Platform forum

PCB not working after few days

Naveen-Krishnan , 07-13-2020, 07:41 AM
Hello guys,

I hope everyone is safe during the health crisis. Take care !
I designed a product which includes SAMA5, DDR2, Ethernet, RGB24, SD CARD, NAND Flash and Modem 4G. The product was tested, we did 5 revisions of the prototype and validated before it was sold to the clients.

During the validation and prototyping phase we did not face any issues with the PCB. But when the products are sold to the clients,
1. The PCB is short circuit after 10 or 15 days
2. The MIFARE chip MFRC630 chip becomes non functional
We are facing issues like these.

I tried to remove all the capacitors in the voltage rail which was short circuited, but still the Short circuit was there. I think the processor or some other ICs like Ethernet PHY, Audio codec is damaged.

For some unknown reasons the MIFARE chip MFRC630 is often getting damaged. Just to be sure I checked the layout guidelines once again, whether I have missed something or not. But it seems the I have followed the recommended schematics and layout.

Not all the PCBs are non fucntional, but for example if we have sold 50, 6 or 8 products is returned with the above mentioned problems.

Please can anyone give me some lead what could the problem ?

robertferanec , 07-13-2020, 08:51 AM
Have you tested your product for ESD? (just first idea)
Naveen-Krishnan , 07-13-2020, 08:55 AM
Hello Robert Feranec,
Thanks for your reply.

Yes we did ESD testing during validation phase.

robertferanec , 07-15-2020, 02:16 AM
It looks, that there may be something wrong in the design. I would recommend to double check the schematic.

These videos may help:
- Do you check your schematic the same way? https://youtu.be/CDAuCchchtI
- 10 Tips for Better Schematic Checking - Processor Boards https://youtu.be/LzlAmPy0VNQ
Naveen-Krishnan , 07-20-2020, 08:15 AM
Hello Robert Feranec,
I followed the schematics check that is present in above link. I couldn't find anything wrong with the schematics design.

The problem is often related to
1. DC - DC Converter IC failure ( TPS65251 )
2. Audio codec TLV320AIC3120IRHBT IC failure
3. MIFARE Chip MFRC630 IC failure

I think the problem is with the layout. I came across the following article :

Not sure though. I will try to improve the layout in the next REV by again verifying the design guidelines in every IC datasheet and adding more GND pours.

Its really frustrating !
beamray , 07-24-2020, 11:22 PM
hey, have you washed your boards after soldering?
soldering flux's salts can behave like that. after some time when they consumed some air (or liquid) water they can provide path for current. I had such problems with no-clean flux.
robertferanec , 07-25-2020, 01:05 AM
@Naveen-Krishnan I asked about ESD as once we had a very similar problem. We had an audio chip with separate analogue and digital ground connected through a BEAD. When ESD pulse was applied to an audio input or output, the audio chip was damaged. We replaced the bead which was connecting the grounds with 0R and that fixed the problem - ESD pulse was discharged through GND plane and did not damage the audio chip.

If your audio chip is damaged, that may also cause the other problems e.g. DC-DC failure.

If there is no issue in schematic (e.g. all the signal and power levels are ok, all inputs and outputs are connected correctly) and if you do not have ESD problem .. hmm, then I am not sure.
Naveen-Krishnan , 08-27-2020, 02:46 AM
Hello Beamray,
Thanks for your response. I will check with the PCB manufacturer thanks for the lead.

Hello Robert Feranec,
Yes you are right with the Ferrite bead. I am using Ferrite bead to seperate Analog and Digital grounds in the Audio chip. I took this reference by seeing some of the motherboard designs. In the datasheet of the Audio chip they havnt mentioned anywhere to use Ferrite bead to seperate the grounds. So I will replace them with 0Ohms.

With the DC DC converter I saw some schematics issues, for example Sync pin in TPS65251 wasn't tied to GND and instead of using 4.7uH we used 47uH. I will rectify those.

With MFRC630 failing : I think it is related to DC DC Regulator placing of components and routing. I missed some critical layout recommendations and because of that the Voltage rail is not clean. Will rectify that also.

Thanks alot for your insights and help. It means alot to me.

Use our interactive Discord forum to reply or ask new questions.
Discord invite
Discord forum link (after invitation)

Didn't find what you were looking for?