solder paste offset from pads

While making a DFN footprint landing pattern for a Sensirion SGP30 Gas Platform sensor, I encountered these instructions.

"It is recommended to design the solder mask as a Non-Solder Mask Defined (NSMD) type. For solder paste printing a laser-cut, stainless steel stencil is recommended, with electro-polished trapezoidal walls and with 0.125 to 0.150 mm stencil thickness. The length of the stencil apertures for the I/O pads should be the same as the PCB pads. However, the position of the stencil apertures should have an offset of 0.1 mm away from the package center, as indicated in Figure 12. The die pad aperture

resulting in a size of about 1.05 mm x 1.5 mm."

A datasheet drawing clearly shows the offset. The stencil paste aperture is the same size as the pad, but appears to fit within the mask.

The TI document SLUA271B doesn't mention offsets. I see the IPC-7351B standard costs $160, but not sure if it'd be helpful for specialized sensors.

--
 Thanks, 
    - Win
Reply to
Winfield Hill
Loading thread data ...

It's probably to improve the self-centring. The surface tension of the solder fillet produces a restoring force that is (iirc) cubic in the displacement. Displacing the pads a bit makes the force linear in displacement, which improves the self-centring.

Back when I was doing on-chip optical communication, we had various schemes for doing that sort of thing, including different melting points, offset pads, and so on.

Cheers

Phil Hobbs

--
Dr Philip C D Hobbs 
Principal Consultant 
 Click to see the full signature
Reply to
Phil Hobbs

Winfield Hill wrote in news:qa6plk014q2 @drn.newsguy.com:

It appears that it wants you to have pad area outside the chip package perimeter to allow proper wicking of the solder and for inspection of the joint (in the 63/37 days we actually inspected joint quality). It is very similar to the old "castle" dual flat pack design configuration some old ceramic chip carriers had. It was little sculpted cups at the edge that extended vertically on the chip. Like little vias that got cut in half.

You could make a PCB to mount the DFN device onto and then mount that to the main PCB assembly as a daughterboard, making it far easier to service or adapt a newer version to. The footprint is almost the same as far as real estate taken up. Actually being a daughterboard suspended above the main, that real estate could be recovered for more parts to be placed under this module.

Reply to
DecadentLinuxUserNumeroUno

Yes, makes sense. They also want the paste aperture inside for the thermal pad. I made the pad in four 0.6 x 0.8mm sections, per other vendor suggestions. I couldn't get Altium to let me specify these things, so made each layer (pad, solder mask, paste aperture) separately, differently for the pins and thermal pad. I'd like to know what I'm doing with this weird stuff.

--
 Thanks, 
    - Win
Reply to
Winfield Hill

Phil Hobbs wrote in news:- snipped-for-privacy@supernews.com:

Absolutely correct. At the moment of reflow, both molten solder and flux present will self center some devices and form perfect solder joints if the stencil was not too thick.

That fillet of solder uses that force to do just that. Without the offset, their is no fillet to tug on the device, and the chip actually ends up on top of a set of solder 'pillows' (can't call them balls as that term is specific), that typically would be a fail on inspection as one cannot guarantee that all pads got 'pillows' under them.

Can't beat 63/37. Those days are gone though. Tin alloy solder joints all look very grainy and they had to change the entire IPC acceptance spec to handle the stupid RoHS switch European paranoids placed on the world. Failed satellites and who knows what else later, and they still haven't figured out that the metallic form lead in a 63/37 alloy solderd PCB assembly does NOT leach out into ANYTHING, much less the water table.

Go to any of hundreds of outdoor firing ranges and find a gazillion lead slugs in the ground, yet no rise in local water table lead values.

But yeah... You hit it dead on. SMD technology design parameters were all about self centering using the surface tension... The RoHS came along and tin alloys do not flow anywhere near as well as the

63/37 we spent years declaring was the best. So the self centering thing may not even work very well at all any more.
Reply to
DecadentLinuxUserNumeroUno

Hah, my board only has three small sensors, plus a few caps and resistors, so it is the "main PCB".

