Electronics > Manufacturing & Assembly

Solder paste coverage for large pads?

(1/3) > >>

knotlogic:
Is there any rule of thumb when deciding the size of the solder paste aperture for large pads, especially like with exposed pad QFN packages?  I've seen recommendations to break up larger areas into a number of smaller ones, but nothing that talks about how large/small to make the smaller areas, or what percentage coverage to aim for vs the original.

mrpackethead:
Almost certainly ( at least for any decent manufacturer ) there will be recommended solder paste patterns for a package in datasheets etc.  The rule of thumb would be to use those.

evb149:
There are many application notes specifically about solder paste design for QFN type components.

In general you should divide pads larger than roughly a couple millimeters in diameter into a checkerboard or similar pattern of paste squares on something like a 1.1-....3mm pitch in X and Y directions, and make each paste pad somewhere around 1mm * 1mm in diameter X and Y.  You want roughly between 50% and 75% of  the exposed pad area to be covered with solder paste with 70% being said to be a good target.  There are limits on the stencil aperture sizes and the sizes of the "spokes" of stencil material between the pasted areas so that will dictate your paste pad and paste pad pitch sizes, usually 0.3mm clear area between pasted pads is called for.

Many stencil designers can accept a PCB gerber set with top / bottom "pad master" gerber layers (or just top and bottom copper layers as less preferred).  The "pad master" layers should include all pads to be pasted and the pads on that layer should be 1:1 scaled (no swell or shrink of dimensions) to the actual copper pad of the PCB footprint.
If a stencil maker service gets a 1:1 scaled pad master layer set from you for pads to be pasted then usually they have CAM software that can adjust the pattern of the stencil according to the various DFM guidelines about how much paste should be on each sized pad depending on the type of component and copper pad size.

Of course low cost low service manufacturers MIGHT not do that CAM for you.  I am actually not sure about current practices of the "super low price prototype PCB / stencil" manufacturers in that regard.  But any "normal" industrial PCB manufacturer will outsource or otherwise handle the stencil design CAM to this extent for you so you just give them enough data as to unusual requirements for your board and devices and they make the stencil according to their usual DFM practices.  Some ICs will call out a very specific paste pattern to be used for their lands so in such cases you should call that requirement out in your fabrication notes and maybe just implement that pattern in your paste layer for those specific ICs but make the rest "generic" 1:1 pad to paste representations on your CAD paste layer.

A search engine fed keywords like "qfn footprint" "qfn land pattern" "qfn thermal via" "qfn solder paste" will turn them up.

Here are some file names which may be relevant, but some are probably on other DFM / soldering / layout topics because I did not have them sorted fully:

001-72845_AN72845_Design_Guidelines_For_Cypress_Quad_Flat_No_Lead_QFN_Packaged_Devices.pdf
2011-03_ASQ-QFN.pdf
20160001774.pdf
an-1028.pdf
AN-772.pdf
AN862.pdf
appnotesLGA0902.pdf
BoardLevelQFN.pdf
Carsem MLP users guide.pdf
MLFApplicationNotes0908RevG.pdf
QFN_AN.pdf
S2083.pdf
screaming_5myths.pdf
SKYA21004_AN_203721A.pdf
slma002g.pdf
AN2409.pdf
apdesign.pdf
Increasing use of High Density Interconnect Printed Circuit Boards.pdf
PCBCADGuidelines.pdf
PCB-Nov2016.pdf
Q&A-from-Deep-Dive-Webinar.pdf
slma002g.pdf
slma004b.pdf
sloa120.pdf
Via_Fill_Plug.pdf
Via Interconnect Holes June 2012 Final.pdf
QFN Layout Guidelines.pdf
AN0001.pdf
AN10365.pdf
AN1902.pdf
AN3778.pdf
AN4530.pdf
AND8211-D.PDF
ssembly_challenges_bottom_terminated_ipc.pdf
Carsem MLP users guide.pdf
centellax_appnote_an08__surface-mount_qfn_package__general_handling_and_assembly.pdf
doc8583.pdf
Empire_Proven_Approaches_to_Minimize_Voiding_under_QFNs.pdf
sbou108.pdf
sloa122.pdf
slua271a.pdf
smt_assembly_for_leadless_packages.pdf
tb389.pdf
the_bga_qfn_repair_process.pdf
slua271a.pdf

knotlogic:

--- Quote from: mrpackethead on July 13, 2017, 12:35:25 pm ---Almost certainly ( at least for any decent manufacturer ) there will be recommended solder paste patterns for a package in datasheets etc.  The rule of thumb would be to use those.

--- End quote ---

Looks like Atmel might not be one of those decent manufacturers...  ;)  Or I've been doing a terrible job of searching for them.  But I've also been looking at various power LED packages from smaller manufacturers, and.... it's messy.  There's a 2835 package that appears to be an industry standard, but there seem to be rather different PCB footprints between manufacturers!

evb149, thanks for the list!  That's going to take me some time to get through though.  70% is rather small though, not to mention 50%!  I was guessing 80% but now that seems way too much.

I've been using EAGLE thus far, and IIRC the paste layer is automatically shrunk a certain amount relative to the copper layer, although it's possible to delete it and insert one's own during footprint creation.  I need to check that.  (I also need to start using CircuitStudio, but that's a different matter entirely...)

I'm not doing any commercial manufacturing with this, and am probably going to go with OSH Stencils for my first time round.

jmelson:
For QFNs with exposed pad under the chip, the amount of solder paste must be reduced a LOT, or the chip will pull down and squeeze the solder out to the rows of pads, shorting everything out.  Many people make "window frames" by making a number of squares with clear stripes between them.  This arranges for the solder to be spread across the pad but still reduces the total solder volume to prevent the shorts.

Larger parts can use 100% aperture to pad size, as the lead pitch is reduced, then you have to make the apertures smaller to prevent bridging.  I sometimes have to go down to about 50% area for 0.5 and 0.4mm lead pitch.

Jon

Navigation

[0] Message Index

[#] Next page

There was an error while thanking
Thanking...
Go to full version