16
\$\begingroup\$

I am a hobbyist and I find it very difficult to solder and work with SMD components which have very small underneath pads. I can't see when the solder flows, I can't touch the pads with the multimeter, and therefore I have no confidence in the board.

I want to make extra long pads so I can touch / see the connections and be more confident.

Will extra long pads as below cause problems for me?

(Normal pads left, extra long pads on right). Extra Long Pafs

Photo of the 9mm wide module I will be soldering onto my board for reference (I will also be using a ST LPS22HB pressure sensor which has much smaller pads).

Module pads example

Thanks, I know this is a bit stupid but I have had a couple failures on this design and have to wait weeks for new revisions, so best to ask. I use solder paste applied by syringe and either a hot plate or a heat gun.

Update a few months later: The extra long pads saved me so many times, was able to see and fix many failed solder joints which I had no way of knowing were failing in the past.

\$\endgroup\$
1
  • 1
    \$\begingroup\$ Ideally, the solder should cover the whole pad. This is a bit of an utopia though and it's far from always the case no matter if reflow or manual soldering. Grounded pads in particular tend to wet worse than others. The recommendation is to follow the recommendations :) That is, the pad layout proposed in the datasheet. \$\endgroup\$
    – Lundin
    Commented Mar 25, 2022 at 14:52

5 Answers 5

18
\$\begingroup\$

No, In fact there are different suggested footprints for hand soldering and for stencil applied paste soldering. https://forum.kicad.info/t/why-different-pcbnew-footprints-for-hand-soldering-smd-603-resistors/3857

\$\endgroup\$
2
  • \$\begingroup\$ Thanks for the confirmation I'm going to go for it! Just haven't seen excessively long pads anywhere before and thought it may flow to other pads too easily or cause other problems. I use solder paste + syringe and a hot plat or reflow gun + measure temperature. \$\endgroup\$
    – exile97
    Commented Mar 25, 2022 at 0:51
  • \$\begingroup\$ Excess of solder is the main reason why solder flows to an adjacent pad, not the size of the pad itself. Enlarging the pads helps the soldering job, even with an iron. \$\endgroup\$
    – mguima
    Commented Mar 25, 2022 at 3:12
18
\$\begingroup\$

Short answer: in your case, there should be no problems.

Longer answer: If you need impedance matching (high speed signals) the size/form of pads can have an influence on the signal quality. But as long as you're not in the field of RF (radio frequency) stuff or interconnects in the gigabit per second range, you probably don't have to care about that with pads. For I2C, CAN (where impedance matching becomes important but still, pads are not an issue), I2S, SPI and stuff: no issue.

Components must self center in reflow

If the pads are not the correct size and form, SMD components do not self center anymore. But that's only an issue if you want to do reflow solder

Tombstoning

Small components (ceramic capacitors, resistors) have a tendency to "stand up" on one of the pads which can be influenced by the shape of the pad. Also, not a big issue with hand soldering because you need to push down on the component while soldering anyway.

Access to Signals

Don't rely on pads to access the signals. Start using testpoints (put them in the schematic already). It will benefit you greatly in the future if you get used to having test points for every signal on your board - nicely labeled and documented.

Indicators

Use LEDs as indicators on your board. Put indicator LEDs on every power rail. Put them on I/O lines (make sure that you don't exceed the load limitations of your components). Put them on TX/RX of your serial connections. Those LEDs don't have to be bright. Choose the resistor value so they just glow (way below 1mA per LED). It will make your life SO much easier when debugging stuff if you see an LED go out if a power rail is shorted. It's so nice to see if data is being transferred on RX/TX lines if you have communication issues. If you have an MCU also put a status LED on a GPIO line which you can blink with different patterns depending on what part of your software is running - it's a great help for debugging.

\$\endgroup\$
6
\$\begingroup\$

Such pads are exactly what's needed for manual assembly with a soldering iron. That's why KiCad has a "handsolder" variants for most surface mount footprints.

Oversize pads cause problems in reflow soldering when using pin-less packages without side wall metallization. A resistor or a capacitor has metallization on the side walls, but various leadless chip carrier (LCC) packages don't. In those cases, as the solder melts and the package is pulled down by the surface tension, the excess solder is pushed out and forms inter-pin shorts, often of a whisker nature, as well as solder balls.

The general idea is: for hand soldering use "handsolder" footprints in KiCad, or equivalents in other EDA software. You can and should create your own footprints as necessary. For reflow - whether in manual prototyping or production - use IPC-compliant pad sizes for machine assembly. Those are the non-handsolder footprints in KiCad.

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

you can use longer pads but it is not very useful. The best way for touching pads is adding test point. Thanks to test points you can touch easily where you want. Here is example;

enter image description here

enter image description here

\$\endgroup\$
1
\$\begingroup\$

Great answers. The only thing I didn't see mentioned:

You may ask yourself, isn't a trace just.. a really long pad? What differentiates a trace from a pad?

Other than width, the biggest thing is solder mask. Traces have it, pads don't. It's there for a reason: if there were no mask at all, yes: it would be very easy to solder everything, but it would be very easy to solder everything to everything else; bridges would abound. I've tried hand-soldering on a mechanically milled PCB with no mask and it's a living nightmare. So, everything in moderation: lengthen your pads, but don't expose so much non-masked copper that you run into trouble with solder bridges.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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