Author Topic: How to create perfect footprint  (Read 196 times)

0 Members and 1 Guest are viewing this topic.

Offline robertferanec

  • Regular Contributor
  • *
  • Posts: 70
How to create perfect footprint
« on: January 14, 2020, 04:15:35 pm »
What pad dimensions should I use and why? Where my pin 1 should be located? What if I do not follow standards? What is IPC about? And more ...

I really hope this video will be useful for many engineers. Please, leave comments to let me know what do you think. - Robert

« Last Edit: January 14, 2020, 04:21:36 pm by robertferanec »

Offline free_electron

  • Super Contributor
  • ***
  • Posts: 7262
  • Country: us
    • SiliconValleyGarage
Re: How to create perfect footprint
« Reply #1 on: January 14, 2020, 04:52:49 pm »
it all depends.

The starting point is : talk to your fabricator and assembler. Find out what they can and cannot do
- soldermask registration accuracy
- minimum soldermask opening over pad
- minimum soldermask sliver
- what silkscreen printing technology ( jets can print finer than optical or silkscreen )

That will determine what you can do in terms of soldermask

SMT pads : rounded rectangle. it is proven it gives better paste release in the stencils

Paste mask openings : don't bother. Set paste mask 1:1 to pad. The stencil thickness and the flux/solder is an unknown, so the amount of contraction / expansion to get the right amount of solder is an unknown. This is up to the assembler to calculate and manipulate. Some manufacturers want home-plate (pentagonal) structures for small parts to avoid tombstoning.

Pad geometry , size and pitch : follow IPC guidelines BUT don't be afraid to override !. IPC is only a guideline NOT a standard !

Even more : IPC is often in conflict with itself.

Example : according to IPC land pattern guide there needs to be a toe to edge of pad gap of a minimum width. The toe needs to sit inside the edge of the pad.
According to IPC assembly defect guide it is ok for the pin toe to stick out beyond the pad ...  So the toe needs to be inside the pad when making the footprint , but when you actually build it it is ok if it sticks out ...

Naming conventions : IPC is severely lagging behind all the new packages coming out and has no name structure for many new parts. Other elements are not handled. For example : TQFP144 pin packages , same pitch, same body size but with a different thermal pad size... how do you name those ? -crickets-

Manufacturers are also often contradictory with themselves. VSSOP , TSSOP , MSOP .. don't trust those names ! They mean NOTHING. Example : TI has a package document where anything pitch 0.65 is TSSOP and 0.5 and below is VSSOP. And then they have a VSSOP8 package with 0.65 mm pitch ... They call it that in the datasheet .. 'oh , that must be a mistake ...'

For me there are only 4 types of packages :  2 with gull wing pins and 2 without pins ( pads)
SON : small outline no leads
SOP : small outline pins
QFN : quad flat no leads
QFP : quad flat pins

note : there is no such thing as a DFN10 or DFN14 package. DFN is Diode Flat No-lead. So it's 2 , 3 or 4 pins max. Just like SOT23 is 3 pins. and sot 143 is 4 pins and SOT25 is 5 pins and SOT26 is 6 pins. There is no such thing as SOT23-5

Other problems are manufacturers being incompatible with themselves. An NXP SOT23 is not necessarily the same as an infineon one. There are slight differences in body size, pin size/shape and tolerances. Why ? Licencing fees! NOt every mfr has their own packaging facility. Many use Amkor anam or other foundries. Each foundry has their own 'secret sauce'.

Even worse : inside the same manufacturer there is misery. Diodes inc is a prime example. They are an amalgam of so many absorbed companies , each having their own molds. So they have at least 5 different SOT23 flavors. A couple of years one of their fabs burnt down and certain molds were lost ... All of sudden : yield problems on too tightly defined footprints.
When making a footprint : grab the geometry from 4 or 5 different manufacturers and overlay them.

Other misery : SOT89 NXP numbers these clockwise, the rest of the world counterclockwise ... Pay attention when making footprints ! The same was is for some thru-hole parts in TO92 like BS170 BS250 mosfets and BC817 darlingtons. Depending on the manufacturer the pin assignment changes !

And when dealing with japanese manufacturers like toshiba ,sanken , jrc et all : all bets are off. Those packages have often nothing in common with what we are used to from western manufacturers. Do you really believe an SC-70 is equivalent to a SOT23 ? Prepare for yield issues if you didn't design it properly ...

As for courtyards : pay attention to part height. The taller the part the more risk of 'shadowing' when wave soldering. so you need a larger area around the part. especially true for 0805 1206 and larger parts. These come in various thicknesses. Have footprints in thickness ranges !
The same is true for through hole parts. The pick and place machines need room to grab the part. Don't place those big electrolytics too close. The gripper on a 4700uf 63V is larger than the gripper for a tiny 10uf 6v3 !

Centroids : put those in the gravitational center of the part , or the pick point. many datasheets show you the optimum picking point for parts. Saves time when programming the machines.
« Last Edit: January 14, 2020, 04:57:11 pm by free_electron »
Professional Electron Wrangler.
Any comments, or points of view expressed, are my own and not endorsed , induced or compensated by my employer(s).
The following users thanked this post: robertferanec, Cubdriver

Offline robertferanec

  • Regular Contributor
  • *
  • Posts: 70
Re: How to create perfect footprint
« Reply #2 on: January 14, 2020, 05:04:47 pm »
@free_electron - a great summary  :-+

Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo