Anyone here a MC34063 guru?

Hello !

So Ive decided to use a mc34063 to drop 12V to 5V at 0.2A max loading, with a switch freq. around 100kHz. Sounds straight forward and was almost done prototyping it but second guessed myself and wanted to sim it first (just to be sure)

I looked around for a model for this device and came across a couple and decided to use one of them. However, after simulation and iteration after iteration, it seems that the model is not showing me the entire picture.

Ive attached a folder which contains the actual sim that im generating for my design and it contains the model (and the orginal authors demonstration circuit) as well.

From what Im seeing, I need to load my converter significantly to get the a clean SW node voltage, CC in the inductor and the a Vripple of 100mV (or less).

If I only load the converter with the load its designed to drive (25ohms on a 5V output rail), my switch node rings and my inductor current has mini peaks (almost like sub.harmonic osc.)

So, here's what Im guessing: either the model needs to be fined tweaked or I need to decrease my freq (and I tried that, it really didn't make that big of a diff.) or I just need to deal with it.

I went out and bought a car 12V USB charger and guess what?? it had the classic mc34063 buck configuration! so I quickly probed SW nodes, cap charging etc and here's what Ive found: the SW rings (just like in the sim) at no/very light loads and is clean when the converter is loaded.

After the sim and the actual probing, I'm beginning to lean towards the fact that the model needs tweaking. But I'm no LTSPICE expert and would like to get an opinion.

Any suggestions? Thanks!

Post your schematic as image. For your spec MC34063 Application circuit also works well. And you must be put a PCB as per the datasheet then only its works well. Or otherwise you should not get proper result.

I ran your simulation and I see your issue. It's not surprising that hysteresis converters tend to show chaotic behavior. The "ringing" is just discontinuous conduction, and should be expected at light loads with any controller. The subharmonic oscillation you're seeing is partially due to the hysteretic control, which tends towards instability if there is too much delay in the comparator and switching compared to the oscillator period. If you want to get rid of that oscillation, then lowering your frequency is probably the best option. As it is, the subharmonic oscillation basically cuts your effective frequency in half anyways.

Also another tip, you can view the internal behavior of your subcircuits in LTspice by going to the control panel, "save defaults" tab, and checking the save subcircuit node voltages/currents boxes. That should give you more insight into what's really going on.

I agree that the simulation probably shows realistic 34063 behaviour. Expecting clean (low ripple etc.) operation under load variation from this cheap and pretty old chip might be expecting too much. Some points are just normal operation, e.g. the "ringing" output node will be observed with any asynchronous buck converter in discontinuous mode, as mtwieg mentioned. The oscillation is involving low energy and not an actual problem. You'll need a snubber if you want to supress it for some reason.

In real live, the exact converter waveforms will be affected by various parasitic cicuit elements. I don't believe that you can reproduce it easily in simulation. You'll better tune the final circuit empirically. If you want predictable behaviour, use a state-of-the-art buck converter chip.

Use this tool Almost perfect for MC34063 and a lot other things.

Well.. a couple of things Ive been observing. So get ready for lengthy post. But let me state one thing: I always use LT controllers..i love them and I think the jigs provide great base templates to expand on and reach a final modifiied design. However, they are quite expensive and when Im working on my pocket..mc34063 it is!

Now, the ringing is caused by the inductance ringing with the diode capacitance. A damping resistor is parallel with the inductor should clear that out. 1K value seems fine.

Secondly, this hysteretic control, as already mentioed here, is really a bad control mode in terms of loop analysis. So, just like what the author of the model did in his example, I can add an external op amp to compensate the filter phase shift add some gain.

However, the author compensates the peak current control. I dont know how thats working because I cant see in the block diagram of the current sense circuitry. But if I have asked the author to explain the working of his control loop and once Ive understood it, I can make do with the changes.

But I did my simulation to stop oscillating: Increased the capacitance and added more ESR to add the ESR zero earlier and help cancel out one pole from the LC filter.

chimera786 said:

Now, the ringing is caused by the inductance ringing with the diode capacitance. A damping resistor is parallel with the inductor should clear that out. 1K value seems fine.

Click to expand...

The ringing shouldn't be a problem, adding a damping resistor will likely just dissipate extra power. If you really want to damp it a RC snubber would be better.

Secondly, this hysteretic control, as already mentioed here, is really a bad control mode in terms of loop analysis. So, just like what the author of the model did in his example, I can add an external op amp to compensate the filter phase shift add some gain.

Click to expand...

I'm not seeing any op amps used in any of these circuits. A phase lead capacitor from the output voltage to the Inv pin will probably help with stability and noise immunity.

Here is an old thread on hysteretic converters that might be of interest:
https://www.edaboard.com/threads/255435/
Using the feedback method shown there (taking DC feedback from the switch node instead of the output, while coupling AC feedback from the output) might be an interesting solution for this problem.

Actually, there is a an op amp and its in the file labelled 15V_3V3. Its in the other folder present in the zip file.

I haven't done much work with hysteretic control and would like to get a first hand experience using it via this controller chip..but if i cant a good feel for the controllers behavior in the simulation domain, I'm not so comfortable using it in a real design.

This was for a personal project. I really don't want to spend 5 bucks (on average) on a controller from, for instance, LT. I love their jigs and can really go to town on their controllers, but too expensive for a personal project.

At any rate, yeah the RC snubber is a good alternative but I usually reseve that if the SW in ringing too excesively..by the way, you should check this link out.. its saved my design a few times: **broken link removed**

I'll post back with some more findings