I am having a problem with inductor desoldering. (Bourns 2310-V-RC) I found a lot of desoldering failure after time.

The inductor is used as an LC filter. Maximum 8 Amps.

This is the PCB view

enter image description here

Are the pads of my design too small? Do you think I did some mistake?

If you need more details please just ask me

enter image description here enter image description here

  • 3
    \$\begingroup\$ can you elaborate on what "desoldering failure" means? How well do the solder joints of the inductor look when it's not failed? \$\endgroup\$ Jul 20, 2020 at 8:23
  • 2
    \$\begingroup\$ that was what I'm assuming: you did very well when designing the pads as heat sinks. So well, in fact, that your soldering process couldn't solder the pins correctly, because the solder got instantly cold when it came into contact with your copper planes. What was the method you used to solder this? \$\endgroup\$ Jul 20, 2020 at 8:45
  • 1
    \$\begingroup\$ that's how the solder joints look coming out of Eurocircuit's assembly? \$\endgroup\$ Jul 20, 2020 at 9:19
  • 1
    \$\begingroup\$ Next board spin, use 'thermal reliefs' on those pad. Every PCB layout software will offer them. \$\endgroup\$
    – Kyle B
    Jul 20, 2020 at 10:36
  • 1
    \$\begingroup\$ For now, the trick is to get the copper planes hot enough w/o damage to the inductor. I would scrape a little of the solder mask away, expose more copper around the pads. This will give an opportunity for greater heat flow from the soldering tip. Use a short fat tip and set the temp about 100 degrees higher than you normally would. Put a blob of solder on the tip, and use that to touch the copper w/o touching the inductor. Let it heat for about 10 seconds. Only then you feed in more solder. Should be able to make a good solder connection then. \$\endgroup\$
    – Kyle B
    Jul 20, 2020 at 10:39

2 Answers 2


That's a horrible attempt at soldering, and if you paid a company to do that you really should take it back to them and tell them to redo it properly. I can't believe that anyone who knows how to solder looked at that and thought it was OK.

The problem you're seeing is that the solder applied to the pins of the inductor has barely flowed onto the PCB and has not flowed at all into the through-holes like it should.

This is caused by those large copper planes absorbing a lot of the heat from the soldering iron, and, as a result, the area around the through-holes is not getting hot enough for the solder to flow properly.

To do this properly will require a fairly powerful soldering iron and possibly pre-heating the whole board, too (or at least the area around the inductor).

I suggest you contact Eurocircuits' QA dept, send them those pics, and ask them how on earth they found that to be acceptable...

  • \$\begingroup\$ Thank you for the advice. Do you suggest to use thermal reliefs or not? I found contrastant information on that \$\endgroup\$
    – Daniele
    Jul 20, 2020 at 12:18
  • 3
    \$\begingroup\$ Well - that ultimately depends on your requirements... Thermal reliefs will certainly make those pins much easier to solder, but will also (very slightly) increase the resistance of the connection. IMO a professional company should be able to solder those without reliefs (as long as they recognize the need for additional effort there), but I very much doubt that adding reliefs there will affect the operation of your circuit. I would probably add the reliefs. \$\endgroup\$
    – brhans
    Jul 20, 2020 at 12:24
  • 1
    \$\begingroup\$ You could probably get a little more mechanical stability by increasing the size of the pad around the hole, especially on the bottom. This particular part is heavy and tall, and will put more than typical torque on the two little wires holding it onto the board. \$\endgroup\$ Jul 20, 2020 at 17:49
  • \$\begingroup\$ @Daniele With such a large lead and so much space you shouldn't need thermal relief since you can just get a big fat iron tip in there. If I put in my 6.6mm tip I could solder that just like anything else without special effort. Heck, it'd be even easier than other joints since everything is so big and easy to see and manipulate. And that's even if I was using lead-free solder. There's just so much space to work with. \$\endgroup\$
    – DKNguyen
    Jul 20, 2020 at 23:48

I would certainly go for a bigger pad both to make it easier to get the heat in there and make a larger solder joint that can hopefully take the stress better. I'd say a pad size about 3x the hole size is preferable.

Sometimes space constraints mean you can't use pads that large but i'd certainly go for them where possible.

Thermal reliefs are a double edged sword, on the one hand they can make it easier to get a joint up to temperature, on the other hand they increase electrical and thermal resistance in use


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.