How do i determine footprint sizes for surface mount components?

[DaveHardy]

Hi,

I've got a board that I'm trying to reverse engineer.  I don't have a problem with the through hole components or the board layout.  However, I have never designed a surface mount board before and don't quite understand how to pull standardized component layouts from the stock libraries.  Maybe I should make my own custom pad layouts?  Stated differently, what I'm trying to do is measure the surface mount components with a ruler and determine what parts to order and what size to make the pads.  I have attached a picture of my project next to a ruler.  For these big 1w 1 ohm resistors, what size are they and how can I search for them at Mouser?  Are the small caps in there 1 X 2 MM?  How big should I make the pads?  Are there any general rules I should abide by and traps for newbies?

-Dave 

[ataradov]

Component sizes have standard dimensions in inches. They are marked as two numbers next to each other with only decimal part of the size.

For example, component with package type 0805 will have dimensions 0.008" x 0x005". 

You can measure your components and do a reverse calculations to figure out their package type. There is a handful of standard dimensions, so you don't really need to be accurate with your measurements.

[DaveHardy]

Thanks for the reply.  I was in the process of answering my own question when you posted.  I have determined that the big 1w 1 ohm resistors are 6mm x 3mm = 2512 = 250 mil x 120 mil.  Should I just use the standard pad library?  The pads are 3.2mm x 1.8mm They are spaced apart 5.6 mm.  Am I doing this right?

[ataradov]

Should I just use the standard pad library?

I see no reason not to use the standard library. As always, double check that library has correct dimensions.

[IconicPCB]

Comrade Stalin said it best "... kantrol is gud.. trust is betr..." this was of course restated by president Ronald Raygun when he succinctly agreed "... trust but verify...".
Yes.. ensure the library content is appropriate. Keep in mind soldering process will have influence on footprint aspect ratio.
Reflow versus wave soldering versus manual soldering.
Talk to the assembly engineers.

[CatalinaWOW]

Pros may have another take, I only do this as a sideline.  Passive components have a fairly small number of footprints.  There is a bewildering variety (to me at least) of packages for active components, switches, relays, connectors and the like.  Regardless, for each component there is a formal definition of pad spacings.  Some are so similar that they can almost be interchanged.  Others will look the same at a quick glance, but will laugh in your face when you try to actually put parts on them. 

The manufacturer of the part may even have recommendations on pad sizes and shapes.   But as stated by others, the people doing the soldering will have their own processes which impacts pad sizes and minimum spacings.  There will also be variations in the courtyard or keepout area which defines how closely components may be placed.

The bottom line, even if you find a footprint in the library that seems to fit your needs, you must carefully check footprint dimensions to assure they will work.  Particularly if you want to make quite a few and have high yield.

[tautech]

Thanks for the reply.  I was in the process of answering my own question when you posted.  I have determined that the big 1w 1 ohm resistors are 6mm x 3mm = 2512 = 250 mil x 120 mil.  Should I just use the standard pad library?  The pads are 3.2mm x 1.8mm They are spaced apart 5.6 mm.  Am I doing this right?

You don't say which PCB package you're using.
Altium for example has 3 standard footprints for each standard passive; low density (largest) medium density and high density (smallest).
Should you want to hand populate and solder the PCB, the low density footprint with the slightly longer pads is much easier to obtain a nice solder fillet with and gives one a bit bigger pad to probe to if faultfinding or checking/developing prototypes. IIRC there's a slightly different spacing between pads too which enables traces to be routed underneath passives on the larger packages. (0805+)

[KL27x]

Buy a pair of $12.00 digital calipers from Harbor Freight or Amazon, or the like.

Those big resistors are probably 2412's. With a pair of calipers you'd be able to verify that in seconds.

As for pads, a lot of people just make their own. I get fed up looking for pads and almost always make my own library parts. Usually, the data sheet for the part will show the recommended pad layout. This may be easier to do than to look up footprints or to screw around with calipers.

[Erickben]

Thats what I wanna say.

Component sizes have standard dimensions in inches. They are marked as two numbers next to each other with only decimal part of the size.

For example, component with package type 0805 will have dimensions 0.008" x 0x005". 

You can measure your components and do a reverse calculations to figure out their package type. There is a handful of standard dimensions, so you don't really need to be accurate with your measurements.

[batteksystem]

Thanks for the reply.  I was in the process of answering my own question when you posted.  I have determined that the big 1w 1 ohm resistors are 6mm x 3mm = 2512 = 250 mil x 120 mil.  Should I just use the standard pad library?  The pads are 3.2mm x 1.8mm They are spaced apart 5.6 mm.  Am I doing this right?

You don't say which PCB package you're using.
Altium for example has 3 standard footprints for each standard passive; low density (largest) medium density and high density (smallest).
Should you want to hand populate and solder the PCB, the low density footprint with the slightly longer pads is much easier to obtain a nice solder fillet with and gives one a bit bigger pad to probe to if faultfinding or checking/developing prototypes. IIRC there's a slightly different spacing between pads too which enables traces to be routed underneath passives on the larger packages. (0805+)

I always like the medium density one, it is not too big but allow you to put the solder head next to the chip while resting on the pad heating both part to get a good joint. However, if you go for pick and place, all the default one would be okay.

