I am attempting to make a board for the tlc5951 24-channel led driver to drive an 8x8 rgb led array. I have made what I think is a good eagle library for the sop-38 package, but I am not sure what to do about the pad on the underside of the ic. The datasheet has thermal characteristics with and without the pad soldered, but I suspect I will want the heat dissipation provided by the pad. This is my most ambitious soldering project yet, and I have a few questions I would like to straighten out before I have the first round of boards made.

Should I hook the heatsink to my ground polygon on the bottom side, or leave it disconnected? I'm not sure if it will cause problems with grounding if it heats up too much.

Is my only option to reflow this, or is there a way to do it by hand? I have never done any reflow soldering, and I am much more comfortable hand soldering. I am definitely not comfortable having a stencil made to do this kind of thing. Is there any kind of thermal compound or something that can make a thermal connection comparable to a solder joint, or is solder best?

The datasheet has very specific dimensions for pad size, via patterns, and stencil opening. Should my solder mask pretty much follow the stencil opening outline on the datasheet?


3 Answers 3


What I do for prototype boards that I'm soldering by hand is to put a large hole in the pad and feed solder into it with the soldering iron. 2 mm works well.

Solder the other pins first, so that the chip is fixed in position.

The flux in the solder will be sufficient.

Number of holes depends on the size of the pad. One is usually sufficient.

You need a good soldering iron with plenty of heat, I use a Metcal.

  • \$\begingroup\$ Would I do that before or after I solder the other pins? Do I flux in there first? Should I make multiple holes, or is one sufficient? \$\endgroup\$
    – captncraig
    Jan 19, 2012 at 6:06
  • \$\begingroup\$ The hole must be metal-coated, right? \$\endgroup\$
    – avakar
    Jan 19, 2012 at 12:43
  • \$\begingroup\$ ... I mean, I tried to do this recently on a hand-made board (way faster and cheaper than professional proto boards), and as such I didn't have coated holes. And I simply couldn't get the pad heated. I eventually had to use hot air... \$\endgroup\$
    – avakar
    Jan 19, 2012 at 12:47
  • 1
    \$\begingroup\$ It only works with PTH boards. \$\endgroup\$ Jan 19, 2012 at 14:22
  • 1
    \$\begingroup\$ Oh, plated is the word, not coated :) \$\endgroup\$
    – avakar
    Jan 19, 2012 at 14:27

To get the most dissipation from the pad it needs to be connected to a decent amount of copper.

This is usually the ground plane, so place vias (no thermal reliefs) from the pad (or surrounding area - see document linked to below) to the plane.
As Leon mentions, putting one large hole in the center of the pad can make it possible to solder it by hand from the other side of the board.

This TI document on power pad goes into some detail about how to do things. Another document here also.


I know this thread is old, but I hope my answer can help others with this question.

I work as a PCB layout engineer, and have designed many circuit boards with exposed bottom die pads. For production-level boards, using a grid of small vias (8-10 mil drill) works best to prevent the solder from wicking through the PCB, but in most cases, adding a large central hole is fine, provided the solder paste stencil has some clearance from this hole. In all cases, multiple vias are far better than a single one to reduce thermal resistance. Remember, the vias and solder are the only connection between the IC and the PCB which is acting as a heatsink. Very little heat by comparison can be dissipated through the leads, especially on ICs that were designed with a bottom die.

In most of my designs, I use a large central hole, but my method of hand soldering is different than the previous answers above, but has proven very effective over the years. The problem I've encountered with feeding solder through the central hole last from the backside of the PCB, is that unless the hole is very large, there is no way to verify that it has in fact wetted to the die, and the percentage of the die which is soldered is similarly impossible to determine. To eliminate this guesswork, I solder it first. Here's how:

  1. Apply solder to the thermal pad on the backside of the PCB, filling the central hole.
  2. Apply solder to the thermal pad on the component side of PCB, until there is enough to form a very low dome shape on the pad.
  3. Place PCB in a clamp in a flat, horizontal orientation. Make sure it's raised off the work surface enough to access the backside of the PCB with the soldering iron.
  4. Place the IC on the PCB, as centered as possible.
  5. Use the soldering iron to apply heat to the backside of the PCB. As the heat transfers to the component side, it will heat up the solder on the pad, and the die of the IC. When they wet to each other, the IC will naturally center itself (though it may need to be nudged with a pair of tweezers)
  6. Pull the iron straight down from the backside of the PCB. Excess solder will pull through the central hole, and the IC should pull flat to the PCB. The remaining pins can now be soldered as usual.

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.