LT Spice AC simulation with specific signal - Page 1
Forum section: electronics / projects

author: mattko
author_rank: Contributor
timestamp: November 20, 2018, 09:28:07 am
content: Hello!I would like to simulate EMC conducted emissions for a three phase inverter topology. As far as I understand there are 3 ways of simulating this:1. Transient simulation + FFT of the signal. I don't like this option because I would like to have more control over the switching waveform. There are also not a lot of options to controll the FFT (e.g. badwidth of sampling).2. AC analysis with a voltage controlled current source + voltage controlled voltage source. For current through switches and SW voltage node. I don't like this, because it sweeps over all frequencies and not just specific switching frequencies I would like.3. AC analysis with specific signal for current and voltage (switching). I don't know how to do this.Any help and tips would be appreciated!

author: macboy
author_rank: Super Contributor
timestamp: November 20, 2018, 03:48:19 pm
content: I'll just point out that you can use a WAV audio file as input to a voltage source, allowing you to have an arbitrarily complex signal. You will need some way to save your waveform as a WAV file. How you make use of that is up to you.For better results with FFT in general, I'd recommend a few settings:- disable "first order compression" in the Compression tab of the control panel, OR add a spice directive ".options plotwinsize=0" which effectively disables compression. The help file also recommends this setting when using FFT.- Try to get a whole number of cycles within the simulation data, which helps avoid DC offset and the resulting increased floor of the FFT plot toward DC. For example, when I test distortion on an audio circuit simulation, I set a "freq" parameter, and use that to set the simulation time to a whole number of cycles (e.g. specify "{50/freq}" as stop time for 50 cycles).- specify the maximum step size in the transient analysis. Lower value will increase accuracy but increase time to simulate, and with compression disabled, the simulation data can become quite large. This isn't as big of an issue these days as it once would have been.

author: Apollyon25_
author_rank: Regular Contributor
timestamp: November 22, 2018, 07:54:09 pm
content: Given the nature of simulation, and given the nature of EMC/EMI, my first question is 'what do you want to achieve from this?'Do you want a simple first order approximation of the topologies for comparison? Or do you want to get super detailed so that your proposed topology and design passes actual compliance?In my experience, the latter is too much effort for too little reward. The former, is more do-able, but you may need an accurate model to get an accurate appreciable difference for comparison so you are back to the latter...

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 23, 2018, 01:24:45 am
content: The best you can do is make a toy model of the circuit as a common and differential mode filter network, and run AC steady state on that, coupling in the expected noise sources appropriately (e.g., switch node is a voltage source, cap-coupled to nearby nodes). Pay attention to representing small imbalances due to component tolerances and circuit geometry, since CM-diff mode conversion is important here and it's very easy to enter excessively lucky values in SPICE!The stimulus doesn't matter any, just scale it afterwards with known switch waveform or whatever. That's what's great about AC steady state, no convolution needed.This still isn't very easy because a practical circuit often has many nodes and complex resonances, and you have to represent all of those with components and couplings. These can be generated with some tools, but you'll be paying five digits for them, and spending an equivalent amount of time setting up and using them. Unless you need the design process, easier to just get the protos in and test them.Or you can build some of the network around the inverter stage, and see how transients get through it. It's harder to get Vrms (let alone QP) this way -- especially through a FWB where you'd have to integrate over multiple line cycles, which just ain't gonna happen in a transient sim.Tim

author: Dave
author_rank: Super Contributor
timestamp: November 23, 2018, 09:14:20 pm
content: Behavioral sourcesin LTspice also accept inputs in the Laplace domain and you can do frequency domain analysis on them. It's going to take quite a bit of fiddling to get it right, but it should be able to do exactly what you're looking for.