INA333 operating point not found error message

Are we missing a parametre adjustment at all?

The below was created uses only the default TINA-TI settings.

Attaching screen shot:

From Page 15 of the INA333 Datasheet.

Could you post the .TSC file?  

Here is the TCS file that gave the error.   I can send the other TSC file that did work when the amps were not together, if that helps.

Dan

Here is the file with the amps separate. In this circuit, things behave properly.  

Dan

Hi Daniel.

The OPA333 and INA333 simulation models are very complex and individually they converge well, but together it sometimes a struggle for the simulators. We are looking at what can be done to resolve the problem longterm.

I found that I can get the troubled circuit to readily simulate by changing the shunt conductance parameter from the default 1p, to 10p. Here is how you accomplish this:

Select the Analysis tab, then Set Analysis Parameters. Scroll down the parameter list until you find Shunt conductance. You may have to open the extended list of parameters by clicking on the hand symbol. Over type the 1p number with 10p and close Analysis tab.

I hope this helps.

Regards, Thomas

PA - Linear Applications Engineering

Thank you for your help.   I did make the change, and the circuit did converge quickly, with expected values.   I really appreciate the help!

But I do want to clarify one thing.

Afrer opening up set analysis parameters, I changed the value the value for GMIN (minimum conductance) from 1p to 10p.  Futher down in the parameters there was another shunt conductance line, it value was 0. ( It was next to shunt capacitance, which was also 0.)  I left that one alone.  Or should this one be changed as well  I just wanted to make sure I changed the correct one so that as the circuit complexity grows I do not run into other issues.  

I attached a file that contains the analysis parameters.  Everything is the default value except for the change listed above.  Does this set of parameters seem correct?

Thanks again,

Dan

Hi Daniel,

PSpice simulators do not always behave as we think they should; especially, when it comes to convergence. Unfortunately, I sometimes have to make a best guess parameter setting and apply trial-and-error until things work. We have learned that reducing shunt conductances sometimes brings about convergence in circuits that exhibit such issues. My thought is that it helps reference the internal nodes to some other point via the conductance path during simulation start-up. Changing from 1pS to 10pS still keeps the numbers in the picos so the conductances are still extremely tiny after the change. The OPA333 has a very long netlist because of the model's extensive detail and huge arrays must be solved during a simulation using that model. The INA333 netlist is 3X+ the length of the OPA333 so when you put them together it is a huge task for the simulator to achieve convergence.

Tina's help guide defines the two conductances as follows:

GMIN  - Defines the minimum conductance connected in parallel to a pn junction.

Shunt conductance  - The conductance specified here is added from each node to the ground. The default value is zero.  Specifying 1p or similar value might solve some convergence problems.

I have tried both of these and find one, the other, or both may help. I tried the GMIN parameter first and it worked well. I didn't even try the Shunt conductance parameter this time. I have had mixed success with it in the past.

Regards, Thomas

PA - Linear Applications Engineering

I really appreciate your help and guidance.  Your suggested changes with the GMIN at 10p allowed me to make some progress with this design.  Yet I have run into another covergence issue as the circuit complexity grew.  I tried some of the things you mentioned, with no success. I was hoping you could take another look. I have atached the present TSC  file where I am now stuck again.  But I thought I would explain the steps I took to get where I am at today.

After your 10p GMIN suggestion, as was able to grow the circuit in steps with good success. As a reminder, I am trying to implement the cicuit in the INA333 data sheet (figure 37) but with one additional gain stage at the output. The INA333 (U1)  driving a OPA333 (U2) , followed by another OPA333(U3) worked well. DC and AC results are as expected.

Then I added the OPA333 (u4) that feeds the  INA333 ref input. I used the values from figure 37 of the INA333 data sheet.  Initially it did not converge.  Then I added a 1.4V/1meg source to the output of u4, thinking there may be a floating node issue.  The circuit did converge, but DC values were not good, most amps were driven to the 2.8 volt rail.  I tried many things, I documented each step on the schematic.  I then changed some of the analysis parameters. Gmin to 20P, no help. Then shunt conductance to 20P, no help.  I put things back to default, but kept GMIN at 10P as your suggested.

One thing I do find that is interesting: VG1 is a signal source with a DC offset.  The ac value is 10 HZ or 50 Hz, 0.5 mV amplitude.  The DC value is nromally 1.4 volts.  With these inputs it will not converge (U1-D17 typically).  If I change the DC value to 1.4005 (introducing a 0.5mV dc offset) the circuit will converge, but DC values are not as expected, driven to rails.  Does this small DC offset point that affects convergence point to anything?

Anyway, I was hoping you could take a look and offer any suggestions.  As I said before, I really do appreciate your help.  I really want to exercise the circuit shown in the data sheet.

Thanks,

dan

Hi Daniel,

Thank you for your very detailed report regarding the steps you have taken to troubleshoot the INA333/ OPA333 ECG application circuit. it is very helpful in understanding the convergence problem.

I spent much time this afternoon working on the convergence issue and it does not appear to be related to the conductance settings which helped much up to this point. Indeed the problem occurs when the integrator is added into the circuit. Integrators can exhibit convergence problems on their own without being connected to other circuits. I did try a web search idea to set the integrator output at a specific level use node sets and that did not help.

