For example. All three of the opamp outputs are connected together with label "vadc-". Is that what you want?

Vadc- is essentially the real ground of the future ADC that will receive the isolated signal in my application. Since the output are connected through a high impedance individual resistor, I don't see any problem with it, It's like having multiple channels connected to a multichannel ADC. The name "Out" in the OpAmp is just part of the model Symbol, not a Label Net

 

I have actually physically built and produced a circuit utilizing the Broadcom HCNR201, which is an identical device, for the exact same application, high performance isolated voltage sensing.

I used the circuit in figure 15B, which works extremely well but requires two optocouplers.

You could try the circuit in figure 15A, which requires a single optocoupler, but the isolated current sources need to be tightly matched and to track across the temperature range. Easier said than done.

But if you are only simulating it, you could give it a try.

Thanks for sharing this other option. I'll consider it in my circuit as well. I'd like to use this kind of opto for the instrumentation of a current controlled power converter that operates through a DSP. The DSP module has its own ADC but it requires isolation since the device and the input of the converter surely will have different potentials

 

hi GP7,
Try this option, C2 A2 reversed, also the -5v supply is set to 0V.
E
View attachment 361299

Hey ericgibbs,
Thank you guiding me, I have simulated the circuit and it is working in both TINA and LTSpice. One thing I'm noticing is that when I use 100E resistor in series with A from 5V supply (V2), the simulation is working perfectly fine but when I change the value to 1k I'm not getting the output. Maybe there seems to be a problem with my model.

Thanks a lot

 

when I change the value to 1k I'm not getting the output

Likely that's limiting the current to the opo and the op amp is saturating.

 

Likely that's limiting the current to the opo and the op amp is saturating.

Hey crutschow,
Yeah, maybe that is limiting the current to the optocouoler. Thank you so much.

 

One thing I find worth of noticing is the input current of the inverting pin of the OpAmp. When it becomes too big, the feedback effect of the P1 diode doesn't work propperly and the output signal becomes too asmall or DC. I don't know if the problem was in the OpAmp iteslf or in the SPICE model I downloaded (I'll work on that later), but when I chosed a new OpAmp with a new model, the circuit worked as intended

 

I don't know if the problem was in the OpAmp iteslf or in the SPICE model

You need to look at the maximum output current rating of the op amp (which drives the opto LED input), and make sure it's not being exceeded.
If so, you may need to add a BJT buffer at the op amp output.

 

You need to look at the maximum output current rating of the op amp (which drives the opto LED input), and make sure it's not being exceeded.
If so, you may need to add a BJT buffer at the op amp output.

The output current of the OpAmp swings around 5.4 mA for TL082 and 3.4 mA for the LM2902. I was a little confused by the way the information is presented on both datasheets, but the TI webpage says the typical output current of the TL082 is 10 mA. It doesn't seem like the problem is there. But when you look at the input current, the LM2902 swings between 4 and 10 nA while the TL082 swings between 20 an 26 uA, the same order of magnitude of the feedback photodiode current.

 

when you look at the input current, the LM2902 swings between 4 and 10 nA while the TL082 swings between 20 an 26 uA, the same order of magnitude of the feedback photodiode current.

Yes.
The input current has to equal the photodiode current, otherwise the op amp wouldn't be in its linear, stable state (essentially no voltage difference between the + and - inputs).

 

Hi,

I'm trying to build a circuit using an IL300 optocoupler. My application is to read an input voltage in the range of 0V to 2V. I followed the IL300 application guide and built my circuit according to the photovoltaic configuration (as suggested in the app note).

I'm simulating the circuit in TINA, but when I run the simulation, the output is always 5V regardless of the input voltage. I'm using OPA2328 op-amps on both the input and output sides of the IL300. I downloaded the IL300 SPICE model from the manufacturer's website.

I’m not sure how to solve this problem. Could you please suggest solutions or point out where I might be making a mistake? I’ve attached my schematic and the IL300 SPICE model for reference.

Thanks & Regards

Hi
Please share your design scratch pad - how did you determine R1 & R2?

 

Hi
Please share your design scratch pad - how did you determine R1 & R2?

Hey,

If you refer to the IL300 app note, as per the Figure 8 circuit, I have considered K1 to be around 0.006 (worst case). I have considered an output current of 15 mA. Solving for IP1 with these inputs, IP1 will be 90 µA. Solving for R1 = Vin/IP1 (in my case, Vin is 2 V), R1 = 22.1 kΩ. R1 = R2 since I'm considering G = 1.