2
\$\begingroup\$

I took from the website of Christophe Basso a simplis simulation. I have some questions about it to be sure to understand it. Here is the schematic of the simulation:

enter image description here

It is a current mode buck converter. I do not understand the purple parts: R4, C2, R7 and the gain G2. Are those values are here to simulated a particular IC? In particular the transfer function of the op amp integrated into the IC? Like the one above (link to the datasheet):

enter image description here

Would it be possible to simplify the schematic like this:

enter image description here

Thank you,

\$\endgroup\$
3
  • \$\begingroup\$ Calling @VerbalKint. \$\endgroup\$
    – winny
    Commented Nov 16, 2023 at 15:23
  • \$\begingroup\$ @winny Title does already :) \$\endgroup\$ Commented Nov 16, 2023 at 15:25
  • \$\begingroup\$ @winny - Just FYI, even though you can type a username into a comment, that does not mean that it sends them a notification. That username would not "autocomplete" when you typed it and that's the indication it's not a "valid" usage. Apart from a few corner-cases (e.g. notifying an editor of the post) that user would need to have written a comment before yours, on the same post (in this case, the question) before it's possible to trigger a notification by writing @their-username. More info here. Hope that's useful. \$\endgroup\$
    – SamGibson
    Commented Nov 16, 2023 at 18:09

1 Answer 1

4
\$\begingroup\$

The circuits I provide in my 90+ ready-made templates are simplified versions of what a real controller would do. It is for clarity reasons, so that everyone can understand the operating flow, but also for coping with the limits set by the demo version. I have circled some of the blocks in the below figure:

enter image description here

  1. The voltage-controlled current source \$G_2\$ together with resistor \$R_5\$ form a voltage divider with a ratio of 330m x 1 = 0.33, a divide-by-3 block as you can find in the UC384x circuit for instance. This block is there to force a higher operating voltage in the op-amp output for a low peak current setpoint. For instance, if the peak current has to be 5 A across a \$100-m\Omega\$ shunt, then you need to apply 500 mV as a voltage setpoint to the current-sense (CS) comparator input which is low for an op-amp. With this extra divider, for the same 500-mV setpoint, the op-amp output will be at 1.5 V, improving the noise immunity significantly.

  2. in any current-controlled power supply, you need a maximum peak current setpoint during the start-up sequence (the loop is open until the output reaches the target) or if the loop fails (short circuit or open-circuited return path) to limit current runaway. Here, I limit the maximum setpoint to 1 V (as in a UC384x) but it could be a lower value for practical reasons (you now see 0.5 V in some ac-dc offline controllers, or much lower in low-voltage dc-dc converters). To clamp this value, I use a piece-wise linear (PWL) resistance whose current depends on the applied voltage. You describe its behavior with lines you fill out:

-100 -2p / 0 0 / 0.99 2p / 1 100

For a positive voltage below 0.99 V, the part leaks with a 2-pA current and it brutally conducts when the voltage reaches 1 V. It leaks -2 pA below -100 V. You can add as many segments you want depending on the usage.

  1. this block injects slope compensation whose level is computed by the macro. The sawtooth \$V_{saw}\$ is buffered and adjusted in amplitude by coefficient \$k_r\$ and adds up to the inductor current transformed in a source by \$F_1\$. \$R_4C_2\$ form a cheap \$RC\$ filter which is done via an active leading-edge blanking circuit (LEB) in a real circuit. The LEB is there to blind the controller for a few hundreds of ns so that it does not react to spurious pulses when the power switch turns on. The \$RC\$ filter simply integrates the current information and attenuate the pulse in this simplified circuit. You can certainly omit here but it does not cost a dime to keep it ^_^

  2. this op-amp is a simplified version of what is proposed in the simulator. I built this circuit that I already used in SPICE to shape the frequency response the way I need. Once the converter operates as expected, I usually replace this simple model by a more complex one or the real part. I always debug with a simple arrangement that I later improve.

enter image description here

The first block with \$G_1\$ and \$R_{OL}\$ build the dc gain, \$A_{OL}=g_mR_{OL}\$ and then a low-frequency pole is introduced at \$f_p=\frac{1}{2\pi R_{OL}C_{OL}}\$ and is located at 30 Hz. If you want to add a second pole, simply insert a unity buffer after \$C_{OL}\$ made of a current-controlled voltage source like \$G_1\$ (100 µA with a resistance to ground of 10 kOhms for instance) and add a capacitor of your choice across the resistance to place the second pole. The output of this extra buffer is clamped as in the original circuit.

\$\endgroup\$
1
  • \$\begingroup\$ What would be my job without you ? \$\endgroup\$
    – Jess
    Commented Nov 26, 2023 at 19:50

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.