4
\$\begingroup\$

Please look at this image(see the PCB traces within the circles).

image

This circuit belongs to a laptop adaptor.

  1. What are those parallel soldered-traces on the PCB traces?
  2. Why aren't they soldered to the soldered legs of the components?
\$\endgroup\$
  • \$\begingroup\$ Are they actually isolated from the trace they are on top of? It's difficult to tell from the picture, they look like they might be connected to me? \$\endgroup\$ – hekete May 25 at 13:57
12
\$\begingroup\$
  1. What are those parallel soldered-traces on the PCB traces?

They are traces where some of the soldermask has been removed in order to allow solder to build up to improve the current capacity of the trace.

The reason they left the narrow parallel lines of soldermask is so that the solder distributes itself more evenly across the width of the trace. Otherwise, it might bunch up on one side or the other. The rings around the component leads serve the same purpose — they prevent solder from wicking away from the joint.

The benefit of this is actually less than most people seem to think. The resistivity of solder is about 9× that of copper, so in order to halve the resistance (double the current capacity) of a trace, the solder needs to be 9× as thick as the copper underneath. For 1-oz. copper (35 µm), the solder would have to be uniformly built up to 0.3 mm or more.

  1. Why aren't they soldered to the soldered legs of the components?

They are in fact soldered to the legs. There is a circle of soldermask around each leg, but the copper still makes the connection underneath.

\$\endgroup\$
  • \$\begingroup\$ Isn't this solder layer just a cargo cult? Solder has much less electrical and thermal conductivity than copper and it hinders thermal relief to ambient. \$\endgroup\$ – Janka May 25 at 14:02
  • \$\begingroup\$ @Janka: Yes, already noted above. (I was editing while you were commenting.) \$\endgroup\$ – Dave Tweed May 25 at 14:04
9
\$\begingroup\$

What are those parallel soldered-traces on the PCB traces?

When you are designing a PCB with high current traces, you want to keep the trace resistance as low as possible. You can do this by multiple methods:

(a) Use a thicker copper layer eg 70 microns instead of 35 microns.

(b) Use bus bars to carry the current instead the PCB traces. These bars are copper metal that can be soldered on a PCB.

bus bars

(c) Use a wider trace - not possible in all cases due to space constraints.

(d) put additional solder on the traces which will reduce the resistance to certain extent. The benefit is 25 - 50 % reduction in resistance as per this video. Again, it will depend upon the copper thickness and lead thickness.

Why aren't they soldered to the soldered legs of the components?

If component pins are included, they will find it difficult to trim the additional pin length because it will become fat due to a lot of solder deposited on it.

They are electrically connected due to the copper trace. They coated most part of the trace with solder but chose to leave the pins. They also made some slots which is not being covered by solder. This is mostly to keep the additional solder deposit uniform and under a certain limit. If you have a larger area being soldered by wave soldering, it will tend to pick up a larger hanging mass of solder (due to surface tension).

\$\endgroup\$
5
\$\begingroup\$

In case of high power adapters, high current has to be supplied. Higher current requires either a wider copper trace and/or a thicker copper trace.

  1. Widening the trace
    Widening a trace reduces the trace resistance and allows a bigger area for the electrons to flow across without much resistance. While this method works in most of the cases, it fails when you have space constraints on the PCB. You cannot have wide traces on your PCB if you want a very small form factor of your finished product.

  2. Thickening the trace
    Thickening the copper trace will mean that the copper layer deposited on the PCB itself has to be thick. More copper = more price. This will increase the cost of the raw material which will ultimately increase the final PCB cost.
    But, we can surely deposit some other metal instead of copper! Solder is the cheapest and easiest of all options. Some parts of the traces are intentionally not covered with soldermask. These areas are later coated with solder during the soldering process. How much area has to be soldered is calculated during the PCB design stage.
    Dave Tweed♦ correctly pointed out the importance of a strip of solder mask between two exposed regions on the trace. This allows for even distribution of solder all over the exposed region. If the solder mask strip was absent, you would have seen a spherical blob of solder in the center of the exposed region. So, instead of a flat solder coat, you will get a coat which looks very much like a mosquito bite!

\$\endgroup\$
3
\$\begingroup\$

In addition to the other good info in answers;

Heavy parts soldered to large circular pads need more mechanical strain relief than electrical conductivity to avoid a microcrack annular ring , which is quite common due to shipping vibration and handling. The heavy track void lines also provide additional surface area for bulged solder to conduct some more current and heat for thermal convection rather than the thermal resistance of a plastic solder mask only, over copper.

Heat emission near to DC output is essential with a large surface metallic area as often the plug gets much hotter from contact resistance over time and heat flows into the board contacts.

Thermal pads with spoke lines allow for heat islands for faster solder flow in soldering and de-soldering.

This would have been wave- soldered and there are many (5) unpopulated locations with red glue dots for inverted soldering. Without the wave, there would be no excess solder, which cause bridging, so an omega vibration is often added to create a turbulence to the wave for higher yields and thicker solder spreading. Spray Fluxing with airation in a bubble stone assists that but whatever process used here was not quite optimized but worked.

Using twice the copper thickness would have been better but also twice the board cost.

Added

Note also the addition of self-adhesive rubber pads across the HV barrier also offer better creapage protection reducing the cost of routing an air gap.

\$\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.