OPA1652: Comparison of OPA1652 and LF353

Hi Marzi,

Yes the OPA1652 should be a better fit considering the CMRR spec is a typical of 110 dB. Also the input bias current is a typical of 10pA on the OPA1652 vs 50pA on the LF353. This improvement of Ib will help with reduce the voltage noise created by ib times source impedance. The OPA1652 also has better input voltage and current noise. Given the CMRR specification improvement alone I believe this will a noticeable improvement. 

I hope this information is useful. Let me know if I can be of further assistance or expand further on the topic. 

Best Regards, 

Chris Featherstone

Thanks Chris. What about GBW - gain bandwidth product? It seems like OPA1652 has  a GBW of 18 Mhz whereas LF353 has 4 Mhz. Does not this mean it will be less stable?

Thanks Art. I will calculate my phase margin with both of the op-amps then.

Are tina models for both correct in terms of bandwidth and phase shift?

Hi Marzieh, 

Yes the simulation looks correct. I was able to replicate Figure 5 from the product datasheet below. 

sbom737c.TSC

Best Regards, 

Chris Featherstone

I measured the input to output gain in our hardware setup with the two different op-amps with CM and DM voltage. 

Red: DM input with OPA4172

Purple: CM input with OPA4172

Purple: DM with 1652

Red: DM input with 1652

So it seems like 1652 has unwanted zero, pole pair. Is this correct?

Hello, 

Can you share your circuit that was used to make the above measurements? Are you able to replicate the behavior shown below to match our measurements?

Best Regards, 

Chris Featherstone

Do I need to build a circuit like this? I have a Ridely box and I can measure loop gain, etc...

Hello, 

Is your goal to measure open loop gain Aol or closed loop gain Acl?

Best Regards, 

Chris Featherstone

I want to measure closed loop gain on my circuit. I guess your circuit is for open loop?

Hi Marzieh, 

Yes the simulation circuit is for open loop gain or Aol. This simulation circuit isolates Aol and feedback network beta. The large cap and inductor are used as a simulation trick to perform the analysis. To measure Acl or closed loop gain you would just apply your network analyzer to the input of your circuit and measure the gain vs frequency. 

Best Regards, 

Chris Featherstone

so simulation needs the closed loop DC feedback to do the AC analysis but implementation does not need it. Right?

Should I use the 10 pF on the output or leave it open?

Hi Marzieh, 

There are two methods for analyzing the Acl or closed loop gain in simulation. The easiest way is to run the simulation as shown below in case 1. I attached the ACL closed loop simulation for convenience. You may modify as needed. I removed the output components. They are not needed unless they are in the actual circuit. The load capacitor of 10pF came from our reference design and is not needed. The implementation for measuring your circuits closed loop gain is similar to method 1. For analysis in Tina either method 1 or 2 can be used. 

1) Simulating closed loop gain Acl:

Tina simulation for closed loop gain Acl:

ACL Closed Loop Gain.TSC

2) Breaking the loop method for stability analysis

In simulation we break the loop with the 1TF cap and 1TH inductor as a trick to isolate the parameters Aol, 1/beta and the loop gain Aol*beta where beta is the feedback network. We can use the post processing equations to write other functions such as Acl. For example I have created Acl below. When breaking the loop with the cap and inductor method the output measurement is Vout = Aol*beta. The post processing equation option is shown circled in red below. For a more detailed training on breaking the loop and tina analysis you may watch our video training series here:

https://www.ti.com/video/series/precision-labs.html

Tina Simulation for breaking the loop:

Breaking the Loop.TSC

Best Regards, 
Chris Featherstone

Thanks Chris.

Did you import the macro or used the one that is already in TINA? 

The content shows empty when I choose the component from the list.

Hi Marzieh, 

I downloaded the reference design from the product page and modified it. You can download my simulation that is in the last post I made and modify my circuit or copy the model from my simulation and paste it into yours by selecting the op amp in the schematic and copy paste it.

Best Regards,

Chris Featherstone