DC-DC Converter/ Feedback/ Verilog-A

OK, asking three different questions in one thread means that something is likely to get lost, but let's see.

1. You probably need to use pss/pstb rather than stb. Both pstb and stb don't "break the loop" (which is the traditional way of simulating stability, by keeping the loop closed for the DC analysis and opening it for AC; this has problems with correctly taking the loading into account). Instead it injects a signal at the probe point and measures it returning around the loop (it's a bit more complicated than that, but that's the principle). Spectre has had this for many many years now. The stb analysis is geared up for when you have a DC operating point and then does a small signal analysis around that. For a switching circuit, you're more likely to need to analyse a period of operation of the circuit and use this time-varying operating point to analyse the time-averaged stability using pstb. I've certainly used PSS (a SpectreRF analysis) to analyse DC to DC converters and gave a paper at a UK National Microelectronics Institute event a few years ago to show this.
2. Spectre has transformers, current sources and all those kind of components. There are analogLib components for them, plus they exist in spectre itself. You can type "spectre -h" on the UNIX command line to find out more info on what's available, or read up in <MMSIMinstDir>/tools/bin/cdnshelp
3. VerilogA models - there are a number of models in ahdlLib and bmslib in the Cadence installation, but you may also want to look at The Designer's Guide Model Library. 

Regards,

Andrew.

Hi Andrew and thanks for the quick reply.

To be honest I didn't understood the point 1.

I have used PSS analysis, in fact I kind use this PSS analysis to make almost all my simulations, instead of transient (more fast).

In the paper that you gave at UK NMI event you have analysed the stability of the DC-DC Converter? Can you send me a private message and tell me where can I find that or maybe you could send me that paper?

Returning to the question of the STB, PSTB, PSS, when you say PSS/PSTB means that one should perform those two simulation at the same time?

Here: http://www.lumerink.com/courses/ece5411/Handouts/Loop%20Stability%20Analysis.pdf you can find the slides from what I was talking about.

As you can see, they put the iprobe at the OPAMP output.

If we grab what you said,  "Instead it injects a signal at the probe point and measures it returning around the loop (it's a bit more complicated than that, but that's the principle)" and look at the schematic on that slides I showed above, slide 4, this means that the iprobe, that has an arrow pointing from "left to right", located at the output of the OPAMP and before the feedbac, is injecting a signal there, that will be going to the load and to the feedback loop? Is that it?

You said "The stb analysis is geared up for when you have a DC operating point and then does a small signal analysis around that. For a switching circuit, you're more likely to need to analyse a period of operation of the circuit and use this time-varying operating point to analyse the time-averaged stability using pstb."

In this case, because we are dealing with a switching circuit,  we're in the presence of a time-varying operating point and what you said in bold is totally right (of course!).

Let me see if I can explain myself and expose my doubt clearly. This means that we can analyse the stability of the DC-DC Converter directly through simulation using the PSS/PSTB, even though knowing that the power devices are non-linear and the circuit is time-varying? There is no need build a linear model, like that one that Mr. Basso's uses in his book using a transformer, current source, etc?

Thanks for your time.

Regards.

I'll send you the presentation I gave. 

More detail on stb can be found in the paper referenced in the slides you shared the link for - http://www.kenkundert.com/docs/cd2001-01.pdf

You cannot use pstb on its own. Like pac, pnoise, pxf etc, it requires the "periodic operating point" found by the pss analysis. The pss analysis captures the non-linearities caused by the large signal periodic sources that you're varying, and then the pac/pxf/pnoise/pstb analyses perform a small-signal analysis around that periodic operating point. So it will include info from the complete switching cycle - however, it is looking at small-signal stability still.

I can't comment on Mr. Basso's book since I've not read it.

Regards,

Andrew.

Thanks for the reply.

But being the DC-DC Converter a time-varying and a non-linear system, we can directly simulate and ask for the stability using the PSS/PSTB without any problem?

I'll be waiting for the paper.

Regards.

Yes, we can. The system is linearized around the time-varying operating point found by the pss analysis and an analysis equivalent to the stb analysis is performed for the zero sideband (the frequencies around DC). You can find a very good presentation on this subject in https://www.cadence.com/cdnlive/library/Documents/2009/EMEA/CD12_WerthT_iasrwth.pdf.

Hi, thanks for the reference.

In order to design the controller, we need to get first the transfer function of the converter so that we can see how he behaves and then study what kind/type of controller we'll need to design. So far so good.

Now, when we're doing the analysis of PSS + PSTB, we need to have all the converter structure designed and working, that is, all the structures in place (power stage, drivers, feedback loop, etc) and by using that analysis we are testing the overall feedback system stability (with the compensator/controller designed, LC filter chosen, etc) right? It seems to be like that of course!

But, what if I want to get the bode plot only the converter itself (to see how the converter it behaves), not resorting to the transfer function (obtained for example through SSA) and then matlab, can I still use the PSS + PSTB analysis to do this?

This is a very important question for me.

How could this be done? For example, having a vpulse source connected to the drivers section along with the power devices and the LC filter attached to the load (resistor) with all the respective vdc sources how I could manage to do that same anaylis and the bode plot of the converter behaviour? After all this is a open loop scheme (the one I described right now)

I would appreciate all the help on this.

Thanks in advance.

Regards. 

 If the loop is not closed, you can use pss + pac analysis (or pss + pxf analysis).

Ok. It makes sense.

Allow me to put my thoughts here regarding this issues that I am trying to address.

(I don't know if you are familiar with DC-DC Converter operation and theory) 

As I said before, maybe not in a clear way, something that had confused me (after reading the SMPS: Spice Simulations and Practical Designs (from Basso) as well as the book Power Electronics Principles (from Erickson) and then go after a solution to get what I am trying to do) was the fact that because we are in the presence of a time-arying circuit with non-linear components (Switches), the authors from the books I referred had modeled the switches in such a way so that they could become linear and from there be inserted into the overall converter to be simulated. The PWM is another example, it is another non linear circuit, modeled too in a way to become linear and so on.

With all this done, the circuit becomes time invariant and linear. In this way we can simulate the circuit without problems, "break" the loop and see the stability and so on.

Now in my searchs I found this solution PSS + PSTB that we're talking in here.

So when you say that the system is linearized around the time-varying operating point found by the PSS analysis, we can say this is similar/equivalent to insert that linear model that I talked just now into the circuit? Or it doesn't have nothing to do with that?

Can I ask you to elaborate what means "performed for the zero sideband (the frequencies around DC)"?

Thanks for you time!

Regards. 

Pyroblast said:

So when you say that the system is linearized around the time-varying operating point found by the PSS analysis, we can say this is similar/equivalent to insert that linear model that I talked just now into the circuit?

Yes.

Pyroblast said:

Can I ask you to elaborate what means "performed for the zero sideband (the frequencies around DC)"?

Please see http://www.designers-guide.org/Forum/YaBB.pl?num=1385605542.

But Frank, in this case do I need any special arrangement to do this PSS + PAC analysis? For example as we need a iprobe for the PSS + PSTB?

Do I need to insert any other component in the circuit to perform the PSS + PAC analysis? I have a vdc power supply to supply the converter, then I have a vpulse to generate/simulate the PWM duty-cycle connected to the non-overlap circuit.

Regards.