possible; we did some work around.

    Work Around:

    We had no time testing this out on a new board since manufacturing one takes time but we managed to put a 2.2uF (C22) as close as possible marked in red on the same old board. You can check the pic.



    There was still no improvement in the system. We destroyed another IC.

    Also I will like to mention we have another board working perfectly fine. I have no idea how its working. Everything is similar as above.

     

    New problem: (on working board with above specifications)

    We wanted battery low indicator at around 3V so we calculated Resistor divider circuit for 3V at LBI Pin.

    According to datasheet:



    We have chosen R2 = 340K. Hence for 3V threshold which gives R1 = 1.7MOhms. The closest we had was 1.87Mohms.

    So when 1.87Mohms is put, the threshold changes to 3.25V. (1.87M ,340k voltage divider circuit).

    After placing the components as per above calculations on the proper working board, we got 2.75V as threshold. (LBO pin was turning off at 2.75V and not at 3.25V).

    Request:

    We want to know if there is any chance our circuit is misbehaving at LBI and LBO. If so please help us understanding the problem.

     

    Please help us know if we are going in right direction.

     

    Jasper Li,

    Since there was no time manufacturing another board and reply you as soon as possible; we did some work around.

    Work Around:

    We had no time testing this out on a new board since manufacturing one takes time but we managed to put a 2.2uF (C22) as close as possible marked in red on the same old board. You can check the pic.

    https://e2e.ti.com/resized-image/__size/1230x500/__key/communityserver-components-multipleuploadfilemanager/f588cf25_2D00_f67f_2D00_4f13_2D00_b6fa_2D00_ff609a1d4ec0-133348-complete/P_5F00_20171124_5F00_104600.jpg

    There was still no improvement in the system. We destroyed another IC.

    Also I will like to mention we have another board working perfectly fine. I have no idea how its working. Everything is similar as above.

     

    New problem: (on working board with above specifications)

    We wanted battery low indicator at around 3V so we calculated Resistor divider circuit for 3V at LBI Pin.

    According to datasheet:

    https://e2e.ti.com/resized-image/__size/1230x300/__key/communityserver-components-multipleuploadfilemanager/f354adf5_2D00_f854_2D00_45bd_2D00_be3f_2D00_17ccf418c8b8-133348-complete/Untitled.png

    We have chosen R2 = 340K. Hence for 3V threshold which gives R1 = 1.7MOhms. The closest we had was 1.87Mohms.

    So when 1.87Mohms is put, the threshold changes to 3.25V. (1.87M ,340k voltage divider circuit).

    After placing the components as per above calculations on the proper working board, we got 2.75V as threshold. (LBO pin was turning off at 2.75V and not at 3.25V).

    Request:

    We want to know if there is any chance our circuit is misbehaving at LBI and LBO. If so please help us understanding the problem.

     

    Please help us know if we are going in right direction.

  • 0 in reply to Macjan Camilo Fernandes
    TI__Mastermind 46905 points
    from your figure, the location is closed to the IC. however, the routing between the capacitor GND PIN to the IC GND is too long.

    about the LBI problem, could you measure the voltage at LBI pin when the battery voltage is 3V to check if the voltage in LBI is correct
  • 0 in reply to Jasper Li
    Prodigy 180 points

    Jasper Li,

    Regarding LBI Problem, we are unable to check that out because our all TPS61090 IC's got destroyed.

    We have now already purchased fixed 5.1V  output type TPS61092 and also redesigning the board as per document SLVA773 and evaluation module( TPS61090EVM-029)

     We will need your help after our designs are ready to check our gerber files. If you can share us contact information of design expertise in India so we can discuss with them the evaluation of our board.

    On the datasheet there was a problem understanding the ground syntax used. Why there are two types of Ground symbols in this schematic? Is it something to do with plane separation or to isolate other grounds and get it to one single point so the return path is through this IC only?

  • 0 in reply to Macjan Camilo Fernandes
    TI__Mastermind 46905 points
    you can send me the schematic and PCB layout image one this post as you sent before. i'll review them for you.
    they the signal GND and power GND. They should be connected in a signal point in the PCB.
  • 0 in reply to Jasper Li
    Prodigy 180 points
    Jasper,

    We purchased new IC's recently for fixed 5V. It's TPS61092.

    We connected on the same (bad layout board) and found it was not even starting up with same configuration as TPS61090. There was 100k resistor pull up on EN pin given which is R63 in schematic. But when we shorted EN pin i.e. 0E on R63 we got clean signal. No damaging of TPS61092 for 3 days. Is there any connection to our previous module where 100k on EN pin was causing any switching malfunction which caused damage to TPS61090?

    Secondly we also wanted to ask about Supply input. We have 5.1V Supply which may vary +/- 8%. And there are chancing that TPS60192 output will be less then Supply input which will be like buck conversion. We wanted to know if this was damage our component? Or should we maintain v input always less then v output for safety.

    We are side by side working on schematic and will be sending you soon.
  • 0 in reply to Macjan Camilo Fernandes
    Prodigy 180 points

    Jasper,

    below are new schematic changes. We only changed r63 to nop so we will enable boost using buffer gate at PI_EN.

    Below contains details of pcb layout. Please we need your help to review it.

    PCB top layer

    Bottom layer

  • 0 in reply to Macjan Camilo Fernandes
    TI__Mastermind 46905 points
    please rotate the C22 and place it closed the IC. place several via beside the GND node of the C22.

    the RC can be used if you can observe voltage spike in SW pin
  • 0 in reply to Jasper Li
    Prodigy 180 points

    Jasper,

    We have done the changes, attached images below contains 3D view and pcb layout view.

    New changes include:

    C22 capacitor is rotated and placed close to IC.

    Lot of vias to PGND.

    SW Pin track to inductor is passing through C22 with 19mils clearance. Will there be any issue here?

  • 0 in reply to Jasper Li
    Prodigy 180 points
    Jasper,

    We have sent the board for fabrication. Will let you know here about the performance of the boost.
    Thank you for the support.
  • 0 in reply to Jasper Li
    Prodigy 180 points

    Jasper,

    We have populated the new board with TPS61092 IC . We have taken some screenshots of the CRO at SWpin.

    Kindly note the behavior in below photos of SWpin and let us know the feedback if this is normal or snubber circuit is needed.

    1.Pulse behavior on No load condition. (Very less switching is noticed)

    2: We connected 56Ohms load. (Behavior noticed on SWpin)

    3. We connected our main application raspberry pi and here are switching pin output below:

    4: When we reduced input voltage to 3.7V at TPS61092 input we got below results at swpin: (very high switching was noticed)

    Thanks,

    Macjan

  • 0 in reply to Macjan Camilo Fernandes
    TI__Mastermind 46905 points
    the waveform look OK.
    to check if need snubber, please zoom in the SW waveform at maximum load condition to check the voltage spike. you can add snubber if the voltage spke is higher than 9V.
  • 0 in reply to Jasper Li
    Prodigy 180 points

    Jasper,

    The output is very stable.  
    Regarding LBI pin. We have calculated resistance for 3.7V minimum input voltage.
    R60 = 1.87M, R61 = 290K. Please see the waveform we are getting on LBI pin.

    Blue signal represents EN pin voltage.

    Yellow signal represents LBI pin voltage.

    Can you please help us find out what can be the problem here?

    Thank you,

    Macjan.

  • 0 in reply to Macjan Camilo Fernandes
    TI__Mastermind 46905 points
    it is strange. the LBI is just input pin, and shouldn't cause this problem. is the input voltage stable or if there is anything any connected to this pin.