4

For a certain TI component, I'm choosing between these two packages, both of which are 24-pad and 0.5mm pitch:

  1. QFN: http://www.ti.com/lit/ml/mpqf167b/mpqf167b.pdf (4 x 4 mm)
  2. BGA: http://www.ti.com/lit/ml/mpbg520/mpbg520.pdf (3 x 3 mm)

Some considerations:

  • BGA is cheaper for a PCBA house to assemble, correct?
  • If I use 3 mil microvias (on a 6-8 layer board) to route out BGA components, how many rows/cols does a 0.5mm BGA have to be before the routing gets annoying?

Any advice appreciated!

AlcubierreDrive
  • 1,484
  • 2
  • 18
  • 26
  • 1
    AFAIK, there's no significant cost benefit to using BGAs over QFN's. I think the tradeoff is that the BGA is roughly 1/2 the area; whereas the QFN can definitely be routed without microvias. If you don't already need microvias for some other part in your design, adding them to support this part might increase your blank board cost by 50%. – The Photon Sep 10 '12 at 01:02
  • 1
    On the other hand, are you sure you need microvias to route the BGA? The first two rows should be routeable without vias under 4/4 design rules. And the center ball has an escape at location b2, so you should be able to route that with a through via. – The Photon Sep 10 '12 at 01:05
  • Already need microvias. – AlcubierreDrive Sep 10 '12 at 01:05
  • Do you know what the surrounding component-free margin would be for the QFN vs the BGA? I would guess 2mm for QFN and 0.5mm for BGA? – AlcubierreDrive Sep 10 '12 at 01:08
  • Also if you put your comments in an answer, I'll gladly accept it. Thanks for the info! – AlcubierreDrive Sep 10 '12 at 01:09
  • you should wait a day or two. Give everybody in all time zones around the world a chance to answer...You might get somebody to give you more details about this particular situation. – The Photon Sep 10 '12 at 01:16
  • 1
    on the clearances to the neighbor components, usually the limitation for these types of parts is to allow for rework without removing other parts. I doubt if there's any reason for different clearance between BGAs and QFNs since both need a hot air system for rework. ... but again, you might get a different answer if other regulars here get a chance to respond. – The Photon Sep 10 '12 at 01:18
  • Ok thanks for the clearance/rework info, and I'll wait before accepting the answer. – AlcubierreDrive Sep 10 '12 at 01:25
  • @ThePhoton What are the 4/4 design rules? Couldn't find it on the web. – Nick Alexeev Sep 10 '12 at 01:45
  • 2
    4 mil minimum copper feature size, 4 mil minimum separation between copper features. Nowadays a pretty common design rule that won't add much to your costs. – The Photon Sep 10 '12 at 01:48
  • It's 2020, and most interesting chips don't even exist in any other packaging but BGA (typically with 0.4 mm pitch). – Brian Cannard Oct 22 '20 at 21:57

2 Answers2

5

AFAIK, there's no significant cost benefit to using BGAs over QFN's. I think the tradeoff is that the BGA is roughly 1/2 the area; whereas the QFN can definitely be routed without microvias. If you don't already need microvias for some other part in your design, adding them to support this part might increase your blank board cost by 50%.

On the other hand, are you sure you need microvias to route the BGA? The first two rows should be routeable without vias under 4/4 design rules. And the center ball has an escape at location b2, so you should be able to route that with a through via.

bga mechanical drawing

The Photon
  • 126,425
  • 3
  • 159
  • 304
5

Why do you think the BGA is cheaper in assembly? The operation is the same for both: pick and place. But the BGA needs X-ray for inspection, and the assembly shop may charge extra for that. The QFN can be visually inspected.

The QFN also lets you reach the pins with a probe. For a scope probe no problem, but for a DMM you'll need needle probes.

If you can afford the extra couple of square mm the QFN needs I would go for that. After all you can still use via-in-pad to save space.

stevenvh
  • 145,145
  • 21
  • 455
  • 667
  • Thanks! For other readers, here are guidelines for via-in-pad: http://i.screamingcircuits.com/docs/Via_In_Pad_Guidelines.pdf Basically you should never have an unfilled via in a pad. Best practice is to plug the via and then plate copper over it. – AlcubierreDrive Sep 11 '12 at 21:31