Transient and DC operating point are different

The transient and DC operating points will be the same if the DC value of the sources is the same as the time zero value of the source. That appears to be the case here.

However, do note that the dc solution for transient will start from the values at the end of the previous simulation - and so that would be the value of x=1.8 (because of the dc sweep). If the circuit has more than one stable operating point, then that could influence the result.

However, in this case I don't know what you're looking at to determine that they are different. I checked the node voltages and currents and they all seem to be the same (comparing the spectre.ic and spectre.dc files). 

What are you looking at which shows you there's a difference?

Regards,

Andrew.

Thank you.

As you said last time I also checked the DC sources value and time-zero value and they are equal.

I've just checked operating points from two files as you said. However, in my case, these files don't have current info. 

What I see the difference is currents through M0 and M1 in two cases.

DC analysis: iM0 = iM1 = 800.026uA

Tran analysis: iM0=800.002uA and iM1=799.999uA

I got this by running each analysis separately and then from ADE print operating points.

I think you're looking at the tranOp results not the time=0 operating point information. The tranOp results are coming from the:

finalTimeOP info what=oppoint where=rawfile

which is the operating point at the end of the simulation, not the beginning. I can't print the operating points in ADE because I don't have the setup, but if I look in the results browser, then I see "tranOp" (which is the aliased name for the finalTimeOP results) and "tranOpTimed" which is the aliased name for the "infotimes" output. It's the latter you want. 

In that, the results all 800.026uA (assuming you're looking at the id operating point parameter for these devices).

A small difference might have been possible (the difference you're seeing is smaller than the reltol in the simulator anyway), but I think it's actually just because you're not comparing the right things.

Andrew.

I tried to check the voltage at two inputs to see if the operating point is beginning or final point and the result confirms that it is beginning point (if nothing goes wrong).

However, in transient analysis, I tried to set infoitimes box with 0 but the result in result browser doesn't have any infor about oppoint at this time.

Is there something wrong with my case? 

I have struggled with it all night now. I need some sleep now. Thank you again for help.

Hi again,

I tried to set reltol = 1e-8 but the resulting current in tran analysis is still not the same: iM0=800.001uA and iM1=799.999uA.

Also, I tried to choose stop time equal to an even number of cycle so that the final point and beginning point are the same with both two input starting at the same value).

However, the result is not different.

How can I save the operating point at time 0 in transient analysis? I tried to put 0 into infotimes box but that doesn't work.

I can't remember which IC version you're using, but I ran the simulation using MMSIM13.1 Update - which is 13.1.1.049. I then used the IC616 base release (I think it was an early IC616 ISR you were using). I found in that release, the infotimes output is in a result called "tran_info" and I can't plot the waveform (it is a single point waveform) but I can send the results to a table. 

I also wrote this short OCEAN script to get the results:

openResults("forum_oppoint.raw")
;println(results())
;println(results(?noAlias t))
selectResult("dcOpInfo")
printf("M0:id = %g M1:id = %g\n" getData("M0:id") getData("M1:id"))
selectResult("tran_info-tran_info")
printf("M0:id = %g M1:id = %g\n" value(getData("M0:id") 0) value(getData("M1:id") 0))

Note I used the "unaliased" result name to ensure it worked in all versions (normally results() and ViVA results browser show the aliased result name to make it more portable and shorter).

Anyway, you can see the results from sending the infotimes (time 0 operating point) to a table, and also the results of the OCEAN script in this screen grab. As you can see, the dcOpInfo and tran_info-tran_info results match:

By the way, I wouldn't set the reltol that tight - that's excessive.

Not sure why you stayed up all night to sort this out - do you not trust the simulator?

Regards,

Andrew.

Hi,

Thank you.

I have just checked it the way you did and the result is same now. However, there are two questions, could you explain?

1. The operating point at time 0: iM0 and iM1 are not the same at the one I had by running transient and plot iM0 and iM1 and then see the current at time 0 of the two curves. They are actually very closed to each other (2pA difference) but should they be exact the same?

