HELP - need to make TINA NETLIST/MACRO for VTL5C3 "Vactrol"

[CharlieLaub]

I am doing some circuit modeling using TINA-TI. I designing a type of limiter and would like to use a VTL5C3 "Vactrol" Light Dependent Resistor (LDR) as a variable resistor element in the circuit. This particular one has the right attack and decay characteristics for my application.

I have been able to create a regression of the resistance versus current curve for the VTL5C3 using the datasheet plot data. I would now like to be able to model this component in TINA-TI.

Can anyone help me create a .cir file that I can import? I am very new at this, so I don't have any experience creating these sorts of SPICE models. Any help would really be appreciated.

Thanks,

Charlie

[Ouroboros]

The full (paid for) version of TINA has many more functions than the free version from TI. One of the functions is the "Controlled Source Wizard" which allows you to define non-linear voltage or current controlled sources. This would seem to be a way to define the non-linear transfer function of your LDR.

[CharlieLaub]

OK, I found a model for the VTL5C2, which is pretty similar to the VTL5C3. It's a start. But the model is for LTSpice, which I have never used. I downloaded and installed it last night and loaded up the file. Here's what I see:



When I ran the simulation, I got this:


As far as I can tell, this is showing the resistance (as voltage V2 divided by current, I2=1 amp) at the LDR's "R" terminals when current is supplied to the "LED" terminals (I1) with the values shown on the x-axis. This just doesn't seem to be right - the model file has a table with resistance values (and the datasheet also has a plot) and for 1mA the resistance should be around 7.2k ohms!

Can any one give me some advice on this, about what I might be doing "wrong"? This is the first thing I have ever done in LTSpice.

If I can be confident that this test model is working for the LDR, I will just rebuild my circuit in LTSpice, since it's not super complicated.

Any help would be appreciated! Thanks,

-Charlie

[Ouroboros]

Are you wanting to drive a constant current through the LDR, and then measure the voltage acoss it? In which case you would need to add a differential voltage probe across the LDR in your schematic and perform a dc analysis with a constant I2 as you varied I1.

By the way. It should be a simple matter to edit the LT Spice model to work with TINA. I did this only a few weeks ago with the LT1016 high-speed comparator without any problems.

[Ouroboros]

It looks from your plot as if you were plotting V across the LDR as you changed I2, rather than I1.

[CharlieLaub]

Originally Posted by Ouroboros

It looks from your plot as if you were plotting V across the LDR as you changed I2, rather than I1.

OK, I'm no LTSpice expert, or really have much of a clue, but I believe that the statement:

.dc dec I1 74uA 40mA 100

is performing a DC sweep of I1 from 74uA to 40mA. I1 is the input to the LDR's LED (see schematic in first plot).

I believe that the plot is showing the Voltage at node 2 divided by the current at node 2 (I2) which is fixed at 1A. This should give the resistance in the loop where I2 is flowing, namely the LDR's resistance cell resistance, R.

Is that not correct?

-Charlie

[Ouroboros]

To be honest i'm not sure as I also have only used LT Spice a few times, as I have the full-spec version of TINA at work. LT spice although extremely powerful is Byzantine in its complexity!
I was fooled by the title of your plot which is V(n002)/I(I2), but of course that is the resulting resistance that you were measuring.
Can you point me to the LT-Spice model for the part you are using? I'll load it into TINA and see what it gives.

[CharlieLaub]

Originally Posted by Ouroboros

To be honest i'm not sure as I also have only used LT Spice a few times, as I have the full-spec version of TINA at work. LT spice although extremely powerful is Byzantine in its complexity!
I was fooled by the title of your plot which is V(n002)/I(I2), but of course that is the resulting resistance that you were measuring.
Can you point me to the LT-Spice model for the part you are using? I'll load it into TINA and see what it gives.

I sent you a PM, but am also including below a link to Gootee's LTSpice model. If there is any chance that it could be adapted to TINA-TI or TINA that would be awesome!
Spice Component and Circuit Modeling and Simulation

-Charlie

[pweaudiotech]

Here is the SPICE Subcircuit for a Light Dependent Resistor.
+ (1) is the LED Anode, - (2) is the LED Cathode, R (3) and R (4) are the Resistor Terminals

*NSL32 (LDR) Light Dependent Resistor SPICE Subcircuit
*****connections:+ - R R
.SUBCKT NSL32LDR 1 2 3 4
bled 1 5 i=exp(v(1,2)*24.154-46.803)
vid 5 2 0
blogivd 6 0 v=ln(i(vid))
rhlog 6 0 1
bcell 3 4 i=v(3,4)*(exp(v(6)*(-0.092947*v(6)-0.54364)-4.6619))
.ENDS

[Ouroboros]

Hi pweaudiotech.
I've been doing some work with the original poster on this. The dc characteristics of the Vactrol are now well modelled and can be altered to match different types of the device. The outstanding issue is how to match the dynamic switching characteristics. The photo-conductive material used in the part has very different response times for increasing illumination and for decreasing illumination. Also the time-constant in both directions is also affected by the level of the illumination around which the change is happening (ie, the dc LED bias current). So there are non-linearities in the dc and the time domains.
If the part is being used in an analogue agc circuit or in a retro-style analogue effect pedal, then the dynamic considerations are likely to be important.