--
 Thanks, 
    - Win
Reply to
Winfield Hill

I do that with the EPC GaN fets, tiny BGAs, because they are very fragile and very difficult to rework. The baby boards become throwaways.

formatting link

formatting link

--
John Larkin         Highland Technology, Inc 

lunatic fringe electronics
 Click to see the full signature
Reply to
John Larkin

Winfield Hill wrote in news:qa730901io0 @drn.newsguy.com:

Heheheh... I see (e few things and only a few things) said the blind man...

I saw one with a fool bore cpu next to it on their site.

Reply to
DecadentLinuxUserNumeroUno

John Larkin wrote in news: snipped-for-privacy@4ax.com:

the

Those look good. You could use large vias and post pins to solder it down and actually get some heat transfer through them. A tiny bit less easily servicable but still easier to swap than right on the board, just like you say.

But since they are baby boards, it would also be easy to reflow it and wipe the parts and reuse the board. Smaller carbon footprint and all that. Not on a customer repair though.

Reply to
DecadentLinuxUserNumeroUno

The mouse-bite boards solder down as surface-mount parts

formatting link

(the ones in that pic are not glob-topped)

and transfer heat fairly well. We hand-solder these.

We have a Metcal tweezer sort of thing that can pluck a baby board right off.

--
John Larkin         Highland Technology, Inc 
picosecond timing   precision measurement  
 Click to see the full signature
Reply to
John Larkin

Don't worry about it:

  1. The mask fab will do the most obvious things themselves (e.g., break large regions into grids). Also typical is making a dogbone or chevron shape for bigger chips (0805+).

1a. Unless you're starting up your own assembly house, expect to do a lot of rework anyway. Pasting saves time over 100% hand soldering, but don't expect it to be perfect your first time, or even your 100th time.

In short, without having any existing process control to speak of, you aren't going to save much time doing tweaks on the front end -- in particular, you won't have any chance to feed changes back into the process.

I'm assuming this is a one-off sort of thing, hence why it hasn't come up before, and may not come up again (but, again again, if you _are_ starting up an assembly house--).

  1. A CM will already have their process dialed in, so will make tweaks to the paste layer to their satisfaction (if you provide a modified paste layer, they'll probably just regenerate it from pads, using their own rules and geometry?).

Concentrate more on getting the pads IPC-compliant. You'll see all sorts of bizarre footprint dimensions in datasheets, but IPC rules exist because they give consistent results.

On that note, some packages are ridiculously loose. JEDEC packages in particular. TO-220 is awful, sure, but DO-214 is as well. Most manufacturers give a footprint that's closer to an IPC "high density" (reduced outline) footprint, but which violates (according to IPC rules) the very drawing they give. Because, of course they give the JEDEC DO-214 with its shitty tolerances, why give the internal drawing with correct tolerances? But they give the footprint from it. So, presumably, you can infer some dimensions of that drawing with modest confidence, based on their footprint. From this, you can draw a regular IPC footprint, of whatever "density" you like.

Again, feedback is possible (maybe the ideal pads are slightly different, for various reasons), but only if you have a closely coupled process.

Another note, don't be afraid to shave pad widths. Some TSSOP, MSOP, etc. have suspiciously wide pins, for which you can't possibly have positive side fillet AND soldermask between pads. The IPC tolerance for side fillet is -0.03mm so a little pad shaving is perfectly acceptable. For 0.5mm pitch, 0.22 to 0.25mm width pads usually leave enough space for soldermask, assuming 3-4 mil minimum web width, and 2-3 mil soldermask expansion. Correct soldermask is best; but if you can't manage it, no soldermask is better than too-thin webs flaking off, adhering to pads and causing open joints.

IPC-7351 is available for free and isn't much different from the latest version, at least in terminology and rough values. You can usually find copies of such documents floating around on suspiciously-public websites, indexes or FTPs; give it a quick search.

Tim

--
Seven Transistor Labs, LLC 
Electrical Engineering Consultation and Design 
 Click to see the full signature
Reply to
Tim Williams

ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.