# What is Circle on a circuit board

## Main Question or Discussion Point

I'm sure this is something so simple, but I've failed to find answer elsewhere, even doing several google searches "circle on circuit board", "diagram of circuit", etc....

What is the circle at the end of a wire\line on a circuit board? (the actual circuit board, not a diagram\drawing of one) What's it's function?

I could see where they might serve as connection points to some component, but I often see like at:

http://www.istockphoto.com/file_thu...4542965-microprocessor-and-circuit-board.jpg"

...in the upper left corner there is a short line with the circles at each end that don't seem to be leading to anything, what function might such an isolated wire serve?

Last edited by a moderator:

Related Electrical Engineering News on Phys.org
cepheid
Staff Emeritus
Gold Member
Welcome to PF gillwill!

It's possible that these circles are vias. Here is an explanation:

A printed circuit board (PCB) like the one in your image often has multiple internal layers (separated from each other by the non-conducting substrate material). These layers also have copper traces on them (just like the ones that you can see on the surface layer of the board). The purpose of having multiple layers is to expand your options when it comes to making all of the electrical connections required for your circuit. Sometimes the two outer surfaces don't provide enough area to make all of the connections. Getting the layout of the traces right is a tricky problem, when you think about it, because no two traces can intersect each other (unless they are *supposed* to be electrically connected). Therefore, sometimes what is done is to start a trace on one layer, and then continue it on an adjacent layer (so that it can pass "below" other traces/components that would have been in its way on the first layer). The vias are what make the connections between traces on different layers. A via is a metal-lined hole that passes through the entire board. The entire inner surface of this hole is lined, so that it can connect things between layers.

EDIT: I think you can also make vias that only connect to two specific layers, and not to any of the others.

Cepheid is correct. All the silver colored dots you see in the image are certainly vias.

While those appear to be vias on that board they aren't necessarily always vias. Sometimes you will see similar looking pads that are used for test points (bed of nails testers).

berkeman
Mentor
While those appear to be vias on that board they aren't necessarily always vias. Sometimes you will see similar looking pads that are used for test points (bed of nails testers).
Test pads won't have solder on them though.

Test pads won't have solder on them though.
Not entirely true - it depends on the location and the manufacturing processes involved in the board. Generally speaking, that is correct, but not always.

I thought that when I was first starting out in my career and was asked to reverse engineer a 4-layer board. It wasn't until after 30 minutes of trying to figure out where the 'via' with the solder on it went that I realized it was a test point.

Look like those are solder mask. Traces go to different layer by vias. I don't know why they put solder mask on the via and let solder flow through the via. In my boards, the vias are all now cover by solder mask and are all cover over by the top green layer. never have solder flow through it.

Our PCB designer says that if vias are filled with solder, higher current can go through via.
We did this on some higher current PCB's.

When I layout pcb trace that carry high current, I use double or even tripple vias as insurance. Contact is only as good as the via to trace, whether you fill the via with solder make absolutely no difference.

I agree that double or triple vias are frequently used for higher currents.
It would be interesting to make some tests to determine if filling a via with solder increases its current carrying capacity.
Strictly from a theory point of view, it would seem that since vias are drilled hole that have a thin plating of copper, adding a filling of solder would increase their current carrying capacity.

I agree that double or triple vias are frequently used for higher currents.
It would be interesting to make some tests to determine if filling a via with solder increases its current carrying capacity.
Strictly from a theory point of view, it would seem that since vias are drilled hole that have a thin plating of copper, adding a filling of solder would increase their current carrying capacity.
Depend on the size of the via, the connecting via has the width of the circumference of the via which is usually wide enough. Problem is the contact between trace and the via, instead of the space inside the vias. A lot of people just too lazy to specify a bigger via and just use the default via in the layout. I define different type of vias in the pad stack so when I need a bigger via, I call out the bigger one. And I still use multiple vias for high current trace. It is all about the layout. That is the reason I do most of the layout myself. AND YES, I even even layout some of my engineer's pcb even as the manager. Layout is everything, I did a lot of signal integrity stuff before, layout is everything.

