Heat sink pads under components, extension

[Joerg]

Question to the folks here:

I use more and more parts that have a ground pads underneath which is
also for extracting heat. Usually I ask the layouter to provide a big
via in the middle so I can reach in with a Weller ETS tip to unsolder
from underneath. I also let the pattern stick out a bit past the ends of
the chips so I can unsolder/solder from the top without always needing
fancy heat guns.

Occasionally I had some groanings from producrtion folks that this is
non-standard (which is true) and that the part may slide. Never saw any
of that in a reflow process, but what do thee all say?

 

[Joerg]

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.

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.

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

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.

 

[Nico Coesel]

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

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.

 

[rickman]

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.

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.

 

[Joerg]

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?

It's chips like this:

http://media.digikey.com/Renders/~~Pkg.Case or Series/16-TFSOP Exposed Pad 12 leads.jpg

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

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? ...

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.

... 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. ...

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

... If you don't cover the pad with solder paste it might
suck the paste from under your chip. ...

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

solder mask, it might impact thermal contact with your iron, or maybe not.

The iron would seriously burn the solder mask.

 

[Joerg]

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

http://www.linear.com/product/LTC2242-12#packaging

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.

https://dl.dropboxusercontent.com/u/53724080/PCBs/T165_A3.jpg

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

 

[[email protected]]

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?

We use many DFNs and SOICs with pads.

 

[John Devereux]

Question to the folks here:

I use more and more parts that have a ground pads underneath which is
also for extracting heat. Usually I ask the layouter to provide a big
via in the middle so I can reach in with a Weller ETS tip to unsolder
from underneath. I also let the pattern stick out a bit past the ends of
the chips so I can unsolder/solder from the top without always needing
fancy heat guns.

Occasionally I had some groanings from producrtion folks that this is
non-standard (which is true) and that the part may slide. Never saw any
of that in a reflow process, but what do thee all say?

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.

 

[Nico Coesel]

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.

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

 

[[email protected]]

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.

Was it this one:

https://www.sparkfun.com/products/10706

Regards

Klaus

 

[Joerg]

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.

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?

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.

https://dl.dropboxusercontent.com/u/53724080/PCBs/T165_Vias.jpg

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

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.

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.

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.

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.

 

[Joerg]

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.

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.

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

 

[John Devereux]

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.

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

 

[Joerg]

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.

 

[josephkk]

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.

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.

?-)

 

[Joerg]

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.

 

[[email protected]]

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.

silk screen would work, but I've tried one pcb maker that removed
silkscreen
overlapping pads so be sure to tell them it is intentional

-Lasse

 

[Joerg]

silk screen would work, but I've tried one pcb maker that removed
silkscreen
overlapping pads so be sure to tell them it is intentional

Good point. I usually tell them not to alter anything in the Gerbers
without prior approval from me. Because once a manufacturer did that,
they "improved" a design. They had to eat the whole botched run and do a
rush run at no extra charge.

 

[rickman]

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?

The pins should help it center, but the large pad under the chip will do
pretty much nothing.

Give it a little thought. The centering works by surface tension. A
pin is typically not much different in size to the footprint. If
movement significantly changes the shape of the solder at the edges, it
will create a force from the imbalance of the two sides. But if you
extend the footprint pad far beyond the pin (or in this case the large
pad under the chip) the change in shape will be very small for a small
movement and there will be very little force generated.

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.

What John is saying makes sense. Use your large footprint pad, but add
solder mask to define the pad area under the chip, then leave openings
in the solder mask *outside* of the chip to lay your soldering irons.
This will give you the proper pad area under the chip which will make
the assembly house happy and give you areas to heat the thermal pad with
soldering irons.

 

[John Devereux]

The pins should help it center, but the large pad under the chip will
do pretty much nothing.

Give it a little thought. The centering works by surface tension. A
pin is typically not much different in size to the footprint. If
movement significantly changes the shape of the solder at the edges,
it will create a force from the imbalance of the two sides. But if
you extend the footprint pad far beyond the pin (or in this case the
large pad under the chip) the change in shape will be very small for a
small movement and there will be very little force generated.

All fine in theory, but I have seen "self centering" fail plenty of
times for no reason that is obvious to me.

[...]