I am building a board based on a working reference design. I've obtained the assembled board based on my design but the '3V3_OUT' signal is failing to carry power anywhere on the board.

The issue seems to be with the power mux (TPS2113ADRBR) as this is where the 3V3_OUT signal is distributed. I am measuring no voltage on the OUT pin (pin7). The two voltage input pins (battery and USB) are both measuring 3.2V (pin6 and pin8 respectively).

I am very much learning this stuff and may be in over my head but I do notice that there is no via under my mux, I am not sure if that may be of concern. Ground planes are used for both layers.

My design which is not producing voltage out on pin 7: enter image description here enter image description here

The reference design which is correctly working: enter image description here enter image description here

The schematic used for both designs: enter image description here

  • \$\begingroup\$ Please run ratsnest on EAGLE so we can see the ground plane. How much current are you trying to draw from 3V3_OUT? It does have thermal protection, so if you're on the high end of the specified power dissipation it won't work without heat dissipation vias on the pad. The datasheet specifies "Must be connected to large copper area in order to meet stated package dissipation ratings." \$\endgroup\$ – MapleTronix May 7 at 18:37
  • \$\begingroup\$ @MapleTronix I've updated the images with ratsnest run. I'm measuring .10 mA on 3V3_OUT. What you are describing would make sense as I failed to place vias throughout the board and under this mux which my reference design did do. Is there a way I can test that thermal protection is preventing operation? \$\endgroup\$ – nullsec May 7 at 18:58
  • \$\begingroup\$ Did it get hot? Any thermal camera? \$\endgroup\$ – Unknown123 May 7 at 19:19
  • \$\begingroup\$ You show a complete different PCB. Is this how it has been produced or is it the suggested new one? \$\endgroup\$ – Huisman May 7 at 19:53
  • \$\begingroup\$ @Huisman I've updated the images with ratsnest showcasing the ground plane. The second image is the already working design. The first one is my design which involves a different layout. In my re-routing it seems that the ground plane EAGLE draws gets isolated in certain areas thus leaving some GND pads unconnected. So it would appear that your original answer may be correct although for components not shown in the picture. I've patched the GND connections for some of these and I'm now getting a voltage on output, although much lower than anticipated. \$\endgroup\$ – nullsec May 7 at 20:19

You didn't connect pin 5.
I would suggest trying to make a connection south or east of pin 5 to the ground plane by carefully scratching the FR4 above that ground plane. However, C46 neither seems to be connected to GND. If there are more unconnected components, you'd better redesign the PCB. See yellow arrows in picture below.

Make sure you use a DRC. DRC would have detected these unconnected components.

enter image description here

  • \$\begingroup\$ Always do a DRC check on designs, and set up the DRC right \$\endgroup\$ – Voltage Spike May 7 at 18:37
  • \$\begingroup\$ DRC did show my GND pins as unconnected but with the ground plane I made the assumption (maybe a wrong one) that routing those wouldn't be necessary. The eagle project file I was referencing had done the same and I have that working board in hand. \$\endgroup\$ – nullsec May 7 at 18:48
  • \$\begingroup\$ No. They did not automatically connect. \$\endgroup\$ – scorpdaddy May 7 at 18:57

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.