I am using this gate drive for driving a PFC boost circuit mosfet. In the datasheet's pin description (shown below) it is stated that the agnd and pgnd grounds should be seperated.


However in the application information (shown below) it says that the agnd and pgnd pins should be connected with a trace.



What am I supposed to do? I want to keep the grounds isolated from each other but I'm worried that it will cause me problems.

this is the link to the datasheet : https://www.alldatasheet.com/datasheet-pdf/view/85238/TI/UCC37322.html

 

Top picture if from TI. Bottom one is how I would have made it.
When making symbols,
1-make them look like the PCB, in this case pins 1-4 and 5-8 just like the layout. (not random numbers)
2-make them so you can see the function. (not a blank box)

You might also consider this symbol.

Pins 1-8 are connected internally. Pins 4-5 are connected inside.
You need a capacitor from pins 1-4. small cap very closely connected.
You must have capacitor(s) connected 8-5. Very close to the IC. !!!! This is a high current connection. You might see 8A spikes. Wide traces! Fill the PCB with copper. Connect 5 to the Source of the MOSFET. I would connect 5-Source with a trace as wide as the IC's pin (or wider). This trace is not part of the ground fill. Then 4-5 with a thin trace. Keep 7,6 to Gate short! Keep 5-Source short!
Pin 1-8 thin trace. Pin8-cap(s) wide trace. Think 8A.

 

Thanks for your reply. I see what you mean aobut the symbol and totally agree. It's just a symbol that came with the footprint so I didn't change it. I have the 2 capacitors (C16 and C17) which will connect pins 1-4. I have 2 more questions:

1-) I will need to connect the agnd and pgnd pins with a single trace correct?
2-) If I use a ground plane (this plane whill only be on the analog side of the ic) for AGND then should I still connect the trace between agnd and pgnd?

Thanks again.

 

Data sheet is best from TI.COM. The AllDataCheets are hard to use. IMO

1-) I will need to connect the agnd and pgnd pins with a single trace correct?

Connect a single trace between the two VDD pins (pin 1 and pin 8);

2-) If I use a ground plane (this plane whill only be on the analog side of the ic) for AGND then should I still connect the trace between agnd and pgnd?

connect a single trace between PGND and AGND (pin 5 and pin 4). If a ground plane is used, it may be connected to AGND; do not extend the plane beneath the output side of the package (pins 5 – 8).

I think TI wants pin the ground plane to not connect to pin 8.
Inside the IC there is about 15 ohms from 4 to 5.
You want a very small loop from IC to Gate and back Source to IC. One option is to connect 6&7 to resistor then to Gate in a direct line. Wide traces. Then bring the Source back, wide trace. Make the out and back in parallel lines.
TI you can also take 6&7 to on the topside to Gate and Source coming back on the next layer down. This makes the area of the loop smaller. Use several VIAs in parallel if you are changing layers at high current.

 

Got it. Thank you!