8
\$\begingroup\$

As far as I understand, through holes in PCBs are often plated, hence the term PTH. Letting red denote copper, the first figure shows a through hole which is plated, and the second figure shows one that is not. The thick black line is the pin of a component, while the silver denotes solder applied. I can't figure out why the copper plating (otherwise known as the barrel) is needed - can someone explain why?

With through plating:

With through plating

Without through plating (why isn't this the norm?):

Without through plating

\$\endgroup\$
  • 6
    \$\begingroup\$ The key issue is that, WITH plated holes the PCB can be expected to function as designed and can be tested "bare". ie it is an engineering component in its own right independent of other components or manufcturing steps. || With links or component leads for connections the integrity of the connections relies on the soldering of components and links. As others have said, both sides of a component may not be accessible or the component may not be "leaded" - or both. An excellent example of the latter is the BGA package. Look it up if you don't know it !!! \$\endgroup\$ – Russell McMahon May 6 '16 at 12:21
  • \$\begingroup\$ There aint nobody under here but us balls and pads \$\endgroup\$ – Russell McMahon May 6 '16 at 12:22
  • 8
    \$\begingroup\$ If you make a board without plated through holes and with pads on both sides, not only will you have to solder both sides, but you may find it harder to do so, as trapped heated gas in the bore of the hole surrounding the pin may interfere with the solder fillet. In a plated through hole, the solder wets the plating and the hole ends up filled with metal. \$\endgroup\$ – Chris Stratton May 6 '16 at 13:30
25
\$\begingroup\$

In order for your scheme to connect the top and bottom layer, TWO conditions must BOTH be met:

  1. The pad on the TOP must be accessible and must be soldered (separately).
  2. The pad on the BOTTOM must be accessible and must be soldered (separately).

In very many cases the top pad of a thru-hole component is NOT accessible because the body of the component covers it. So that is not practical.

In MOST cases there IS NO component lead at all where you need to via from one side to the other. Inserting short bits of wire and soldering BOTH SIDES is simply not practical even for manual assembly not to mention automated assembly as virtual all modern gear comes from.

It doubles the effort to require soldering to BOTH sides of even a thru=hole component lead. That takes double the assembly time, and greatly increases the chances of assembly error. It is simply not reasonable at any level.

\$\endgroup\$
  • \$\begingroup\$ Hi Richard - I'm trying to understand your second point "In MOST cases there IS NO component lead at all where you need to via from one side to the other." Are you saying the component lead is not long enough to reach from one side to the other? Thanks for other points - they make sense. \$\endgroup\$ – Tosh May 6 '16 at 6:43
  • 1
    \$\begingroup\$ Also, I found this image imgur.com/G7Ygv8F in Khandpur's 2006 book. This resistor appears to be soldered from both sides, right? So I assume this is not one of those "MOST cases" you mentioned - am I correct on this? \$\endgroup\$ – Tosh May 6 '16 at 6:45
  • 2
    \$\begingroup\$ @Tosh: He's saying that it is more common to find a via where there is no component lead (and therefore no "easy" way to connect the two sides) than where there is one. \$\endgroup\$ – Ignacio Vazquez-Abrams May 6 '16 at 6:49
  • \$\begingroup\$ @IgnacioVazquez-Abrams If there is no component lead...wouldn't that be a surface mount device then? So then there wouldn't be a hole in the board in the first place? \$\endgroup\$ – Tosh May 6 '16 at 6:55
  • 7
    \$\begingroup\$ @Tosh, you are dramatically underestimating the necessity for VIAs. A VIA is a place on the PC board where you must connect from one layer to the other, but there IS NO component there at all. So you need a plated-thru hole to make the connection. This is critically necessary for boards with more than two layers. \$\endgroup\$ – Richard Crowley May 6 '16 at 7:02
13
\$\begingroup\$

Your first image is not completely accurate. The solder should also be sticking to the plating in the hole, and not just connecting to the top and bottom layers of metal. That is to say, plating offers improved mechanical stability and increased joint strength due to the much larger surface area available for soldering.

\$\endgroup\$
  • 4
    \$\begingroup\$ Also, not plating holes does not save any processing steps in most designs, because there are still vias -- but a design without non-plated holes can possibly skip a drilling step. \$\endgroup\$ – Simon Richter May 6 '16 at 5:32
  • \$\begingroup\$ @SimonRichter - not sure I understand your point about saving the drilling step; the hole must be there so there is no getting away with drilling, right? \$\endgroup\$ – Tosh May 6 '16 at 6:46
  • \$\begingroup\$ Ignacio - I found an image that illustrates your point: imgur.com/G7Ygv8F about the solder sticking all the way through. But I don't see how plating makes the connection stronger - the solder would stick to the substrate as well, wouldn't it? So sticking to the substrate should increase mechanical durability the same amount, wouldn't you say? \$\endgroup\$ – Tosh May 6 '16 at 6:48
  • 1
    \$\begingroup\$ @Tosh: No. Solder-metal bonds are much stronger than solder-non-metal bonds, assuming you can even bond them in the first place and don't end up with something like the second picture in the question. \$\endgroup\$ – Ignacio Vazquez-Abrams May 6 '16 at 6:52
  • 2
    \$\begingroup\$ @Tosh, you have one drilling step before plating, and one after plating. The former can be omitted only if there are neither plated thru-holes nor vias, the latter if there are no non-plated holes, which is more likely. \$\endgroup\$ – Simon Richter May 6 '16 at 7:45
11
\$\begingroup\$

If you have plated-through holes, tracks on both sides of the board (and any internal layers) are connected without any further action.

Holes exclusively for this purpose are called "vias" and may be smaller than regular holes for component leads.

