FEDEVEL
Platform forum

Karan paliwal , 01-05-2025, 11:45 AM

Hi @Robert Feranec
I want to create a footprint for a BGA package IC(MCXN546VDFT). However, the datasheet specifies three parameters:

1. Solder mask expansion (0.38 mm)


2. Solderable area (0.28 mm)


3. Solder paste stencil (0.34 mm)



I’m confused about determining the ball landing sizes for the following:

Solder paste size

Solder pad size

Solder mask opening


Could you please guide me on what values I should use for each?
DATA SHEET(https://www.nxp.com/part/MCXN546VDFT)

QDrives , 01-05-2025, 02:38 PM

Solderable area = pad size as copper top.
Solder mask expansion = wrong 'name' as it is the opening, which is 0.1mm larger or 0.05mm either side. So 0.05mm is the solder mask expansion.
Solder paste stencil = the size of the aperture in the paste stencil. It is 0.06mm bigger than the pad, so 0.03mm expansion for the paste mask.

Karan paliwal , 01-05-2025, 04:51 PM

@QDrives
Sorry ,I am having a bit of difficulty understanding this. Could you please explain it to me with reference to the BGA ball value(X/Y , PAST MASK EXPANSION, SOLDER MASK EXPANSION)? It would help me gain better clarity. Thank you for your time and assistance!

QDrives , 01-05-2025, 05:00 PM

"*...with reference to the BGA ball value...*" -- and then you show Altium???
These are the solder balls details:

Karan paliwal , 01-05-2025, 05:16 PM

@QDrives
What are the correct parameters for creating this ball? Could you please guide me on what values I should use to define it accurately

QDrives , 01-05-2025, 08:17 PM

You are not creating a "**ball**", you are creating a "**pad**".
Yes, this is language, but if we are not able to communicate in the same language, we are unable to communicate period.

Anyhow, the (package) datasheet already states it for you.
Pad shape = round
Pad size (X and Y) = [Solderable area] = 0.28mm
Solder mask expansion = ( [Solder mask opening pattern] - [Solderable area] ) / 2 = (0.38 - 0.28) / 2 = 0.05mm
Paste mask expansion = ( [Solder paste stencil] - [Solderable area] ) / 2 = (0.34 - 0.28) / 2 = 0.03mm

https://www.nxp.com/docs/en/package-information/SOT2172-1.pdf

Problem with paste mask is that they do not specify for which stencil thickness nor paste type these values are designed for.

Karan paliwal , 01-06-2025, 01:19 AM

Thanku