[tautech]

Thats what I wanna say.

Component sizes have standard dimensions in inches. They are marked as two numbers next to each other with only decimal part of the size.

For example, component with package type 0805 will have dimensions 0.008" x 0x005". 

You can measure your components and do a reverse calculations to figure out their package type. There is a handful of standard dimensions, so you don't really need to be accurate with your measurements.

And you would've been wrong like ataradov was.

package type 0805 will have dimensions 0.008" x 0x005" 0.080" x 0.050"

Metric is also used, just not so often. eg 2012 = 0805

[ataradov]

And you would've been wrong like ataradov was.

Typo, obviously. You may also argue that "0x005" is not a valid number, unless you are a programmer

[T3sl4co1l]

Rules?  Absolutely!
http://pcbget.ru/Files/Standarts/IPC_7351.pdf
The easiest to remember:
Toe: solder fillet in the lengthwise direction. Add >= 0.3mm to max component dimension.
Heel: * * * * under-component direction.  Subtract >= 0.3mm to min component dimension.  (Usually you have to subtract max lead length 'L' from min overall width 'B', but if this is missing, min. body width 'A' can be used.)
Side: -0.03 to +0.03 of max. lead width and positional tolerance.

There are a couple basic types of solder joints:
- Flat or curved leads, laying on pads: gull-wing (SO, QFP) and J-lead (SOJ, PLCC) for example.  These have all three types of fillets.
- Solid, leadless, or metallized ends: SON/DFN/QFN periphery contacts, chip (R/L/C) ends, flat-lead diodes, SOT tabs, etc.  These have toe fillets, and have >= 0.3mm side fillets if the metal protrudes from the body (diodes and SOTs).

If there's no side fillet (or it's not desirable to make one), the side clearance should be about equal to the the average or maximum dimension (the +/- 0.03mm case).

Most chip R's and D's don't have side metallization, so no side fillet is possible there anyway; the pad should be made equal size for these.  Most chip L's and C's are metallized all around, but side fillet is undesirable as it increases strain on the part, and can lead to tombstoning (for small parts, sometimes 0603s, usually smaller) and more risk of fracture.

QFN lands are covered by plastic on three sides, so they only get added toe length.

Likewise, chip R's, C's, etc. don't have a heel fillet, so that added dimension is near zero.

- Flat-face lands.  PQFNs, LGAs, BGAs, exposed thermal pads.  There is no toe, heel or side, just a periphery, which, as you might now be expecting... as it's flat with the surface, the pad size is +/- 0.03mm of nominal.

BGAs are kind of a special case, because the ball allows the pad to be somewhat larger or smaller.  Which one you choose also depends on choice of SMD/NSMD (solder mask defined, or non-) pads.  NSMD is generally preferred (i.e., solder mask expansion is outside the pad, so the full pad copper is soldered).

Tim

[tszaboo]

Recommended land patterns are also shared in datasheets. Not always for resistors, well because they are so general. I also recommend reading and using as a reference IPC-7351.

[T3sl4co1l]

Use caution: datasheets are manufacturer specific, and honestly, may not fit their own parts very well, let alone anyone else's similar parts.

I don't think I've ever seen a datasheet specify what it's optimized for.  Low or high density, high manufacturing yield, IPC guidelines, etc.

For example, TO-220 (not -AB) is a terribly unspecific drawing.  Have you ever seen one with round wire leads?  I have.  Thick tabs?  Usually.  Thin tabs?  New LM7805s and etc. are usually made with thin tabs (because, really, you can only dissipate so many watts in a 7805 anyway).  Some people are surprised that "TO-220" can allow such thin tabs, but it's been there since the beginning.  TO-220 is a JEDEC standard from, I don't even know...the '60s?

The familiar proportions, with a usefully thick tab, and usually with the semicircle cutouts in the body as well (I forget if it's on the drawing), are TO-220AB, actually.  (If it matters, be specific!)

That doesn't usually affect mounting (aside from a few threads worth of screw length, and the hole size), but many JEDEC SMTs are just as dubious, like the DO-214 series (commonly called SMA/B/C).

Recently cleaned up an SMA footprint in a DFM (design for manufacturing) review.  It was straight out of the (in this case, ST) datasheet, probably minimal size, to the part they manufacture.  The footprint DOES NOT FIT THE PART DRAWING THEY GIVE, because it can't.  Their part, presumably, has tighter tolerances than the JEDEC DO-214AC specification, but they can't call it "DO-214AC" if it doesn't match the same tolerances.  So they give you a shitty, loose drawing, an overly tight footprint, and let you figure it out.  Will that affect yield?  Rework?  Thermal or mechanical performance?  Who knows.  (Rework probably, as undersized pads are bad for hand soldering.  But if you use hot air anyway, who cares.)

It's always safer to use oversized pads, except when it can cause tombstoning on small parts.

Tim