Heat sink pads under components, extension

Have you tried unsoldering when the pad has the usual bunch of thermal vias to the bottom? If it works OK, then you don't need the rest.

I bought a $99 ($199?) air reflow station from Spark Fun which works quite well. for this sort of thing.

That makes it even tougher because then the GND plane sucks all the soldering iron heat away. What works nicely is to heat the individual pins, slide a thin valve gauge blade through (remember those?), then hold the tips of two Wellers onto the solder sticking out the sides and ... voila. Of course one would technically need a 3rd hand but I usually flick it up gently with one tip.

One of our Labradors would not have this 3rd hand problem. He can scratch himself behind an ear with one hind leg during a dog walk and continue walking at our regular brisk clip on the three remaining paws. Amazing.

Those have a hard time if you have more than 1/2oz copper and the pad is completely covered by the IC. Best way to get it off is to also put the board on a hot plate but that's not going to work when stuffed double-sided.

I have been using the multiple vias methode for years. A proper 80W iron with a big tip does excellent for double sided boards even if the ground plane is continuous. Otherwise I pull out my hot-air station. I've found a hot air station is a very useful tool and they are really cheap these days.

I don't recall using any chips with thermal pads with pins on only two sides. The ones I see this on are mostly quad no-leads, QFN chips. What do you do with those?

Regardless of how large your pad is, it is important to break the solder paste area into segments smaller than the pad. Do you cover the entire pad with solder paste, solder mask? I'm not sure exactly how you do this without impacting manufacturing. If the pad is covered with paste it might well cause the chip to float away, although the pins should prevent that. If you don't cover the pad with solder paste it might suck the paste from under your chip. If you cover the excess area with solder mask, it might impact thermal contact with your iron, or maybe not.

It's chips like this:

I am letting the pad for the bottom stick out on both sides (where there are no pins).

Yep. It's the only way because the paste gets screeded onto anything that doesn't carry solder mask. I want solder exposure on the sides so I can heat things up underneath the IC from the side the IC is mounted.

That is exactly why I am posting, asking for others' experience.

That's what I'd like to know. Can it suck the paste out? Could it float away? Or will it make a solid contact and not float?

If you cover the excess area with

The iron would seriously burn the solder mask.

We use stuff like that, and leadless parts with power pads

I just put 4 or 5 or 8 vias right in the power pad region, no solder mask. The vias usually go right to a layer 2 ground plane, so the thermal path is short.

It gets pasted and soldered, and we haven't had any problems with solder stealing by the vias. Manufacturing can rework these with IR and hot air, so I don't make any provisions for hand soldering from below or from the side.

Sometimes, if I have a lot of heat or want really low ground inductance, I will extend the topside ground pour beyond the actual power pad area and add more vias.

Do you leave some area bare so solder paste is on there? That's what I want to do, to be able to heat it up from the small sides (after lifting all the other pins) until the IC floats up.

Which IC are you referring to? My color vision isn't that great. When reviewing layouts with PADS Viewer I am constantly switching colors.

We use many DFNs and SOICs with pads.

There are three big black pads, each with extended topside copper pours and extra vias outside the part footprint. The PADS part decal has a numbered pin, the power pad, which is the same size and shape as the power pad on the bottom of the part. That shape gets bare copper (nickel/gold, actually) without solder mask, and that's also where we solder paste. That alignment (probably) makes the part self-center when we reflow it.

U9 (green power pad near the center of the board) has leadless signal pads on all four sides, so the topside copper can't be extended out beyond the power pad. It has a bunch of vias inside the pad area to transfer heat out.

I did that layout myself! This picosecond+thermal stuff is often easier to just do than to explain to The Brat, plus I like to keep in practice.

If you're not boxed in by signal pins, you could expose some of the extended topside copper in a couple of strips, just outside of the part outline, as places you could land a couple of hunky chisel-tip irons, to manually desolder if you had to.

I did this for the prototype, and never bothered to change it for production since it did not seem to cause any trouble. Despite the theoretical danger of the via "sucking away" the solder or whatever.

Never had any problem, in fact it is probably the most reliable way of sticking down a 0.5mm pitch part I know of, and I would prefer this package type now. Over normal QFPs, say.

This was total production of ~2k pcs though, so YMMV for millions.

This is why you need vias in the thermal pads. They suck away excess solder making manufacturing painless.

Was it this one:

Regards

Klaus

solder

the

That's what I am wondering about, if this area is larger than the bottom part but only at two side, and stick out the same lenth, will it still self-center?

Is the solder mask free area on the power pad of U9 larger than recommended in the datasheet footprint?

just

I've got too much stuff on my plate which is the main reason why I don't do layouts or software. Sometimes that comes back and bites me.

Right now it's extended and exposed at two sides, making the power pad about 60-70% longer in chip length direction, but same extra length on both sides so the chip still sits symmetrical. It could not really be split into strips or feathers at each end because the parts are so small to begin with. MSOP and such.

Worst case if an assembly house is unhappy with that they could tuck in the solder mask by a layer edit in the Gerbers. Not an ideal procedure but could be done.

The big via is something I've done many times before, that has never caused any trouble. I am just wondering about the extra (solder-pasted) length of the pad. It's 60-70% longer than the recommended one in the datasheet.

This unit won't be produced in more than a few thousand per year.

Oh sorry I must not have read your OP properly. How about a line of mask to form a "solder barrier"?

That's a good idea but my layouter will probably have a fit if I request that :-)

I guess I'll let the assembly house deal with that. We use turn-key so if they don't like it (I will point it out to them) they can do a Gerber edit and we could correct the orginal data set accordingly if needed.

any

usually

pin,

bottom

solder

the

Don't know, but why take the risk? Leave some solder mask to define the inner pad. Open up some windows to the topside copper, outside of the part outline, for solder access.

No, the PADS pad (and stencil cutout) is from the data sheet.

just

desolder

Mostly these things just work.

is

big

unsolder

ends of

needing

is

any

(solder-pasted)

mask

Thinking about this while reading the thread lead to the question of where are the forces coming from. IIRC they are viscous forces so that if the oversize pad extends on both ends the same amount no net force should be created. Then the forces on the device contacts (leads) should keep it self-centered.

?-)

That's also my thinking. However, there are always drafts and whatnot even in reflow ovens so I decided to play it safe. We'll cover it but probably just with silk screen. Then we can scrape that off in a pinch and apply solder.