0.3mm pitch mail order PCBs and toaster reflow

[carl0s]

I was wondering, am I pushing my luck with 0.3mm pitch connectors on my PCB, and stencils ordered online?

Specifically some of LCD connectors I am using have 0.3mm pitch spacing. It seems like not a lot of solder is going to get on there.

My first prototype will use connectors with a 0.6mm PCB pad pitch (it's double row, for a 0.3mm pitch FPC), and even that seems tiny. The actual 0.3 or 0.35mm connectors are ridiculous. (Panasonic AXG series).

Or will it all just work out nicely and flow into place?

[daveshah]

I have hand soldered 0.4mm and 0.35mm LCD connectors before with an extended pads footprint, on ordinary Elecrow PCBs. But whether or not that will work depends a lot on the style of the connector.

[wraper]

It needs to be a thin metal stencil, 0.1mm is preferable. 0.12mm might work but not sure. With very precise alignment when applying the paste. Connector must be placed precisely too. Polymer stencils are useless for this.

[wraper]

Solder paste must be fine enough as well.

[carl0s]

Thanks guys!

Yes I was thinking of extended pad footprints.. make them longer than necessary, and also a fine solder paste.

One thing that's worrying me, is I suppose there will not be any solder mask between such fine pads?

[David Chamberlain]

Yes solder mask at those pitches is probably not going to exist.

You will want to controll the amount of solder by reducing the hole size in your stencil.

[wraper]

I suppose there will not be any solder mask between such fine pads?

Only if you use top of the end factory for PCB production. This sure will cost very extreme at low quantities.

[carl0s]

OK, interesting. It might be a challenge then :-)

I'd better get the PCB design finished.. there's not much to it, but it's my first try.

[jmelson]

The big trick is to make the apertures in the solder mask SMALLER than the pads on the PCB.  How much smaller?
Oh, that's the tricky question.  With a leaded chip, the excess solder paste can squish out between the pins, and then draw back in as the solder melts.  When you have leadless devices, or anything with really fine pitch, any excess solder causes bridges.
So, as the pitch goes smaller, the amount of area reduction for the stencil apertures needs to be increased.  I usually use something like reducing linear aperture dimensions to 60% of the pad for the really small stuff.  I also use .003" stencils, which comes out to about 0.07mm.  But, my apertures are etched, so likely actually come out to a bit bigger than the 60% size as drawn on the artwork.

I think you will end up having to experiment a bit to get the right amount of solder.

Jon

[wraper]

The big trick is to make the apertures in the solder mask SMALLER than the pads on the PCB.  How much smaller?

There is no trick. Cheap factories don't have good enough solder resist alignment to play with things like this. 0.3mm pin pitch? they often have 0.3mm solder resist offset. Even for solder resist between 0.5mm pitch pads you cannot use cheapest fabs and need to pay a bit more.

[Siwastaja]

Yeah, nope, SMD (solder-mask defined - gotta love the super confusing acronym) type pads are not going to cut it.

Maybe jmelson meant apertures in the paste stencil, not solder mask?

[chris_leyson]

Datasheet says pad size 0.2x0.4 with 0.18x0.31 paste mask and 100u stencil. From the CAD data the pin width is 0.12mm so you've got 0.04mm of pad either side of the pin for the solder fillet and a good toe and heal so you should be OK with that size paste opening. Personally I would reduce the paste mask a little bit.

I've seen problems on similar connectors, Hirose DF12 connectors, 0.25mm wide pin on 0.3mm pad with 0.28mm mask opening. The heal on the back of the pin is non-existent and we had a lot of solder shorts at the back of the pin underneath the connector. When we used the recommended land and mask patterns we had solder shorts and the "trick was to reduce the paste mask" and that fixed the shorting problems. That's why I said reduce the paste mask a little bit.

Looks like the Panasonic AXG connector will give you a much better heal fillet when compared to the Hirose DF12. Anyways, good luck with hand placing those.

[carl0s]

Well, luckily, those are bottom of my list. I have a collection of mostly round LCD TFTs here now, and the ones with that style of connector are my least favourite.

Those that I am using to start with are of the double row sort, so a 0.3mm pitch flat flex, but my connector has 0.6mm pads ( https://www.mouser.co.uk/datasheet/2/18/10061122-1274022.pdf )

However, I do also have a big 0.5mm pitch Samtec DSI connector on the same board (https://www.digikey.co.uk/product-detail/en/QTH-030-02-F-D-A/SAM9115-ND/6613651 )


I am basically making an alternate MIPI DSI daughter board (adapter board) for the stm32L4R9i-discovery board, to use instead of the included amoled one.

[wraper]

For 0.6mm pitch, you'll be best with 0.12mm stencil. No solder resist is required between pads. Cheap fabs are still not good enough, you may try but they will either remove it or there likely will be a lot of boards with solder resist partially covering the pads due to misalignment. Or solder resist occasionally missing between pads due to weak adhesion.  Just be sure that there is no offset when you apply solder paste, it's the most important part. Polymer stencil still sucks for this. Basically if you manage to accurately apply the solder paste, you'll be fine.