Solder Paste Mask Expansion for QFN44 footprint

[Luca]

During the footprint creation in Altium Library, QFN44, i've done the Paste Mask reduction for the big center pad as the image shown.
Did you also take in account the reduction for every pins pads? Or just leave the job to stencil manufacture?
Did you use different pin shape for mark the first pin of IC?
And last, but not least, which pad geometry did you adopt?

[mairomaster]

It looks perfect to me, the way you've done it. You normally don't want reduction on the pins. The shape of the first pin is up to you. Before I used to use rectangular pads for everything. A few months ago I switched to rounded rectangle for the pins of all components with more than 4 pins, since it is recommended by IPC for better solderability. With the components with less than 4 pins I didn't bother switching. I haven't had problem with either of the shapes - as long as the dimensions are right everything should be fine with the assembly. We've had problems mostly with BGA packages, but there you always have round pads anyway.

[Luca]

Thanks for fast reply, in that case the pad dimension is 0.3 x 0.9 mm with round shape that's different from rounded rectangle, as you know.
Wich corner radius and pad dimension did you use for rounded rectangle shape?
The solder mask exspansion is 0.04 mm and no paste mask modification, i've read in a document that for chip with 0.5 mm pitch the reduction of
the paste mask should be between 2 to 5 mils (0.08 mm in average). Actually i'm at work in SMT line and i can't search that document for link here.
Do you know if your stencil manufacture do the reduction for each pin with similar geometry and fine pitch?

[mairomaster]

I am using the default - 50%, it looks good to me. For pad dimensions I use either what is recommended by the manufacturer or whatever the Altium IPC footprint wizard generates.

I use 0.05 mm solder mask expansion for 99% of my components. Here and there I will have a very small pitch BGA (0.4 mm for example) which will require smaller solder mask expansion. I've never used paste mask expansion for component pins - I always leave it to 0, no problems so far.

The stencil manufacturing is handled by our assemblers so I am not sure what they do.

[Luca]

Thanks for reply, so you suggest to do not the reduction also for pad and, if it's necessary, the manufacturer of stencil do for us?

[mairomaster]

I suggest doing a reduction for the big ground pad as you did already and not reducing the pin pads. It's best to speak to an assembly specialist about the stencil manufacturing. I know it is a complicated topic and it depends on many things - the solder paste the assembler uses, technology used, pick and place machines, ovens, temperature profiles, etc.

[Luca]

Yea i know, i work in SMT assembly house, for the moment... and i never take in account this stencil design before this project that it's slightly different from other customers.
Simply i receive the stencil and use it, for my personal project i can't ask too much because my boss don't like... but i'll try to take some information and then, if is possible, i post here for other forum users.
Thanks a lot mairomaster for your time!

[Luca]

This is the first:

https://www.multi-circuit-boards.eu/fileadmin/user_upload/downloads/leiterplatten_design-hilfe/ipc-7526.pdf

Second:

http://www.smta.org/chapters/files/SMTA_India_05_SMTA_Presentation_Workshop_on_SMT_Stencil(R1).pdf

[robertferanec]

Luca, awesome documents!

[Luca]

Thanks Robert, i'm looking for other documents and "tips" from stencil manufacturer that we have here in my region, not so far from where i work every day in a P&P machine...
I hope to post here early.