Why are there teardrops on PCB pads?

Question

What's the use of the teardrop shapes around some PCB pads?

enter image description here

Good question. I've never used them, and I see that teardrops are sometimes optional in EDA suites. — stevenvh, Apr 18 '11 at 15:44
@Dean - added a picture (I think you need a minimum rep to do so) — stevenvh, Apr 18 '11 at 16:00
Going to guess to improve connectivity between track and pad. — Dean, Apr 18 '11 at 16:00

score 53 · Accepted Answer · edited Apr 18 '11 at 17:22

53

There are primarily two reasons to use teardrops:

It avoids a pocket (where the trace meets the pad) that could collect acid from the PCB etching process which would later do bad things.
It reduces mechanical & thermal stress resulting in less hairline cracks in the trace.

That being said, in professionally made PCB's teardrops are rarely needed. It's almost more of an aesthetic thing than a solution to a real problem. I've done many boards with and without teardrops and I have yet to notice a difference. In my opinion, they are more trouble than they are worth.

edited Apr 18 '11 at 17:22

Daniel Grillo

7,659
18
51
69

answered Apr 18 '11 at 16:43

4

I see how they could be little use; but how are they trouble? (as in "more trouble than they are worth.") – Javier Apr 18 '11 at 20:06
2

@Javier It really depends on how your CAD software handles them. What you don't want is to have to draw the teardrops manually for every pad/via. Years ago I used Protel that would make good looking teardrops, but had some bugs that caused problems in the gerber output when teardrops were used. Now I use Cadence Allegro, which has lots of issues. At the very least, the teardrops simply take longer to draw and makes editing the PCB more cumbersome (assuming that you have a super complex PCB to begin with). – Apr 18 '11 at 20:20
I've seen a number of PCBs with broken pads that cracked at the point where the teardrop touches the trace. – endolith Apr 26 '11 at 14:41
16

It's worth noting that teardrop-pads *are* necessary in some specialist situations, namely *flex-pcb*. Teardrops on flex-pcb layouts serve to reduce the stress bottleneck where the trace joins the pad. – Connor Wolf Jul 07 '11 at 23:12
also there could be issues with electromigration. Electromigration is the transport of material caused by the gradual movement of the ions in a conductor due to the momentum transfer between conducting electrons and diffusing metal atoms. – Jeff Wurz Dec 11 '15 at 09:51

Daniel Grillo · Answer 2 · 2021-01-20T03:37:57.253

19

The teardrop is to help the drilling process. It prevents drill breakout where the trace joins the via or through-hole. Sometimes it's not necessary to do it because the manufacturer can do it for you.

Where I work, our repair department recommends we do it because it increases the strengthening of connections between pads and tracks.

edited Jan 20 '21 at 03:37

answered Apr 18 '11 at 17:22

Daniel Grillo

7,659
18
51
69

It might help the drilling process, but I've seen plenty of them on SMT pads. – Apr 18 '11 at 17:25
We have never had any issues that I know of with pads getting pulled up when drilling after etching. – Kellenjb Apr 18 '11 at 17:30
@Kellenjb: it's not that the pads pull up, it's that the drill can be misaligned by a larger distance and still not create an open-circuit by drilling through the narrow track. – Martin Thompson May 11 '12 at 10:24

score 16 · Answer 3 · edited Apr 13 '17 at 12:32

16

If you look at the picture the Ben Jackson posted in answer to a question about solder mask expansion, you'll see that the drilled holes can be significantly off-center from the pad centers.

In extreme cases, you could actually end up with holes that leaves no or very little annulus to make the connection to outgoing traces. The tear drop ensures that there's enough pad material left over to have a solid connection to the pad.

edited Apr 13 '17 at 12:32

Community

1

answered Apr 19 '11 at 00:39

Toybuilder

2,018
1
11
12

2

I understand that the hole isn't always dead in the center, but if it's so far off that it goes off the pad I think I would go and find another manufacturer. – stevenvh Apr 19 '11 at 06:13
It might be a cost-quality tradeoff. Perhaps the main goal is to slap a product together cheaply - they might be willing to go with a lower-precision fab, and design the board to accomodate that choice. It might also be that there is only a small handful of parts that need extra densely placed PTH's that doesn't justify paying for higher precision fab for the other 99% of the board. The teardrop might be the "compromise" solution for those cases. – Toybuilder Apr 19 '11 at 17:31
@stevenvh, most fabs I've used give a minimum annular ring spec that allows for something like 20% breakout of the hole (which they derive from their copper and hole registration capabilities). If you really want to never have a hole go off the pad, you just need to use a larger pad size than they gave you as the minimum. – The Photon Jan 10 '14 at 17:41
1

