LMR14006Y cannot reach Iout 0.6A

Hello,

You should make sure that your power supply can provide the right amount of current. If it is current limiting then the output of the LMR14006 will not be regulated at load.

Also, please share your clear pictures of layout (preferably in pdf format) with us so that we can debug the problem better.

Regards,
Akshay

Il will check again the PSU, in the meantime here is a snapshot of the "pcb"

The bottom layer is all groundplane

I did try to reiforce the connection to groundplane to the GND ping of the chip, no difference

tryed to increase the inductor L14 ten times, no mayor difference

Your layout looks un-optimized and if you are able to verify that your power supply is indeed not current limiting, then I believe you are seeing problems because of noise coupling. Your feedback network is right next to the inductor, your diode ground and the input cap ground are far away, and even though your bottom is all ground, you are connecting to it through vias which add inductance in the path. Please go through the layout guidelines on page 13 of the datasheet. You could also look at the demonstration board for LMR14206 (http://www.ti.com/lit/ug/snva502b/snva502b.pdf). The LMR14206 is part of the same family as LMR14006 and you could use the same board, if you'd like, after replacing the IC.

Increasing your inductance should not be much difference. When there is no apparent problem with the BOM, it usually is the layout that can cause issues. At high switching frequencies this is more of a problem.

I hope this helps.

Regards,
Akshay

ok, basically the main difference I see is that the L1 inductor is righ close to the pin, whereby on my board it is a bit further away. There is also the case of the feedback trace that is longer.

So, assuming that the chip can actually arrive to .6A I should draw a small board that I will then test with the samples I ordered.

I will let you know, thanks

The easiest thing would be to use the LMR14206 board and change the IC to check your design. SMPS have to be laid out such that you bypass noise properly. I have attached a presentation for your perusal too.

Regards,
Akshay

8484.Switching Power Supply Design_ EMI.ppt

Good catch! This makes it much easy to layout the board properly.

Wow, yes ! 

To be sure: when packaged in TSOT-6L package pin 1 is CB and pin 6 is SW

I had the footprint correct but mixed the drawing, testing time....

About the EMI, I had no issues whatsoever with EMI..

We would still suggest that you consider laying out the board according to the guidelines. it would definitely help your performance.

Regards,
Akshay

Ok, attached there is a layout that should be good and with real components

Talking about EMI and avoiding overvoltages I followed the AN 88 of Linear and added a .5 ohm on the input net A_DC_VIN

C37 is 4.7uF 100v ceramic, the resistor should avoid excessive inrush and overvoltage from the L13 filter

The question: Do you expect any instability on the swithing by adding the R8 to the circuit ?

Thanks

Hello,

Here are some comments.

You want to keep the catch diode and input cap ground very close to each other. I'd suggest moving the indcutor to the right, rotating the bootstrap cap 90deg rightwards, and then rotating the diode leftwards such that the anode and input cap ground are right next to each other. You need multiple vias (kind of via matrix) at C37 ground, anode of diode, lower feedback resistor, the ground pin, and the output cap ground. Single vias add inductance and having multiple in parallel help reduce that and provide a low impedance path for high frequency AC currents. Since you are using only the bottom layer as ground, you want to make as many connections to that as possible. You also want a good solid copper fill from your filter inductor to the input. I am not sure what C35 is being used for. You could use an electrolytic there and that could be your bulk cap. Please refer to the attached spreadsheet for input filter component selection.

Your surge limiting resistor (R8) is in series with your ceramic cap. If you want to limit a current surge in to the input pin then you need the resistor in series with input pin and filter inductor. Your C37 should be right at the input pin because its bypassing noise there. Your R8 when introduced in the power path is going to cause a good amount of power loss. Ideally you do not want any resistance in the input path.

You could use an 0805 cap for bootstrap. I think you are using a bigger one. Your Vout trace is still right next to the inductor. I usually route it on the bottom layer with a ground middle layer. This way its away from the inductor flux and also has ground shielding.

I hope this is helpful.
Regards,
Akshay

Thanks, I will make the most of your post, bearing in mind that I am on a two layers PCB and have some positioning issues

Ragarding R8, that was the real question, please find attached the AN that explain its rationale

It would be great if you could comment on it

Thanks

ok, new layout according to indications

Surge limit resistor is now before cap, as correctly required

Thinking about it, it would be great if in the datasheet there was a real example of a layout

This placement looks much better. I would actually suggest using a NTC thermistor instead of a fixed resistor for surge limiting. This way your DC loss would be lower and you would still have good surge limiting. Also I would increase the number of vias on R48 and C35 ground and make min trace width about 20 to 25mils.

The example layout is usually the EVM. The datasheet does not usually have the example layout because the EVM user guide is written exclusively for the EVM. 

Regards,
Akshay

I am having trouble to find a suitable NTC, the logic is that the "steady" current will heat it up so it exibits a low resistence. But this circuit does have a low "steady" current and form time to time it wakes up and do work. I am wondering if I will "starve" the board at wakeup time, (also thinking of main supply possible drop)

Maybe you have a pointer on the matter ?

A PTC like nichicon ZPC1MCC0R3B is more like it in term of resistece but is quite costly and is PTH mount. 

Thanks !