2. The final operating point also differs from that got from plotting iM0 and iM1 and then see the current at time stop time of the two curves.

Is this normal?

Not sure why you stayed up all night to sort this out - do you not trust the simulator?

Honestly I would like to see it works at least one time myself.

Unknown said:

They are actually very closed to each other (2pA difference) but should they be exact the same?

You're really worried about 1 part in 40 million? Circuit simulators solve nonlinear differential equations. It's not possible to get an exact solution to such equations, so numerical methods are employed (e.g. Newton Raphson) which iterate towards a solution and determine that the solution has converged when the error is small (this is all part of a tradeoff between speed and reasonable accuracy). The criteria used to determine the error is generally in the form reltol*quantity+abstol (so this might be the change between two iterations, or the error in the sum of currents into a node).  reltol defaults to 1e-3, and vabstol is 1e-6V and iabstol is 1e-12A. The absolute tolerances are for when the signal levels are close to zero - because otherwise you'd have an ever increasing accuracy for tiny (insignificant) signals. So a difference of only 2pA is remarkably small (it's close to the abstol), especially in a current of 800uA. I didn't actually see that difference. Even if I had, the starting point for the two DC solutions may have been slightly different (it typically starts from whatever set of numbers were used previously - or it may have been that there was a small difference in the number of iterations - either way, the differences are well within the accuracy tolerances).

There is a small amount of inaccuracy that appears in the DC solution with reltol=1e-3, which reduces if you tighten it to 1e-5 (note, I seriously doubt you need this level of accuracy for this circuit) - and if you compare the three operating points, they are very close:

DC : M0:id = 0.00079999999976654 M1:id = 0.00079999999976654
TRAN 0: M0:id = 0.00079999999976654 M1:id = 0.00079999999976654
FINAL : M0:id = 0.00080000135675758 M1:id = 0.00079999851611377

This was with this script:

openResults("forum_oppoint.raw")
;println(results())
;println(results(?noAlias t))
selectResult("dcOpInfo")
printf("DC : M0:id = %.14g M1:id = %.14g\n" getData("M0:id") getData("M1:id"))
selectResult("tran_info-tran_info")
printf("TRAN 0: M0:id = %.14g M1:id = %.14g\n" value(getData("M0:id") 0) value(getData("M1:id") 0))
selectResult("finalTimeOP-info")
printf("FINAL : M0:id = %.14g M1:id = %.14g\n" getData("M0:id") getData("M1:id"))

Note I did this with MMSIM14.1 ISR18 so your results may be slightly different (although not significantly different). All the results there are well within the tolerances. There's probably some longer term settling effect - I found this reduced if I ran a much longer simulation with a lower frequency sine wave too. There's also some error that occurs (local truncation error) during transient which also will give a small error in each instantaneous time point, but this won't accumulate over time.

So I would say you're worrying about a level of accuracy that really isn't warranted.

Regards,

Andrew.

Hi,

Actually, I don't need that accuracy just to confirm my understanding about the two analyses. I thought that in transient analysis the zero time and stop time points of current should be equal to the transient operating points of current at time 0 and stop time respectively. However, that is not the case in my simulation.

As you can see the transient operating point for id at the time zero:

DC : M0:id =800.000003e-6  M1:id = 800.000003e-6

TRAN 0: M0:id = 800.000003e-6 M1:id = 800.000003e-6

However, when I run the transient analysis, then plot id and look at the id at time zero I got the result is a bit different:

TRAN 0: M0:id = 800.000005e-6 M1:id = 800.000005e-6

I thought they should be the same. I just want to confirm my understanding about the analysis. In this case the difference is insignificant. However, is there a case where the difference is large (beyond the tolerances )?

Unknown said:

I thought they should be the same. I just want to confirm my understanding about the analysis. In this case the difference is insignificant. However, is there a case where the difference is large (beyond the tolerances )?

No, not unless there is some circuit behaviour (such as something that hasn't settled in the duration of the simulation, or some adaptive non-periodic behaviour like a sigma-delta modulator) which means the beginning doesn't match the end. 

Andrew.