2
\$\begingroup\$

I am attempting to simulate a DC-DC power supply in LTSpice (using LT3748, 48V in, 5V 3A out).

There is concern about the amount of noise that will be on the 48V input rail, and so we want to simulate with a noisy input (exact figures on the noise levels are also part of my research, but that will be a different question).

To simulate the noise on the power rail I started with something similar to the answer given to this question: How do you simulate voltage noise with LTSpice? Using two voltage sources to give the power, separated from each other with resistors: Two input voltages, each leading into 100R resistors before power rail

This then gives a noisy output based on what SIG and NOISE are set to. My question is; if I know what I want to have on the power rail, how do I set the voltages of NOISE to give me the spike etc that I want? The current draw will clearly play a part, but that is part of what I'm trying to measure. Is there a way to work out what my voltage spikes on V2 should be to get a 200V surge spike on the IN rail based on the value of R9 and R8?

I should add that the NOISE simulation in LTSpice is not really what I am after, I am looking more at surges and spike than noise. There is also an issue with the model of LT3748 (and error about it being time dependant is raised), and so the voltages on OUT are not correctly modelled.

(While this is an isolated supply, I haven't isolated the grounds on either side just to make it that bit quicker to draw).

EDIT: I realise that when I've been saying "noise", that has been wrong. I should have used "surges" and "transients", as they are a better description of what I'm interested in. So the question would be better phrased "how do I put a surge onto my input rail?". With that as the question, PlasmaHH probably has a good answer; putting two supplies in series with one another so that my stable 48V has the pulses put on top of it.

\$\endgroup\$
2
  • 2
    \$\begingroup\$ If you know exactly the waveform your voltage should look like, it is often much easier to use some PWL file for it than to add together multiple voltage sources. If you still want the voltage sources, putting them in series without resistors leads to much better results. \$\endgroup\$
    – PlasmaHH
    Oct 15 '15 at 8:09
  • \$\begingroup\$ Put the noise source (sinewave or otherwise) in series with the main DC feed - forget about resistor coupling - this just clouds the issue. \$\endgroup\$
    – Andy aka
    Oct 15 '15 at 9:46
2
\$\begingroup\$

I concur with @PlasmaHH's idea for the usage of PWL. If you only need a few data points, use the PWL source type directly. Otherwise, put the values into a text file and feed that to the PWL. Excel is nice for this, export as .csv file. That way, any kind of data you can imagine can be converted to a voltage.

This can also work for other primitives besides voltage. Say you wanted a wildly-varying resistance:

  • Create a new voltage source, say V3. Ground one end of it.
  • Create a new net label, say V3val, and wire it to the V3 source.
  • Put the data points into the PWL file of V3 (use whole integers, not "10k".)
  • Add a resistor say R5, and change it's "R" value to "R=V(V3val)".

Then R5's resistance will be modeled as the "voltage" generated by V3.

\$\endgroup\$
2
\$\begingroup\$

You must be aware that one noise is not the other noise !?!? OK, components in linear circuits (amplifiers for example) generate noise, mainly thermal noise and 1/f noise. This is type of noise is what I would call "small signal noise" meaning that these are small signals and you can evaluate them by using a linear representation of the circuit you're investigating. The noise properties of those two voltage sources concern this type of noise. Also you can only simulate the noise behavior of an amplifier by using the noise simulation, this is a variant of the AC simulation. If you would do a time (TRAN, transient) analysis of an amplifier, you CANNOT simulate the noise. OK, I use an advanced simulator called Cadence Spectre, it has a transient-noise simulation but I don't expect LTSpice to have this.

HOWEVER here we are dealing with a NON linear circuit ! It's a switching converter and therefore it has no "small signal transfer" like an amplifier would have. You can only simulate its behavior by running a transient (time) simulation. As I stated earlier, in a transient simulation you cannot simulate the noise.

Also, when talking about noise in relation to switched converters, that noise is not the thermal or 1/f noise of the individual components (see above). What is meant is the spurious content of the DC output voltage, so the variations that are on that DC voltage. Although it is called (switching) noise, it is different in that it mainly consists of spurious components (harmonics) of the switching frequency of the switched converter. "Proper noise" on the other hand (like thermal noise) consists of ALL frequencies.

The good thing is, you CAN simulate this switching noise by using a transient simulation. But the noise settings of the two voltage sources have no relation to this noise !

You want to know the suppression of the noise on the input voltage to the output voltage. This is called "line regulation". What I would do is place a sinewave source in series with one DC supply source (remove the pulse source, there's no use for it) and let it add a small (100 mV) ripple on the supply at a frequency of for example 10 kHz. Then at the output I expect to see peaks at multiples of the switching frequency with additional peaks at + and - 10 kHz around these peaks. The level of these additional peaks gives you an idea of the line regulation. Line regulation is frequency dependent so also try for other frequencies !

\$\endgroup\$

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.