Footprint for PIC16F18856 (6x6mm QFN)...no solder resist to be used beneath part?

Hi,

We are doing the PCB footprint for the 6x6mm QFN version of the PIC16F18856.

The recommended land pattern , on page 664 of the datasheet gives no recommendation for solder resist masking.

As such, we have put absolutely no solder resist anywhere under the body of the part. This is because we believe that solder resist would hold the part up off the board during reflow, and prevent proper settling of the part onto its pads. Do you agree with this?

Even if we put solder resist beneath the part, the gap between centre pad and outer pads is too narrow, and so we would get smatterings of solder resist over the pads, which would make the part even less likely to properly settle on its pads during reflow....do you agree?

The land pattern dimensions and the solder resist mask are shown attached.

PIC16F18856 datasheet
https://ww1.microchip.com/downloads/en/DeviceDoc/PIC16LF18856-76-Data-Sheet-40001824D.pdf

Soldermask dimensions are adjusted according to PC design class. A usual soldermask enlargement for fine pitch PCB is all round 50 µm. This gives 100 µm solder mask dam for the pads in the 6x6 mm 28 pin QFN footprint. You have set the exposed pad size landing to maximum, which is probably no good idea. If would reduce it e.g. to the nominal pad size.

Thansk, but i always worry about using nominal pad width, as the part may land on a bit of solder resist and get stuck there, and thence not settle onto the footprint?
Also, i used the footprint dimensions from the part datasheet

Hi,

Don't worry about the thickness of the solder resist. Nowadays one uses laqueur. (In former one used relatively thick solder resist foil).
The IC maybe doesn't settle directly on the PCB, but the solder will do it's job.

Klaus

Also, i used the footprint dimensions from the part datasheet

Click to expand...

No, you used the maximum size without considering if It's appropriate.

No, you used the maximum size without considering if It's appropriate.

Click to expand...

Thanks, yes, page 649 of the datasheet does list the "MAX" sizes, but this is what is in the recomended land pattern on page 649. Its X1 by Y1 which is 0.37mm by 1mm.....its exactly what we have done...ie we copied microchip's recommendations.
I am quite prepared to accept though, that the recomended land pattern is incorrect.

Hi,

Solder mask thickness on the PCB surface is 1 to 2 mill max , Component leads will come with 1 mill height shown in package drawing on page no :652 check A1 value. Thermal pad to signal pins you have 0.225mm it more enough. No issue will happen in reflow. No need to follow no solder resist.:-o