Hello Friends
I am putting a 0805, 10V, 1uF capacitor footprint into Cadstar.
It will be for reflow soldering,.
Do you think that the solder resist mask should extend 0.1mm further outside the pad.?
And do you think that the solder paste mask should come up to 0.07mm from the edge of the pad?
To summarise:
The pad is 0.9x1.25mm
So the solder resist mask should be 1.1 x 1.45mm?
And the solder paste mask should be 0.76 x 1.11mm?
Those numbers should be ok.
I set the solder mask swell to 0.1mm in PCAD and Altium Designer.
The solder paste I set to the size of the pad or slightly smaller.
If you follow it, the IPC7351 standard requires that solder resist is supplied to the manufacturer at 1:1 so that they can adjust it’s size
as per their own processes as some will require an 8 thou oversize while others may only require 4-6 thou.
(or whatever the mm equiv is).
Same suggestion goes for the solder paste layer - Either set this as 1:1 and let your screen manufacturer reduce the pads by
whatever percentage you ask for overall (usually 10%). Or if you want to be able to specify it then do some sums on how much solder you want on the pad/component joint then use that value (or simply use slightly smaller TBH the difference is negligible).
Don’t forger that in CADSTAR if you reassign a paste or solder resist layer on the top you should also do it on the bottom.
That way if you mirror it onto the bottom of the board the reassignment is also mirrored.