0
\$\begingroup\$

I am designing a footprint for the SOT765-1 using Altium CircuitStudio, and I am a bit confused regarding the solder paste and solder land definitions found on Page 3/5 of this datasheet. For the bottom-left pad, should I make the pad 0.3mm × 0.65mm and set the "Solder Mask Expansions" to 0.1mm? And can I consider solder land to be a synonym of copper pad?

\$\endgroup\$
0
\$\begingroup\$

This datasheet uses the term "Solder Land" to define the suggested size of the copper pad. The manufacturer recommends a 0.4x0.75 "Solder Land" (copper pad) for the bottom left of the drawing (pin 1), as well as pins 4, 5, and 8.

The suggested solder paste shown by the drawing is 0.3mm in the X dimension, but is not given in the Y dimension. You can infer that the manufacture is suggesting to make the solder paste 0.1mm smaller than the copper pad in both axes. So, the solder paste opening should be 0.3x0.65mm.

In order to automatically achieve this, Altium uses the "Paste Mask Expansion" property for the pad in the library. Altium interprets the value as the expansion if positive, or pull back if negative, from all edges. In order to achieve 0.1mm smaller solder paste than the copper pad, the Paste Mask Expansion value needs to be set to -0.05mm.

I'm using Altium 19 as the reference.

| improve this answer | |
\$\endgroup\$

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.