I was reviewing a design earlier, and I noticed something interesting. The designer had removed unused pads on the chip. I have never seen this done before.
Is this something that is good practice? Is it even okay?
\$\begingroup\$
\$\endgroup\$
2
-
\$\begingroup\$ No mention of the silkscreen underneath the component? That's a good way to lift your legs off of the pads on one side of the component. (Edit: Accidentaly commented on duskwuff's answer, not the question) \$\endgroup\$– Jason_L_BensCommented Apr 15, 2017 at 0:52
-
\$\begingroup\$ I think somebody didn't know what to do with the NC pins! Regarding silkscreen, I think this is an overblown concern for TQFP and SOIC type chips where there is usually some clearance gap between the body and the board. Note there is no thermal pad here so package is not intended to sit on the PCB. In my experience, this is never a problem except for leadless packages like QFN where the pad sits flush with the package. \$\endgroup\$– Joel WigtonCommented Apr 21, 2017 at 19:20
Add a comment
|
4 Answers
\$\begingroup\$
\$\endgroup\$
6
This is not a standard practice, and should be avoided.
First: Along with providing electrical connectivity, pins also mechanically anchor a chip to the board. Each pad that's removed increases the stress on the remaining pins, which will increase the risk of the chip detaching from the board.
Second: All of the remaining pins have nothing but soldermask between them and a trace underneath them which they aren't supposed to be connected to. Soldermask is not very thick, and it's not very durable either. If the mask is breached -- from a pin vibrating against it, for instance! -- the pin may become intermittently connected to something it wasn't supposed to be.
-
\$\begingroup\$ Very good point with the breach of soldermask! I hadn't thought of that! \$\endgroup\$– ReidCommented Apr 14, 2017 at 19:34
-
14\$\begingroup\$ Solder mask is just designed to be a mask during soldering. It is not designed for, and should not be used as, an insulator for your pcb design. Ever. \$\endgroup\$ Commented Apr 14, 2017 at 20:41
-
\$\begingroup\$ I would argue that some pins may be inputs, others may be NC, so there are possible cases when breaching solder mask is not a problem. \$\endgroup\$– user76844Commented Apr 15, 2017 at 3:59
-
2\$\begingroup\$ @GregoryKornblum If there's no problem with having some of the pins touching, though, then why not put real pads there? \$\endgroup\$– user39382Commented Apr 15, 2017 at 4:23
-
2\$\begingroup\$ If the mask is breached -- from a pin vibrating against it, for instance! -- the pin may become intermittently connected - I've seen some boards where a simple work around for that was applied: the unused pins were additionally.. cut off. But that were some very old boards, obviously soldered manually and only large packages were used back then so cutting the pins was easy:) \$\endgroup\$ Commented Apr 15, 2017 at 11:21
\$\begingroup\$
\$\endgroup\$
0
No, it's not good practice, but if done really carefully it can open more space for routing on the top layer. This is only useful if that makes the difference in being able to drop layers and make the board cheaper. This in turn means it only makes sense for high volume products where the price of the board actually matters in the overall product, and where it is significant relative to the engineering investment.
Otherwise, there are reasons not to do this:
- Pads are for physical mounting too, not just for making electrical connections. This matters more for some packages than others. For a 64 pin TQFP like this, removing half the pads shouldn't reduce mechanical strength to where it matters for most cases.
- Unless you are careful to remove the pads reasonably symmetrically all around the chip, the surface tension of solder can pull the chip off center during reflow. This is a serious issue you have to think about carefully. You may also have to change the pad shapes for the remaining pads so that the center of the pull is where the chip is supposed to be.
- You have to be really sure that the unused pins done touch anything conductive. The solder mask should take care of this, but stuff happens. If there is a lot of vibration or thermal cycling, are you sure the unused pins won't eventually rub thru the solder mask?
answered Apr 14, 2017 at 19:35
\$\begingroup\$
\$\endgroup\$
It would ease the layout at the expense of making the assembly more fragile. It's probably not okay according to the IPC (using solder mask as an insulator)-- see for example this thread- but I don't have specific chapter and verse to cite. Further, the soldered leads will have a relatively large gap bridged with solder because the other leads are sitting on top of solder mask, which makes the assembly even weaker.
So I think this is amateur hour stuff but it probably works okay enough and might be acceptable for a throw-away consumer product. Definitely not acceptable for a high-reliability design.
answered Apr 14, 2017 at 19:35
\$\begingroup\$
\$\endgroup\$
6
He clearly needed that for routing. Probably otherwise he would drill holes, make more layers... As long as number of removed pads is low and it's safe to assume that the component will not fall, it's a brilliant idea for saving costs.
-
-
4\$\begingroup\$ Rule of thumb: each two layers add 30% to PCB cost. And of course vias cost too, although much less. \$\endgroup\$– user76844Commented Apr 14, 2017 at 19:30
-
1\$\begingroup\$ Yeah I did that on a design. There were stubborn tracks that I couldn't route... And NC pins... \$\endgroup\$– bobfluxCommented Apr 14, 2017 at 19:30
-
\$\begingroup\$ Sometimes i connect NC on BGA to other nets to route them to deeper rows. \$\endgroup\$– user76844Commented Apr 14, 2017 at 19:32
-
2\$\begingroup\$ @duskwuff On a QWERTY keyboard, B is directly to the left of N, and V is directly to the left of B, so yeah, probably a typo caused by somehow misaligning the first and the last out of the three keypresses on the bottom row of the keyboard. How he managed to correctly hit M is anyone's guess. Mobile phone perhaps? \$\endgroup\$ Commented Apr 14, 2017 at 21:55