LM5181: EMI placement review

Bob Shaikhvand

Part Number: LM5181

Hi,

We are having some EMI issues with our board and I would like to rule out any placement and layout issues with LM5181. The layout is very similar to what is recommended in the datasheet.

Following is the schematic, placement and the layout of the part.

Please advice if you see issues with the design and also how to improve EMI.

Thanks,

Bob

over 3 years ago

0 Samuel Jaffe over 3 years ago

TI__Mastermind 25590 points

Hello again, Bob!

Please tell me more about the noise. What frequency band and what measurement technique?

One consideration on the schematic is the zener voltage of D50. 24VIn with a 24V zener gets you a ~48V spike on SW. Choosing a lower zener voltage reduces this spike (and reduces EMI) but will extend the duration of the spike.

The layout places C2 far from the VIN and GND pins. This capacitor should have a low-inductance path from VIN, through the cap, to GND in order to handle high-frequency noise. Place this capacitor to the left of C96 and move the EN/UVLO trace to a mid-layer.

You could also move the IC and surrounding components to the left a bit while keeping D50 and D52 in place. That will reduce the length/area of the noisy SW trace.

Lastly (and this is harder to test) it may be less noisy if you swap the pins of the transformer on the primary and secondary sides. Transformers are not typically symmetrically constructed. The dot usually signifies the start of the winding, often at the bottom or inside if there are multiple layers. This should be connected to SW because the lower/inner windings are shielded better by the PCB GND plane and outer windings when compared to the top/outer windings.

Other than those recommendations it looks pretty good.

-Sam