This makes manufacturing any board too complex to be single-sided, easier and usually much cheaper than otherwise possible, since no extra effort such as inserting jumper wires or soldering on both sides is required.

It also makes design and layout of double-sided boards much easier since you no longer have to strain to minimise the number of tracks on the "other" layer, or minimise the number of jumpers, or ensure crossings between layers aren't underneath components.

And that allows you to increase the board density and use smaller boards, cheaper enclosures, etc...

It also allows the PCB manufacturer to perform "bare board testing" of every one of these interconnections before any components are added - thus eliminating many defects. (Some PCB makers perform bare-board testing free of charge).

Plated holes give you all this before even considering how you actually solder a component to the PCB - though it offers advantages there too...

\$\endgroup\$
  • 1
    \$\begingroup\$ Plated through-holes are nice even when hand soldering otherwise-single-sided boards. If solder is applied to a pad without a plated hole, it will tend to form a "donut" around the hole; if a pin in the middle of the whole is supposed to be connected, one must finagle the solder to make it bridge between the pin and the pad. When applying solder to a pad with a plated through-hole, the solder's natural tendency will be to try to pull itself through the hole, thus much more easily grabbing any pin that might be there. \$\endgroup\$ – supercat May 7 '16 at 16:08
8
\$\begingroup\$

Most circuit boards are soldered by machines. Solder wave in the case of through-hole boards. The solder wave is a ripple in the surface of molten solder that the board is dragged through using a conveyor. It passes over all the pads and trimmed leads on the bottom of the board. It does not solder the top of the board. Soldering leads on the top would not only require them to be accessible but would require hand labor to solder each one. This would not be cost-effective in the case of production quantities- any tiny saving in the boards would be dwarfed by the hand labor required, not to mention the cost of a design constraint that requires all the leads to be accessible on the top (think of connectors, electrolytic capacitors, IC sockets etc.)- that means bigger boards, bigger housings, more packaging, more shipping costs, more shelf space etc.

So the standard for 2-layer boards is plated-through holes, and at some small additional cost you can have unplated holes as you mention. It's an additional operation so it costs more- the holes have to be drilled after the plating operation. Probably most boards have some unplated holes as well- they tend to be better for things like pressed in pins because the dimensions are more controlled.

There is nothing stopping you from ordering boards with unplated holes everywhere if you enjoy the extra soldering (though they may think you made a mistake and 'correct' it for you if there are connected pads on either side of a hole) but you won't save any money.

\$\endgroup\$
  • \$\begingroup\$ Spehro, thank you for your answer. You mentioned that wave soldering only solders the bottom but not the top, so this made me think: what about SMT devices that need to be soldered to the top? Wikipedia says "[SMT] components are glued onto the surface of a printed circuit board (PCB) by placement equipment, before being run through the molten solder wave." Does this mean the SMT device is somehow soldered to the top by the solder wave, perhaps on a second pass? Link: en.wikipedia.org/wiki/Wave_soldering \$\endgroup\$ – Tosh May 20 '16 at 8:49
  • 1
    \$\begingroup\$ SMT boards are generally printed with solder paste and then the parts are set down on the sticky solder paste and reflow soldered (using IR or other heating the board is heated to a couple hundred degrees C briefly). \$\endgroup\$ – Spehro Pefhany May 20 '16 at 11:58
  • 1
    \$\begingroup\$ It's possible to glue parts down and wave solder them .. That method is sometimes used in mixed through-hole and SMT boards (with SMT parts on the 'bottom' side), but it's hard to solder really fine pitch devices without shorts. Glue is sometimes used when reflow soldering boards with parts on both sides but it's not always necessary. \$\endgroup\$ – Spehro Pefhany May 20 '16 at 12:03
2
\$\begingroup\$

Most mpdern electronics has some measure of SMD (surface mounted) components, the leads of SMD parts lay flat and don't go through the board. Plated through holes are a handy way of linking top to bottom. That way, the top and bottom layers come connected from the factory so you dpn't have to connect them yourself. They also make a good low thermal resistance path when you want to use the board as a heatsink (plain old FR4 makes a terrible heatsink). Where PTHs are real useful is when you have more than two layers and you need to connect them or when you have parts with really small pads that need to be connected to another layer, pads far to small or too numerous to connect them manually (OSH park will happily make you a 4 layer PCB with 0.25mm holes with 0.45mm pads, and that's at hobbyist prices, cutting edge IT stuff can have 10-20 layers and holes less that 0.1mm wide that only go part way through a PCB). You don't have to use PTHs but the technology os at a stage where it adds only a few percent to the overall cost of a professionally made board.

\$\endgroup\$
0
\$\begingroup\$

I have made, for the sole purpose of saving money, two sided board without PTH (as the second figure of your question). The board was very simple, but testing was painful! - Testing net connectivity on the board was impossible without soldering first all the components - Bad soldering of the components (the mounting was by hand) meant electrical connectivity lost, so I have to re-check all the joints several times

After that experience with a two layer but no vias PCB, I opted for paying a little bit more but having faster testing times.

So, the point is: you can go without VIAS, but if you are talking about any real, practical project, you will be sorry of not having them.

\$\endgroup\$
0
\$\begingroup\$

Richard answered the question well, but WHY a plated-through hole only needs to be soldered from one side hasn't been properly explained in this thread. The surface tension of the solder wicks it along the barrel and component lead all the way through the hole, providing a connection that is both electrically and mechanically solid. If the hole isn't plated through, the circuit board material is resistive enough to solder that it won't wick through and reach the other side, so both sides need to have solder directly applied.

Structural instability issues can arise in the highly likely chance that air is trapped between the two solder layers on a non-plated-through board.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.