0
\$\begingroup\$

I'm trying and want to learn how to use the PWM Switch Model by DR.Vorpérian , both for the voltage mode(VM) and current mode (CM) model. I've read some about the models in "Switched-mode power supplies" by Christophe Basso. However a book can't answer questions, so I hope this thread will be useful on the the way of learning.

Question 1) If I've understood the PWM Switch Model correctly for both the VM and CM case, the model can be directly inserted in any simulation so long it's "rotated" correctly for the current topology, without any modification or calculation necessary because the model is just a linear model of the switch?

Question 2) Which means I can add an infinity amount components outside the so called PWM switch model without the need of modifying the function of the model?

If the answear to the above questions is "Yes" wouldn't it be possible to use the models presented at Bassos webpage which are derived for LTspice?


The model I'm talking about can briefly be found here: https://www.onsemi.com/site/pdf/pcim_basso.pdf

The model symbol when implemented in spice

Yes I do wonder if the LTspice models available on bassos webpage is complete. In that way that they can toggle between CCM and DCM operation and do not need any modifications.


@laptop2d answer

The idea off the model is to simulate the SMPS behavior in a much quicker way than actually components to analyze the circuit in a big scope. To be able to look at the transition between CCM & DCM and to analyze the transfer function and make the circuit stable before moving on to a more real component simulation.

My question do need knowledge about the “PWM switch model” to be answered correctly. If I’ve understood the PWM switch model correctly it only need to be derived once to be implemented in any topology, which in that case means that I don’t have to derive every model to be able to simulate a circuit quickly and tweak them. Which you have to do with the state space averaging (SSA) method which requires that you rederive the average model every time you add or take away any component.

So my questions are; if the PWM-switch model is correctly described for LTspice att Basso’s webpage, can they be used directly? Without any derivation? For any topology? for both the CCM & DCM case for the VM & CM-model?


\$\endgroup\$
  • 1
    \$\begingroup\$ Please post a picture of the model, we have no idea what your talking about \$\endgroup\$ – Voltage Spike Apr 26 '17 at 16:05
  • 1
    \$\begingroup\$ I'm a bit confused. You want to know whether the LTspice models already existent on Basso's page can be used? \$\endgroup\$ – a concerned citizen Apr 27 '17 at 5:53
1
\$\begingroup\$

Question 1) If I've understood the PWM Switch Model correctly for both the VM and CM case, the model can be directly inserted in any simulation so long it's "rotated" correctly for the current topology, without any modification or calculation necessary because the model is just a linear model of the switch?

Sure, if PWM switch model is a spice model and your running a spice simulation, you can insert a spice model into any spice simulator. But why would you want to? If your simulating an SMPS, you'll need a physical switch like a mosfet. Models don't need to be rotated, spice is code. The nets need to match up with the model. If you have a graphical package like LT spice, then it generates a netlist for you but you still need to know how to code in spice when problems arise and check subckt netlists.

Question 2) Which means I can add an infinity amount components outside the so called PWM switch model without the need of modifying the function of the model?

You can't add an infinity of components in any spice simulator or any simulator for that matter, the spice simulator has limits that are based on the computing resources available. If the PWM switch model is a spice model, then it could be used in any spice simulator (unless it has components inside the sub circuit file that are specific to LT spice which is unlikely but possible)

\$\endgroup\$
1
\$\begingroup\$

Let's see how I can answer your questions:

Q1: yes, the idea behind the PWM model is to replace the switching cell made of the switch and diode by a 2-port circuit in which non-linear time-continuous equations describe the average behavior of the cell while switching. This principle follows that already adopted with the hybrid-\$\pi\$ model of bipolar transistors where you replace the transistor symbol by a linear model and follows the pin arrangement c-b-e when rotating the model to match the original circuit. Whether this is a common-emitter, common-base, common-collector or another arrangement, the hybrid-\$\pi\$ model remains the same: it is an invariant model.

With the PWM switch, it is the same. Once you have identified the switching cell in a switching converter, you plug the PWM switch model as shown in the book or even here, for a recent refresh on the subject: http://cbasso.pagesperso-orange.fr/Downloads/PPTs/Chris%20Basso%20APEC%20seminar%202013.pdf The simplest form of the CCM voltage mode model is a "dc" transformer having a turns ratio \$1:D\$, \$D\$ being the duty ratio. Of course, this is a non-linear equation but the cool thing is that SPICE being a linear solver, when you press AC or TRAN analysis, SPICE will always linearize equations around the computed bias point. So if you plug the simplest form of the model (a \$1:D\$ transformer), you can already simulate and obtain the frequency response of all CCM voltage mode topologies. Now, if you want to derive a given transfer function, you will have to linearize the \$1:D\$ model into a small-signal model. Once this is done, plug it back into the circuit and work on a linear circuit.

State-Space Averaging is indeed a powerful tool but as you said, it considers the entire converter during the analysis. Should you want to add a resistor somewhere, a front-end filter then you need to re-start from scratch. With the PWM switch, add any linear component like a front-end filter, a post LC filter etc. the model does not change.

Q2: Yes, there are some LTSpice models in the page you mention and indeed, they work. Please note that from a voltage mode model, you can easily turn in into a current mode model just by adding an equation linking the control voltage \$V_c\$ to the duty ratio \$D\$. The only thing is that you won't be able to predict sub-harmonic oscillations unless you add a second-order polynomial form in series with the \$D\$ generator. A modeling approach of this technique is here http://cbasso.pagesperso-orange.fr/Downloads/PPTs/Duty%20ratio%20factory%20modeling.pdf

\$\endgroup\$
  • \$\begingroup\$ I understand the derivation of the VM case of the PWM switch but the CM model is really hard for me to grasp. According to slide 110 of the APEC 2013 presentation the downslope is dependent on the output voltage of the buck converter. But at another place it's said that V_cp = d V_ap which would mean it's directly dependent on the input voltage. In the book S1 is dependent on V_ac, but v_ac(t) is zero at the time the current ramps up because the switch is closed. What am I misunderstanding here? \$\endgroup\$ – christoph Jul 9 '18 at 17:49
  • \$\begingroup\$ The relationship \$V_{(c,p)} = DV_{(a,p)}\$ is preserved whether you are in VM or CM. Remember, these are average models meaning that the upslope is actually \$\frac{V_{in}-V_{out}}{L}\$ but in terms of invariant relationship and considering 0 V across the inductor on average at steady state, \$V_{out}\$ is actually seen at terminal c hence the upslope equals \$\frac{V_a-V_c}{L}=\frac{V_{(a,c)}}{L}\$. This relationship no longer depends on the buck but suits any of the other structures. Look at the boost and the buck boost, this expression still holds. Does it make sense? \$\endgroup\$ – Verbal Kint Jul 9 '18 at 21:03
  • \$\begingroup\$ For me the difficulty lies in the fact that the time frame in which the slopes are derived is a single period (is it?), so according to my understanding BEFORE the waveforms are averaged. Of course I can simply accept that voltages across inductors are zero as well as currents through capacitors, but this whole approach is just new to me and hard to follow. \$\endgroup\$ – christoph Jul 10 '18 at 16:14

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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