Drilled holes might be a little off-center, but not necessarily in the direction of the teardrops. Teardrops are oriented to the direction of the track and this may be different for each pad. But if there is a misalignment between drill holes and pads, the direction of misalignment may be the same for all or most pads. If you want to be sure to get a minimum annulus in every case, you just have to use larger pads. – Uwe Dec 15 '16 at 09:39
A fast-turn manufacturer I use says the only way to safety use an 18mil ring with an 8mil hole, to avoid breakout, is to use teardrops. In this situation they are a real benefit on tight boards. – BenYL Jun 28 '19 at 15:10
The purpose of the annulus is to connect the via barrel to the trace with imprecision in the drill center. There is both offset for all holes in a given board as well as wander, variation from hole to hole. IPC specs allow some portion of the via barrel to 'break out" from the pad. This "allowed" amount can be enough to cut the trace from the annulus when in the right position (not allowed). Tear drops prevent this for smaller annulus. They also mitigate "acid trapping" which may no longer be a problem. I've never seen evidence this is a design problem and not a quality control issue. – gnuarm Dec 25 '20 at 18:11

score 15 · Answer 4 · edited Apr 18 '11 at 16:29

15

They are mainly used on single-sided boards, to increase reliability. I often use them on my home-made PCBs.

edited Apr 18 '11 at 16:29

stevenvh

145,145
21
455
667

answered Apr 18 '11 at 16:05

Leon Heller

38,774
2
60
96

3

Is that because it's single-sided, or (with all respect) because it's non-professional (DIY)? In other words, are they also useful if you have your PCBs produced in a shop? – stevenvh Apr 18 '11 at 16:11
3

It's mainly because single-sided boards don't have PTH. – Leon Heller Apr 18 '11 at 16:37
2

that was going to be my answer... The bit about it not having plated through holes which results in the pad being able to be pulled up a lot easier or move around with shock resulting in breaks over time. – Kellenjb Apr 18 '11 at 17:13
2

In my dictionary PTH = Pin Through Hole, but I guess you mean Plated Through Hole. :-) – stevenvh Apr 18 '11 at 17:30

score 3 · Answer 5 · answered May 11 '12 at 16:18

The simple answer is for Strain Relief.

Like a plug with a thin cable, it needs a graduated support to prevent the shear forces of thermal expansion when desoldering a component or when a human interface force is involved ( eg mic jack or a heavy part on a board.)

Where you do not have strain or any thermal or mechanical stress in the application, it is unnecessary. But I have seen dozens of times when this would have prevented a track failure that was hard to see with the naked eye. One example was a $2K Mac vertical monitor with the flyback transformer on the main board... It created a micro-sheer crack impossible to see, but whenever the CRT went blank a slap to the side of the case fixed it. Which lasted for a few days, until the secretary cried.... help.. so I came to the rescue with a soldering iron. and said to myself... I wish the board designer knew about tear drop pads.

If it's for strain relief can't you simply use a larger pad? A lot easier and more effective, as it goes all the way round the pin. — Federico Russo, May 11 '12 at 16:35
Absolutely not. It is the track that needs to be enlarged , or rather the track pad interface... When you put teardrops into the standard library for interface devices its not hard. It is not needed for every via. — Tony Stewart EE75, May 11 '12 at 16:42

score 1 · Answer 6 · answered May 01 '15 at 20:33

I thought it had to do with IPS-6012C for rigid board. Specifically related to section 3.4.2 Annular Ring Breakout. For example, Class 2 allow for an annular ring to break out (be missing) for 90 degrees. This is due to drill misalignment. On large vias or plated through holes, this is not likely to happen in modern fab facilities. When dealing with 10 mil finished drill holes and 20 mil pads this is much more probable. If the breakout happens on the side of the trace exiting the pad, Class 2 states that it can cut the trace down to 50um and still be acceptable. If there was a teardrop (or fillet), the misdrill would not cut into the trace.

score 0 · Answer 7 · edited May 29 '16 at 18:27

A teardrop via make it easy to remove embedded resistors when using ECL logic. This was done by Harris Computer Systems about 1987 to make it easier to repair memory PCA's that cost upwards of $15,000 (or more) in their h1000 and h1200 systems. To remove the embedded resistor that was connected to the via all one needed was a pin vice and then drill a hole at the point of the teardrop. Then add a wire to a spare embedded resistor or add an external resistor. I remember building the light box to see the teardrop via.

Why are there teardrops on PCB pads?

7 Answers7

Linked