Using the TLC5940PWP package correctly (TSSOP w/ PowerPAD)

Community PCB Design
1

Hi everyone,

I’m trying to design a board around the TSSOP version of the TLC5940 IC (a 16-channel LED driver) present in SparkFun’s Eagle library. This chip has a thermal pad on the bottom which TI recommends connecting to a ground plane. Whoever designed the Eagle package was nice enough to include an SMD thermal land for soldering the thermal pad on the underside of the chip to, as seen here:

http://i.imgur.com/wJmLn.png

Based on my understanding of [this “PowerPAD Made Easy” guide (pdf) and [this technical report (pdf) from TI, I think I have a couple of options for making use of the powerpad:

  1. Connect the powerpad to a large area of copper and expose an area of this copper using a solder-mask defined pad. (single-layer PCB)

  2. Do #1 AND add thermal vias in the exposed copper region to connect to an internal ground plane. (multi-layer PCB)

So far, does this seem correct?

My real question is how do I actually go about connecting that SMD pad in the package to my ground plane in Eagle? When I place my chip on the bottom layer, which has the ground plane, I see a border around the thermal land:

http://i.imgur.com/GUnOA.png

Even if the chip were on the top layer, I don’t see how I could connect the thermal pad to the ground plane without using vias.

Thanks!

-vishal

(p.s. I have read phalanx’s replies on this thread: viewtopic.php?f=20&t=7314 . This was very helpful and probably the route I want to go, but I need to know how to connect up these pads/vias first.)](http://www.ti.com/lit/an/slma002g/slma002g.pdf)](http://www.ti.com/lit/an/slma004b/slma004b.pdf)

2

Hi Vishal!

Here is how you can go about making the Sparkfun library part work in the way you want it to. The library itself needs to be modified so you can make connections to the GND pad in the TSSOP28 package.

This first step is optional depending on whether or not you want thermals to appear when connecting a plane to the GND pad on the same layer. If you don’t want thermals on your GND pad but want thermals everywhere else on your GND plane, you need to open up the Sparkfun library in the editor and edit the package for the device. Click info on the center pad and uncheck “thermals.”

http://home.comcast.net/~wahconah98/pcb/tpad01.jpg

Next, you have to edit the TLC5940 package. Once there, we need to edit the TSSOP28-GROUNDPAD varient connections. When the connection window pops up, you will see that Pad 29 isn’t connected to anything. If you are using Eagle 6.0 or higher, you can now assign multiple pads to the same pin (earlier versions would require another pin to be defined in the symbol). To do this, highlight Pad 29 in the list as well as the G$1.GND line in the Connection box. Once highlighted, click Append.

http://home.comcast.net/~wahconah98/pcb/tpad02.jpg

When Pad 29 has been appended to the connection G$1.GND, it will look like this which means the GND pin from the symbol is now connected to Pad 1 and Pad 29 on the package.

http://home.comcast.net/~wahconah98/pcb/tpad03.jpg

To connect your ground pad to GND, simply connect Pin 1 to GND in your schematic.

http://home.comcast.net/~wahconah98/pcb/tpad04.jpg

When you look at your board layout, you will see that the top layer GND plane I made connects to Pad 1 with thermals and to the ground pad without thermals. To get the ground pad to connect to the plane on a different layer, I manually added vias defined as ‘GND’ to the area where the signals overlap.

http://home.comcast.net/~wahconah98/pcb/tpad05.jpg

Eagle 6.0 and up now support arbitrary pad shapes which could also be used if you feel like experimenting. Their limitations are listed in the Eagle help files and users guide.

I hope that gets you moving in the right direction!

-Bill

3

Thanks for the superb answer, Bill! Seeing the pin connection dialog was the “aha!” moment for me, as I have almost zero experience with editing packages and hadn’t ever seen that before. I think this will carry me a long way, so thanks again!