Electronics > Projects, Designs, and Technical Stuff
LTC3895 step down converter burns off
<< < (4/6) > >>
Srijal97:

--- Quote from: capt bullshot on January 07, 2019, 11:22:49 am ---The SMT caps to handle the input voltage won't be small anymore, but still SMT. One can buy ceramic SMT caps rated for such high voltages, though they will be rather large and expensive. You've got a THT cap in your layout, a good film cap will also work here. Don't operate the board without proper input caps, or put some protection circuitry within the IC's power supply.

I wouldn't replace the bootstrap cap, it's just ridiculously large but should work. Most important change would be the GND modification.

If you have access to such equipment, use a variable output power supply to ramp up the input voltage slowly for the first tests, and observe critical waveforms (e.g. the switching node) with an oscilloscope. Be sure to use a very short grounding path for your scope probe, the usual ground clip supplied with the probe often is too long.

--- End quote ---

Okay, I will try and do that tomorrow...and let you guys know what happens.


--- Quote from: capt bullshot on January 07, 2019, 11:22:49 am ---Here's two examples of power stages / step down regulators I've done to give you some impression of how to do GND planes on a double sided circuit board:

http://wunderkis.de/pvbat/converter.pdf

http://wunderkis.de/dcdc/Test-LTC3775.brd.pdf
http://wunderkis.de/dcdc/Test-LTC3775-2.sch.pdf

--- End quote ---

It would be very helpful to see those...but the links don't appear to be working anymore? Also, what other resources would you suggest for these kinds of designs?

Miyuki:
Srijal97: as you have your circuit in SPICE you can simple replace main traces with inductors and put in values from your layout (just convert length of traces to inductance) and you will see what is happening in "real" circuit
It might take little longer to simulate, but can provide fairly close results and show where is your main problem

Use power of computer! We are not 50 years ago when you have just paper, slide rule and need to build many prototypes to do real measurement. Now you can simulate your layout within minutes (sometimes hours) and not wait days/weeks to build many versions and waste money. Even free or very cheap tools can do it today
Srijal97:

--- Quote from: Miyuki on January 07, 2019, 11:47:08 am ---Srijal97: as you have your circuit in SPICE you can simple replace main traces with inductors and put in values from your layout (just convert length of traces to inductance) and you will see what is happening in "real" circuit
It might take little longer to simulate, but can provide fairly close results and show where is your main problem

Use power of computer! We are not 50 years ago when you have just paper, slide rule and need to build many prototypes to do real measurement. Now you can simulate your layout within minutes (sometimes hours) and not wait days/weeks to build many versions and waste money. Even free or very cheap tools can do it today

--- End quote ---

Oh yes, that's a good idea! We'll try and do that too, thanks!
capt bullshot:

--- Quote from: Srijal97 on January 07, 2019, 11:41:48 am ---
It would be very helpful to see those...but the links don't appear to be working anymore? Also, what other resources would you suggest for these kinds of designs?

--- End quote ---

Sorry, that was my fault. I've uploaded them here.

Other resources regarding such designs would be e.g. datasheets and demo board manuals of other DC/DC controllers by LTC / Analog Devices and other manufacturers.They have better ones (datasheets and manuals) than this particular one, describing what is important in the layout. TI also has some good documentation, but it's not always easy to find. Sometimes stuff (like the noise you mentioned in your first post) is over-emphasized within some documents leading you in the wrong direction. The most important part  of a good design is still experience, so it's quite normal to have your first designs fail, that's part of the experience gaining process. Second most important is to provide a massive ground plane to your circuit, usually it delivers better results than trying to divert currents to reduce noise coupling. Third is to reduce stray inductances along the traces where they really hurt in the first place. E.g. having a longer trace in series with the filter inductor isn't as bad as a longer trace from the MOSFETs to to input decoupling capacitor. The stray inductance in series with the inductor just increases its effective value a bit, but doesn't do harm in the first place. Stray inductance within the MOSFETs drain and source connections causes voltage transients that may do harm. Stray inductance within the GND connection of the controller IC causes its ground to bounce in respect to the power ground, leading to all kind of trouble. This is to get your circuit working.

Then you look at the output switching noise, that's the point where you optimize your output capacitor and maybe add an LC filter.

Next would be to reduce EMI, that's the point where you look at minimizing the loops and tuning the gate resistors, as seen somewhere above in this thread.

Last would be to minimize output regulation induced noise, that is where you might think about splitting the ground plane. But if you've done everything right until here, this step won't be necessary anymore in many cases.



Srijal97:
Hello again,

So during the testing with the modified board(extra GND wire and more capacitors), the LTC did not blow up but we had absolutely nothing on the output. We also probed Vout and the Switching node with an oscilloscope(But normal pen type probes, we did not have specialized ones) and saw nothing, a straight 0V line. The output changed from around a few mV to about 600mV upon increasing the input.

We decided to completely focus on getting a new layout done, and I've tried to follow as many points given in this thread, application note 136 (June 2012) from Linear Technologies, and the DC2117A reference board layout. I've attached the new design with this post.

In addition to improving layout, we worked on the selection of proper capacitors. For our last design, we simply bought local capacitors after referring to values that LTpowerCad showed. There was a lot of uncertainty in ESR values. We also had not realized the effect of high frequency that we are using(855 kHz). This time we followed this for the capacitor selection: https://www.powerelectronicsnews.com/problems-solutions/the-buck-regulator-power-supply-design-tutorial-part-2-1

When calculated using formulae given in the tutorial, we found we needed a minimum input capacitance of about 0.7uF and output capacitance of 0.04uF. We also realized that using MLCCs for this purpose is useful and so made capacitor banks using MLCCs. In order to form these capacitor banks, it was suggested in the tutorial to add a bulk capacitor(electrolytic) with a bad ESR in parallel to damp oscillations and reduce ringing. It was also mentioned that a resistor can be connected in series with the bulk capacitor to increase ESR. We were having difficulty finding proper electrolytic capacitors whose values can be clearly defined(ESR value at our operating frequency of 855kHz and effective capacitance due to the DC bias effect due to the input voltage of 120V). We then simply used an MLCC capacitor and connected a series of resistance to it. Is this a good idea? As for our output capacitors, should we do the same or should we use an electrolytic capacitor as part of the capacitor bank?

It would be great if I can get some improvements and comments before I place an order for manufacture, thank you very much for your time!
Navigation
Message Index
Next page
Previous page
There was an error while thanking
Thanking...

Go to full version
Powered by SMFPacks Advanced Attachments Uploader Mod