Certain that the problem was related to the integrator stage I substituted another low voltage CMOS operational amplifier model (OPA340) for the OPA333. It has a good, but simpler simulation model. The circuit would not converge with the OPA340. I then replaced the OPA340 with a simple Boyle model used for one of our TLV CMOS amplifiers. Again the circuit would not converge. Finally, I used TINA's ideal operational amplifier model (under the semiconductors tab) for the integrator amplifier and the circuit converged. I suspect it is the added complexity of the operational amplifier circuit in this path that is proving so difficult for TINA to achieve convergence. I've attached my TINA circuit containing the ideal operational amplifier as the integrator.

When I had tried simulating this same circuit in the past with another PSpice simulator it would not achieve convergence either. Therefore, the convergence issue is not unique to TINA Spice. A quick web search on PSpice convergence issues brings up many and some resources provide suggestions. Also, there may be some parameters settings that would help achieve convergence but that would require more evaluation.

I will continue to research the integrator circuit convergence. If I find some helpful solutions I will be sure to let you know.

Regards, Thomas

PA - Linear Applications Engineering   

Hi Daniel,

Here's the INA333/OPA333 ECG TINA circuit.

Thomas

Thanks for you prompt response and continued support of this issue.   I will take a look at the circuit your provided.   I did have some additional success / issues  after I posted yesterday. I was going to send you another  update, your quick response beat me too it!  We have also tried Hspcie and Pspice, both have similair issues, either no convergence or convergence with shifted DC values.   I thought I would share the following since I can get one case where the circuit will converge, using the OPA333 inetegrator and I get expected DC and AC results.   But as you will see, it is very touchy - which is disturbing.  I talked to a few other here and obtained some other input. Here is a summary what I did.  The detailed steps are on the schematic. 

I took the circuit called ecg-step-5 and made a new version called ecg-step-5x.  The TSC file is attached. In the analysis parameters I changes GMIN to 100p, shunt conductance to 10p, I changed the four DC error terms from 1 to all 10's.  You can see I have a OPA333 integrator in the loop going back to the the INA333.  I removed the floating node voltage source / 1 meg resistor from the output of U4.  In this case the  circuit will converge, but only when there is a +0.5mV dc offset added to the neg input of the INA333.  I set the DC value of the VG1 source to 1.4005, The AC value is 0.0005V.  The good thing is that it converges, the DC offset is corrected by the integrator and I get the desired AC at the ouput. (Just so you know at this point I was going to stop and have a "happy beer", but I made the mistake of trying a few more things.... )

I tried several other changes to the VG1 DC values, which led to convergence issues.  In summary there are two distrubing issues.

1. If the INA332 neg input is at 1.4005 the circuit converges.  Note that the other (pos) input is fixed at 1.4 V by VS3.  If I put VG1 at 1.4000 so the inputs are balanced, it does not converge. If Iower VG1 to 1.3995 (a 0.5 mV shift the other way), it will not converge.  If I put VG1 to 1.4 and change the other postive input input to 1.3995 volts (causing a 0.5 mV shift/ the other way) it will also not converge.  I also thought that since I am using a single supply that some of the resistors to ground may be pulling thing slightly, I added the 1 meg pull up to the output of the INA333, still no converge.I changes thing back to where it would converge.

2. In another test case, when I got the circuit to converge (VG1 at 1.4005) I tried the following.  I removed R10, a 1 meg to ground at the output of u2.  The circuit would not converge, and the operating point not found was on U4,d17 (integrator).  The minimal change in the load on u2 (1 meg removal causes about a 1 uA reduction) should in no way affect the intergator loop. The u2 path is separate, with no feedback.  This is really strange.

Anyway, I am posting the circuit that converges, then you can try the simple changes (for example slight change in DC offset) to see is you get the no-converge.

Is there any plans to look into these INA/OPA models further?  We really want to use these parts, but are concerned with the modeling difficulties for relatively simple circuits.

Any additional thought are welcome.

Thanks again,

Dan 

Hello Daniel,

Thank you for the interesting information that you provided regarding your progress with the INA333/OPA333 ECG circuit convergence. It is always an unsettling result when a small, intentional voltage change results in the difference between convergence and non-convergence. It is akin to straddling the razor's edge. This is a more common situation than one might want to believe, but a reality when highly complex simulation models are involved in the simulation circuit. Convergence issues are the #1 headache encountered by users simulating circuits. This is something simulation software companies spend much time attempting to improve upon. Quite often, when a newer revision of one's software becomes available, it is because they have tweaked their convergence algorithms to improve the likelihood of circuit convergence.

We have been having discussions about the INA333/OPA333 ECG circuit and what can be done, if anything to the models, to help bring about easier convergence. The OPA333 and INA333 models are very sophisticated as mentioned previously and I don't want to do anything that would lessen their ability to accurately behave in simulation as the actual product does in circuit. The discussions have resulted in plans that I'll be moving forward with. This is not a simple matter to resolve so it will require time and effort before we will be able to accurately assess our success with the project.

Best regards, Thomas

PA - Linear Applications Engineering