Help with designing LM3404 LED driver in Eagle CAD

[aiq25]

Hi. I'm trying to design an LED driver using the LM3404 IC. I have a basic schematic and PCB layout done but I need some helping finishing it. I'm new to LED drivers and doing PCB layout. I'm using Eagle CAD to do the PCB layout. Attached are all my files. For the inductor I'm planning on using a through hole component, since it will be easier to solder. The part I'm planning on using is LHL13TB101K. I created a library for this part and for the LM3404 IC. I'm not sure if the package is correct the way I have it. I took a through hole component and just change the spacing to create this. If someone could verify this I would really appreciate it. I'm planning on adding a SMD inductor, SDR1806-101KL. I haven't added this to the schematic. I think I'm just going to create some padding based on the PCB so I can try to solder this instead of creating a part for this and adding this to the schematic. Does this seem like a good idea?

Also, I looked at the application/demo board for this IC. On there they have some large traces connecting VIN, GND, LED+ and LED-. I was wondering how wide do I need to make these traces? Here are the specs of my application:
Vin: 39-40V
Vout: ~33V
Iout: 0.6A

I used the TI WEBENCH to create the schematic and get the values. I will be hand soldering this.

[aiq25]

Here are the schematic and board layout so far:

[XFDDesign]

There were a few bugs I found in the design. Namely:
1. For your through-hole foot print, you put a drilled hole on top of a through-hole pad.
2. Your bottom ground plane was not connected to your top ground plane.
3. You had some unfinished/unrouted connections to deal with.
4. (Design opinion) you had too much spread for your components. A switcher with long loops and traces for the magnetics will sing to any device willing to listen. [fixed.]
5. (Design opinion) Changed sense resistor connection to a Kelvin-like connection. Not necessary, but it makes it a bit cleaner.
6. Setup the cam file to export gerbers and a drill for you.
7. Exported gerbers + drill.

Cheers!

[aiq25]

There were a few bugs I found in the design. Namely:
1. For your through-hole foot print, you put a drilled hole on top of a through-hole pad.
2. Your bottom ground plane was not connected to your top ground plane.
3. You had some unfinished/unrouted connections to deal with.
4. (Design opinion) you had too much spread for your components. A switcher with long loops and traces for the magnetics will sing to any device willing to listen. [fixed.]
5. (Design opinion) Changed sense resistor connection to a Kelvin-like connection. Not necessary, but it makes it a bit cleaner.
6. Setup the cam file to export gerbers and a drill for you.
7. Exported gerbers + drill.

Cheers!

Thank you so much for your help, I REALLY appreciate it. Just one question. When I opened the project in Eagle the top and bottom plane were not visible. Attach is a screenshot of what I mean. I just need to click on "Ratsnest" correct?

[free_electron]

Not good. Your layout is scrap.
The diode needs to be as close as possible to the chip.
The coil is the wrong type.
Your sense resistor placement is wrong. The return path is much too long. Your output cap needs to be tied to ground, not sense.

A switcher is a power converter. It pumps energy from the source in the coil. So in fase one current flow supply-chip-coil-led-sense resistor-ground-supply
In fase two current flows coil-led-sense resistor-flyback diode-coil.

Those are the two loops that need to be optimised to be as small as possible

[marshallh]

Take a look at some commercial SMPS layouts. Read Maxim, Analog Devices etc appnotes for proper layout of these devices. Loop area is critical on some nodes. Understand current flow in relation to the pcb geometry and return paths.

[XFDDesign]

Thank you so much for your help, I REALLY appreciate it. Just one question. When I opened the project in Eagle the top and bottom plane were not visible. Attach is a screenshot of what I mean. I just need to click on "Ratsnest" correct?

Right. That does a copper pour.

Someone else pointed out you don't have the right inductor. Mouser states it's a 0.79A inductor, which is much too low. You may be going for 0.6A avg out, but you have to factor in ripple current and other switching factors. Typically you will design for a target ripple current, then you find an inductor with an Isat_max = Iavg + Iripple + some_small_margin. I would be looking for an inductor of 3A I sat at a minimum, personally.

[aiq25]

Thank you so much for your help, I REALLY appreciate it. Just one question. When I opened the project in Eagle the top and bottom plane were not visible. Attach is a screenshot of what I mean. I just need to click on "Ratsnest" correct?

Right. That does a copper pour.

Someone else pointed out you don't have the right inductor. Mouser states it's a 0.79A inductor, which is much too low. You may be going for 0.6A avg out, but you have to factor in ripple current and other switching factors. Typically you will design for a target ripple current, then you find an inductor with an Isat_max = Iavg + Iripple + some_small_margin. I would be looking for an inductor of 3A I sat at a minimum, personally.

When looking at the current I should look at the Max DC current right? I don't see just a current parameter for this inductor on Mouser. The Max DC current for this inductor is 2A. I'll switch to a 3A one. Thanks.

[aiq25]

Here is an updated design. I'm still looking at what parts to use. I'm not really sure how else to reduce any loops. I will try to pack everything closer together. I'm trying to create a 3D rendering of this so I can get a feel for how all the parts will look (at the IC and the SMD components). I think that will give me a better idea of how much I can move the components by and try to reduce the size even further.

[marshallh]

Check out the eval board:
http://www.digikey.com/product-search/en?mpart=LM3404MREVAL&vendor=296

Click on the eval guide PDF in the datasheet section. Board layers are in there so you can see how they laid it out.