# Is it better to route a pad to a trace, or a trace through a pad?

When routing a PCB, is it better to route a trace through a pad as in 1 below, or to route a pad to a trace as shown in 2 below?

Electrically, there is no differences.

Well, in fact there are some... But only when considering very high frequency signals.

If the passive element is a decoupling capacitor, your solution 1 will looks like this:

simulate this circuit – Schematic created using CircuitLab

L1 and L2 represent the little inductors made by the routing tracks themselves. You can see that the capacitor is connected directly between L1 and L2, without (or more precisely "negligible") inductance. The decoupling will be good. (even better if L2 is very small by putting your decoupling caps very close to the load).

But using routing option 2:

simulate this circuit

The little extra routing track forms an added inductor (L3) between the decoupling caps and the load. Thus your decoupling would be worse rejecting very high frequencies.

It worth nothing to mention that there is also an unwanted inductor at the GND connection of decoupling caps. This should be as small as possible too.

There is another reason: Reflow soldering.

Your component has to be "thematically balanced". I mean that your footprint has to look symmetrical. Thus it will heat-up evenly during reflow soldering and your component will not rotate or just move due to surface tensions into the liquid solder. Imagine that the solder paste get liquid on one pad when it is still solid on the other, because of thermal imbalance on the footprint: The component may move and end up soldered at one pad only. (see picture)

If both pads were routed using your option 1, this is not symmetrical in the X nor in the Y direction. But if both pads were routed using your option 2, this would have been perfectly symmetrical and this is good. In that point of view, everything that is symmetrical (in X and Y) is good. (there are other thing to consider but I will deliberately omit them here, because it would be out of scope)

I would finish by saying that these things are becoming critical only when considering mass production and relatively high quantities. Reaching thermal balance on your footprints may reduce by some percent the number of badly soldered components.

• Will assembly houses tell you if they have this kind of problem with your boards? I haven't been careful about it, but the boards seen to come out fine. – Jeanne Pindar May 23 '14 at 12:45
• If you have a good relationship with them and plan to do big volumes, yes. At some point you may ask them to review your routing and they may come up with improvement suggestions based on their knowledge of their assembly process. In fact, I have learned a lot during theses kind of meetings. Thing such as, hot air masking of big components that impair soldering of very small that are nearby. The time lost by the rotation of the pick and place head when your passive elements are randomly rotated and do not use preferred orientations. etc. – Blup1980 May 23 '14 at 13:32

In the rather obscure field of designing zener barrier circuits (for intrinsically safe equipment), option 1 would be the preferred solution because if a zener diode became disconnected by a PCB track break, then the output of the "barrier" would naturally be disconnected from the potentially dangerous input voltage i.e. it is fail safe: -

simulate this circuit – Schematic created using CircuitLab

• Could one reliably do a four-point connection to the zener? I would think that the most likely cause of failure would be a bad solder joint. – supercat May 23 '14 at 2:27

If you need to split a trace to two different locations, do it from the pad. I prefer option one, with one modification. Make each trace meet the the pad right on the corner. Personally, I like the nice smooth 135 degree pad to trace angle, but more importantly, having 45 degree angles between copper features is asking for etchant traps. Meaning that in the etching process, acid gets caught in the acute angle, and continues etching unpredictably. The boards will test fine in the manufacturing process, but there will be random failures in the field. The way to prevent it is keep all angles greater than or equal to 90 degrees. PCB manufacturers have better control over this than they once did, but for high reliability and long service life products, it's a chance not worth taking.

To add my E 0.01: For a prototype I prefer (for all other things the same) the 2nd option, because it makes it easier to cut the trace to the component and make some other connection to it. But when space is tight I will switch to the 1st version, although I would prefer to avoid that sharp angle.

• Seconding that! For cuts/jumps on protos, and if you do the same during board-level debug on old equipment, it's better to have the component pads separate from the circuit nodes. Yes, with Rs and Cs you can easily lift one end of a part, but for anything with 3+ leads, it's less damaging to slice a trace than to try to desolder/lift just one pin. Similar issue: don't route traces onto pads underneath ICs, instead bring traces out from underneath before connecting to a pad. – wbeaty May 23 '14 at 5:56

I think that's quite personal (I prefer the second solution) but there are some objective differences. Option two might be better because soldering on that pad is somewhat easier since the thermal resistance to a bigger thermostat is double the first solution resistance. If you are soldering by hand that might make a big difference. Moreover excess solder can be swept easily away in solution 2, while in solution 1 that's somewhat more difficult. That's particularly true for SOIC or similar SMD chips, if your trace comes out at an angle it might be very, very difficult to solder them by hand.
I bet there are other issues, I'm sure somebody around here can add a lot, that's just my two cents. Anyway, as I said, I find option two a whole lot neater than one.

• Having traces come off at angles does not make components harder to solder, unless your traces are huge, in which case it makes no difference how you attach them. I don't get what you're saying about excess solder being swept away either. – Matt Young May 22 '14 at 12:40
• that only applies when you hand solder. if there's too much solder it's easier to take it away if there's a copper trace that it can follow. – Vladimir Cravero May 22 '14 at 12:57
• So you're talking about a board with no soldermask? – Matt Young May 22 '14 at 12:59
• I am talking about the kind of board an hobbyist can etch with sone HCl and H2O2, that's the boards I've access to... – Vladimir Cravero May 22 '14 at 13:01

Simple, if its a POWER trace like VCC of GND you should defenetly go for 2, if its some signal its your choice.

• "if its a POWER trace like VCC of GND you should defenetly go for 2." Why? – Nate May 22 '14 at 14:00
• Power trace works like the main supply pipe, it cannot be interrupted, if that resistor on the picture above breaks or burns, in case 2 the rest of the circuit can still function. – Electropepper May 22 '14 at 15:03
• I duno who put a minus, but i have more then 10 years experience i know what im talking about, you have my opinion, its up to you to use it or not. – Electropepper May 22 '14 at 16:04
• It wasn't me, but my guess is that it's because your answer is so short and without explanation. Answers on here are generally encouraged to be thorough and not one-liners. – Nate May 22 '14 at 16:30
• True, i will try to be more explicit. – Electropepper May 22 '14 at 17:19