I know I am off the subject, but this is just so so important and I so wish professors in college will spend more time on pcb layout with signal integrity and good pcb layout pratice.

Last edited:
When two Gurus say different things it's interesting to try and determine who is correct.
There were two identical obsolete PCB's on hand.
The boards were designed for mounting through hole components.
The boards were two sided, FR4, 1/16", plated through holes, 1 oz copper.
Trace was 0.02" wide, Pad was: 0.038" Hole, 0.075 Width, 0.075 Height.
The via had one trace connected to it on top of the PCB and one connection on the bottom of the PCB.
The approach was to fill the via in one PCB with solder and nothing in the other via, then raise the current through the vias until via failed.
The test results were that something started to smell hot at 15 amp RMS 60 Hertz after 1 minute.
Then trace on the board that had the via filled with solder started turning black at 17.5 amp. The trace on the board without the solder in the via started turning brown at same current.
Conclusion: Still don't know who is correct, but the via handled much more current than expected.

When two Gurus say different things it's interesting to try and determine who is correct.
There were two identical obsolete PCB's on hand.
The boards were designed for mounting through hole components.
The boards were two sided, FR4, 1/16", plated through holes, 1 oz copper.
Trace was 0.02" wide, Pad was: 0.038" Hole, 0.075 Width, 0.075 Height.
The via had one trace connected to it on top of the PCB and one connection on the bottom of the PCB.
The approach was to fill the via in one PCB with solder and nothing in the other via, then raise the current through the vias until via failed.
The test results were that something started to smell hot at 15 amp RMS 60 Hertz after 1 minute.
Then trace on the board that had the via filled with solder started turning black at 17.5 amp. The trace on the board without the solder in the via started turning brown at same current.
Conclusion: Still don't know who is correct, but the via handled much more current than expected.
You really did the experiment for this thread?!!?

Sounds like they don't make too much difference. I think two via is safer just simply because if there is any defect with the bonding of the via to the trace of one also.

berkeman
Mentor
This has turned out to be a pretty interesting question and discussion. I'll try to ping our assembly house tomorrow to ask if they know why there seems to be solder paste on non-tented vias. As I've read through the thread (especially since the assembly seems to be a low-power SMT PCB), I'm starting to wonder what the reasoning was...

cepheid
Staff Emeritus
Gold Member
Strictly from a theory point of view, it would seem that since vias are drilled hole that have a thin plating of copper, adding a filling of solder would increase their current carrying capacity.
For what it's worth, this would be my intuition as well. It seems like the resistance of the connection point would be lowered by having a larger cross-section of conductor present.

This has turned out to be a pretty interesting question and discussion. I'll try to ping our assembly house tomorrow to ask if they know why there seems to be solder paste on non-tented vias. As I've read through the thread (especially since the assembly seems to be a low-power SMT PCB), I'm starting to wonder what the reasoning was...
I've dealt with this in a recently episode where the layout artist forgot to select the correct options in his layout package. Apparently some layout packages allow this option. Something you might want for a high current bus. In older technology, as I've been told, the solder mask artwork was generated by taking a defocused (high contrast) photo of the pads photo. The end result is a solder mask with a few mil clearance around the plated through holes. This consequently included the vias.

I use OrCad, last revision I used was 9.2. We defined the solder mask in the pad stack of the via. I usually not define solder mask for them and result was no solder flow through the via. I think who ever did that pcb have the solder mask defined for the via so they are not covered by the greed material. You can see the circles are quite big also. I don't think the board was done with high current in mind because most of them are digital signal traces.

berkeman
Mentor
Interesting topic.

I found this: http://www.emtworldwide.com/article.aspx?ArticleID=15052

I couldn't agree more with yungman about the importance of layout. It is simply not taught in schools and yet is a critical factor in getting all but the simplest circuits to work.
Good link, and that makes a lot of sense that you would fill vias that you also want to use as test points. On PCBs where there isn't room for separate vias and test pads, when you combine them, they will usually be filled with solder to give a better contact with the ICT pogo pins. Interesting.