• Not Answered

INA333 operating point not found error message

Hi, I an using a tina-TI version 9 and trying to do a simulation on a circuit using the INA333 and OPA333. I downloaded the the spice models form the TI site.  I am trying to create a portion of a ECG circuit that is shown in the data sheet for the INA333, figure 37.   When I set up my first simulation using the ina333 and opa333 separately, things behaved as expected.  This was with separate voltage sources on each input. The DC analysis works fine, with both balanced inputs and when I introduced a DC differential on the inputs, the difference times the gain gave me the expected output.  INA333 gain was 10m opa333 gain was 100

 

Then I connected the output of the INA333 to the input of the opa333, hoping for a total gain of 1000.   When I perfrom the DC analysis, I get an error message:operating point not found, U1,D17.   I am using the default TINA-TI parameters. 

For a simple circuit like this, I thought the sumulation should be straightforward.  Am I overlooking something simple?

Dan

 

 

 

The INA333 output is connected

12 Replies

  • 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.

  • In reply to Larissa Swanland:

    Could you post the .TSC file?  

     

  • In reply to Dave Weinzierl:

    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

    ecg-step-1.TSC
  • In reply to Daniel Schwab:

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

    Dan

     

    ecg-step-0.TSC
  • In reply to Daniel Schwab:

    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

     

     

  • In reply to Thomas Kuehl:

    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

     

  • In reply to Daniel Schwab:

    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

  • In reply to Thomas Kuehl:

    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

    ecg-step-5.TSC
  • In reply to Daniel Schwab:

    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