LTM8002 PCB Layout

Hello all,

Regarding the LTM8002 Recommended PCB Layout, I wanted to know if the following components layout is acceptable (compared to the recommended datasheet layout):

Pros: 

1- Output capacitor ground return path loop is much shorter than the recommended layout

2- Signal ground is more isolated from power ground (connected only to A7 pin)

Cons:

1- Feedback resistor is placed at bottom layer, and the resistor connection to ground is a bit longer - can it cause problem? 

Can someone say why I shouldn't  use this layout?

Thanks!

Nir



.
[edited by: Nir76 at 1:00 PM (GMT -4) on 28 Sep 2020]
Parents
  • 0
    •  Analog Employees 
    on Oct 7, 2020 5:33 PM

    Hello Nir,

    Since this is a buck converter, longer ground loop from the output is not a concern. The output of a buck converter is an inductor, hence the current is continuous. In this case, there is not a high di/dt current along the ground from the output cap. Isolating signal ground from the power ground is always better, but unfortunately we are battling with other sacrifice, such as our FB pin.

    Fb pin is a high impedance node, in other words, an antenna which will pick up, literally, everything. So, i would definitely make sure FB pin to be super short and isolated from anything else.

    I hope that answer your question.

    Best Regards,

    Owen Jong

  • Hi Owen,

    Thanks for your reply!

    Regarding the FB pin, actually the additional section (in yellow) is about 5mm long, and I can route it between two GND internal layers. Of course that it is best to use the shorter route, but under this condition - do you still think that this is a risk?

    I still can't understand how placing the FB resistor GND connection right at the power GND path will not effect the FB voltage...surely the FB GND will not be as "quiet" as using a separate GND away from the high return currents...dont you think?

    Thanks again,

    Nir

  • +1
    •  Analog Employees 
    on Oct 7, 2020 6:18 PM in reply to Nir76

    Nir,

    If you burry the FB trace in between ground, it would probably be better, but i'd still prefer shorter trace. Since this is a module, i wouldn't know how the fb trace inside the module was routed, so i don't want to add more risk into this.

    The so called noisy ground of this module is already isolated on the input side of the module. For buck converter, noisy ground comes from the input loop (Vin cap, Top Fet and Bot Fet) not on the output.

    The FB voltage is affected when there is too much current where there is a DC voltage difference between PGND and Quiet GND. If the current is only 2 to 3 A, the offset will be miniscule to even notice, hence this is a lower risk sacrifice.

    Best Regards,

    Owen Jong

  • Ok Owen, Understood.

    Thanks for your quick replay, you've been a great help.

    Nir

Reply Children
No Data