1. LTspice
  2. Теми

Ultrasound transducer modeling - NanoVNA, s2spice inside #S-parameters

 

I guys,

I'm working on some ultrasound transducer signal conditioning (1-port device for emission/reception).
I have a NanoVNA to measure transducer impedance and I'm able to use these measurements with a custom subcircuit in LTSpice.

Question 1 : looks like s2spice is not able to create 1-port device library because it asks me to choose between 2 and 8 ports.
Why ? Is there a way to convert s1p file to LTSpice 1-port device ?
For now, I created a Python script on my own to create it but if there is something generic on the shelve it would be better.

Question 2 :
- During the emission step, the transducer is a load for the high voltage driver, I can simulate it "easily" with LTSpice adding my subcircuit in parallel => cool
- But during the echoes reception, the transducer acts as a voltage source (few mV) and I don't know how I am supposed to use my "impedance" subcircuit. In serie with a volatge source ? In parallel ? Just don't use it ?

Any help on these two topics would be really appreciated <3
 

On 16/07/2024 11:18, 6u1lh3m@... wrote:
I'm working on some ultrasound transducer signal conditioning (1-port device for emission/reception).
I have a NanoVNA to measure transducer impedance and I'm able to use these measurements with a custom subcircuit in LTSpice.

Question 1 : looks like s2spice is not able to create 1-port device library because it asks me to choose between 2 and 8 ports.
Why ? Is there a way to convert s1p file to LTSpice 1-port device ?
For now, I created a Python script on my own to create it but if there is something generic on the shelve it would be better.

As you know, S11 is just a representation of complex impedance as a reflection coefficient referred to a reference, usually 50Ω. It's easy enough to do it in a spreadsheet. If you have implemented the conversion to R+X in a script, why not carry on using it?
Question 2 :
- During the emission step, the transducer is a load for the high voltage driver, I can simulate it "easily" with LTSpice adding my subcircuit in parallel => cool
- But during the echoes reception, the transducer acts as a voltage source (few mV) and I don't know how I am supposed to use my "impedance" subcircuit. In serie with a volatge source ? In parallel ? Just don't use it ?
You are free to use the series impedance form with a voltage source, just like you would do with a microphone or phono cartridge source.

What I would do instead of directly using the Freq, R, X table that you have is to devise a simple RCL equivalent network that approximates your measured impedance - rather like that of a quartz crystal. That's probably good enough and is more friendly to analysis in the time domain, which can be an issue with impedances implemented as Freq, R, X tables.

--
Regards,
Tony
 

6u1lh3m,
 
Thinking in a general sense, if you don't know how it should be represented electrically, then you have to treat it as an unknown "black box" where the only thing you know about it is its terminal impedance Z(f).  A black box might literally be a complex RLC network which happens to have a source embedded somewhere in the middle of it, and you don't know where, making it impossible to tell where to put the source in your model.   It is not likely to be that complex, and at the end of the day it might not matter.
 
I would make a "best guess" as to what it actually looks like electrically, and build it that way.
 
You wrote that "the transducer acts as a voltage source" and I am unsure how to interpret that.  Does it mean you already know it's a voltage source?  Or that it drives a very high-Z load, so that only the driven voltage is sensed?  Do you know that the voltage is directly proportional to the acoustic 'signal' (as a function of frequency)?
 
For me, the answer to the question is a big unknown.  You mentioned "signal conditioning" and it could mean that you need to adjust its frequency response to flatten out imperfections in the transducer.  Let's say, for example, that it is resonant with a sharp peak.  That might suggest that you need to construct an equivalent circuit based on more than the VNA's measurements.  Will the signals, or the simulations, be narrowband so that it doesn't really matter how you draw it?
 
Andy
 
 

As you know, S11 is just a representation of complex impedance as a reflection coefficient referred to a reference, usually 50Ω. It's easy enough to do it in a spreadsheet. If you have implemented the conversion to R+X in a script, why not carry on using it?
I managed to make the s2spice work for 1-port device... It accepts 1 as the number of port even though it says no... BUT the data are converted in a bad way... So, I will definitely keep using my script.
 
You are free to use the series impedance form with a voltage source, just like you would do with a microphone or phono cartridge source.
It makes sense indeed. I will try to do it like that to see how it looks.
 
Thank you for your help
 
 

You wrote that "the transducer acts as a voltage source" and I am unsure how to interpret that.  Does it mean you already know it's a voltage source?  Or that it drives a very high-Z load, so that only the driven voltage is sensed?  Do you know that the voltage is directly proportional to the acoustic 'signal' (as a function of frequency)?
In fact, I'm sure of nothing about it. I consider it as a source voltage because I have some "voltage" on the scope during echoes. It is connected to a LC network just before a HF transistor that perfoms a first stage amplification : not really a high-Z load...
 
For me, the answer to the question is a big unknown.  You mentioned "signal conditioning" and it could mean that you need to adjust its frequency response to flatten out imperfections in the transducer.  Let's say, for example, that it is resonant with a sharp peak.  That might suggest that you need to construct an equivalent circuit based on more than the VNA's measurements.  Will the signals, or the simulations, be narrowband so that it doesn't really matter how you draw it?
My ambition is to be able to simulate all or part of the "chain" to understand how any component impact impedance, bandwitch etc.
Maybe I’m trying to do something too complicated cauz I'm not sure to understand what I'm doing :D
 
Thanks for your help _/|\_
 
 

You can make up values for S21, S12 and S22 that will transform your 1-port S11 data into 2-port. You can also terminate Port 2 with the system Z and only use Port 1. 
 

Ok thank you for the tips

1 - 7 з 7