Hi all. I would like to know which of the following is the best way to route between pad and track where the track passing through the pad to some other component. I wish to know which one is the best practice and the reason behind it. Thank you in advanced 
I use A just because I think it looks better. But, technically both are correct as long as you donât use 90 degree corners. I will tell you that the trace going between D95 and D100 is too close to D100. It should in the middle. It also looks like the traces are too thin.
A is better. When tracks join pads or other tracks at acute angles, they can form an acid trap, which could result in the trace getting etched away.
/mike
Thanks for the well explained repliesâŚ
Another add-on question here. What if I add teardrops to them?
Still A is the better option or both are at the acceptable quality?
Tears drops are nice for high voltage/amperage traces. âAâ is the preferred routing method. Like n1ist stated, if you are etching your own boards, it might make for a difficult time because of the tight corners you are creating. With âA,â you are eliminating angles under 90 degrees.
You still need to be aware of the thin traces you have. You have plenty of room to widen them. You also need to check with your PCB house to find out their design rules.
This may be slightly askew of topic, but I had an electrical engineering friend of mine suggest that I shouldnât run a signal âthroughâ a pad (as shown in both A and B above), but rather branch off a bypassing trace to the pad. Can anyone suggest the pros-cons to that?
If youâre running power traces around signal traces, you might get interference on the signal lines. If the GND pour is adequate in the area, then you should be fine.
B can actually be better however the traces should not form acid traps, D95 & D91 do as there are little bits of less than 90 degrees.
D100 has balanced entry exit points on the left pad however it would be better if the track exiting and going to the right was raised to the same extent as the one on D99.
Historically we would enter a pad as per D95A but these days there is no reason not to enter via the corner of a pad, there is no detriment to it.
Ditto about fattening the tracks - Iâd double them at least.
Thanks for all the discussions. I knew that the trace is too thin for this case. I just wish to know the best practice for routing between pad and trace. Perhaps we should focus on certain application such as signal trace, high power traces and high frequency traces. We had option A and B at the beginning but seems like we have option C - Should not run a signal trace through a pad which is stated by Rohar.
Hi, this is an interesting discussion 
Iâm also often very unsure as to trace width ? can anyone give some pointer as to how to determine what width is optimal ?
i know that some fab house has limits to minimum width and space between , but as a rule of thumb of some sorts.
normally i use eagle standard widt of 10mil, and ground pour , around power thingies i go to 16mil just cause i âbeliveâ it to be better but this is just guessing, would be nice if anyone have a sort of âhow to do it rightâ pointer
Width is generally decided by the current that the signal carries, Saturn PCB Designâs PCB toolkit is a free program that will calculate the track width for you given conditions entered and this uses current standards, not outdated 50 year old tables. I suggest you look it up.
For a minimum width I would consider about 8 thou an average, yes you can thin it down but if you do not need to then dont. The same goes for the track to track/pad gap - the bigger you can make it the better. Generally the fatter the track the lower the impedance to signal travel.
When you start to get your tracks down to thin widths you risk higher failure rate in manufacture among many other electrical issues.
Although thin widths and close spacing can be and are made often, this comes with higher board costs, higher likelihood of crosstalk etc so its best not done unless necessary.
As for running tracks through pads, there are IPC standards that say the opposite is god and through pads is bad - however IMO these are way outdated and no longer good practice.
ISTR reading that having lots of little spurred off connections is bad for EMC but running through the pad does not.
On the other hand I have read that running through a PTH pad can if the pad is lifted, break the entire connection and the whole net causing failures. There are arguments on both sides as to whether that is good or bad (it depends on the circuit).
PCB layout practice is a difficult subject to talk about because there are so many that have differing views because some make small runs, some make hundreds of thousands, some do low speed, some do high speed, some pass EMC, some dont. So many different circuits, methods, techniques rules, regulations, standards to meet etc.
For everything I have said there will be at least 2 people that disagree completely - and probably (hopefully) 2 more that agree.
hneve:
Hi, this is an interesting discussionIâm also often very unsure as to trace width ? can anyone give some pointer as to how to determine what width is optimal ?
i know that some fab house has limits to minimum width and space between , but as a rule of thumb of some sorts.
normally i use eagle standard widt of 10mil, and ground pour , around power thingies i go to 16mil just cause i âbeliveâ it to be better but this is just guessing, would be nice if anyone have a sort of âhow to do it rightâ pointer
I use http://www.4pcb.com/trace-width-calculator.html a lot. It really depends on the design load and what temperature rise/resistance you are OK with. With a 1 oz trace, you can use 10 mil for anything under 500mA if you are OK with a 25° rise in temp. Play with temperature rise, ambient temp and trace length until you get a feel for it.
You also want to take trace impedance into account; I wouldnât use a long thin trace for power to a chip even if the current draw was lowâŚ
/mike
Rohar:
This may be slightly askew of topic, but I had an electrical engineering friend of mine suggest that I shouldnât run a signal âthroughâ a pad (as shown in both A and B above), but rather branch off a bypassing trace to the pad. Can anyone suggest the pros-cons to that?
Depending on the situation, you WANT to run signals through the pad. For example, if you have a bypass cap filtering power, the power trace should go THROUGH the pad as opposed to connected to the net by way of a trace. This comes from an EMC guru who has helped a lot with our designs.
One of this favorite quotes is, âThe answer to every questions is: It depends.â So is the case here. It all depends on your intentions behind placing the component and trace.