Post Layout simulation accuracy

For very low DC current levels, your simulation results may be affected by parameter "gmin" - the default is (I think) 1e-12 S (or 1e12 Ohm - i.e. 1pA for 1V voltage).

"gmin" is a resistor (conductance) that SPICE simulators connect between every node and the ground (to avoid nasty floating node problems, to have a deterministic and converging solution).

Just set it to a different value - e.g. 1e-18 - and check if you a difference in your simulation results.

Maxim

Thanks for replying Maxim. I did it but still, I see the unexpected output after extraction. I have also changed the iabstol to 1-15 ( it doesn't converge for lower iabstol). So in terms of accuracy, if I use these low Gmin and iabstol values, the accuracy of the results should be fine, right? Is there any other parameter that I should be aware of for a circuit with very low current inputs? As for my findings, the mom caps after extraction cause the problem. So now I need to be sure I have the simulation setup and parameters completely right.

Thanks

Thanks for replying Maxim. I did it but still, I see the unexpected output after extraction. I have also changed the iabstol to 1-15 ( it doesn't converge for lower iabstol). So in terms of accuracy, if I use these low Gmin and iabstol values, the accuracy of the results should be fine, right? Is there any other parameter that I should be aware of for a circuit with very low current inputs? As for my findings, the mom caps after extraction cause the problem. So now I need to be sure I have the simulation setup and parameters completely right.

Thanks

Dear Fatima65,

Fatima65 said:

f I use these low Gmin and iabstol values, the accuracy of the results should be fine, right? Is there any other parameter that I should be aware of for a circuit with very low current inputs? As for my findings, the mom caps after extraction cause the problem. So now I need to be sure I have the simulation setup and parameters completely right.

A few comments if I may....

1. Are you sure your models support this level of accuracy? I would be very surprised i your PDK vendor guarantees a fA level of current accuracy. At the fA level, the presence of even ambient light will impact the currents and I can't imagine how the vendor could qualify any level of accuracy to this degree.  Have you inqured?

2. You might examine the limits of SPICE accuracy in terms of its parameters at URL:

https://www.google.com/url?sa=t&rct=j&q=&esrc=s&source=web&cd=&ved=2ahUKEwjP8aTkj_rxAhXLFVkFHU58B60QFjAGegQIDxAD&url=https%3A%2F%2Fdesigners-guide.org%2Fanalysis%2Fdg-spice%2FchA.pdf&usg=AOvVaw2r19Ksg3wDbO2TO5zaXaTP

(section of Ken Kundert's book)

Section A.2.1.1 speaks tp iabstol and its limits for a desired accuracy.

3. One approach might be to run your simulation at a much higher temperature to determine if your currents are showing signficant increases, I assume the relationship with temperature is exponential.

Shawn

You do not provide enough information to help you debug the problem.

What is "unexpected output"?

Is this DC or transient or AC problem?

"MOM caps after extraction" causing the problem - What's wrong with MOM caps after extraction?

Do you have capacitance double-counting (SPICE elements and parasitics)?

Do you extract them as "device" or as "parasitics", or both?

Hi Maxim,

Thanks for the reply and sorry for the incomplete info. I am running transient simulations (it is a very low-speed circuit) and by unexpected output I mean the output is not periodic after extraction. Recently I discovered that it only happens when I use the APS simulation option though. With normal spectre (conservative)  the results are fine. I have changed the Gmin and iabstol, so could that be the reason why the APS doesn't return the same results as spectre? I am pretty sure I am extracting caps correctly.

Thanks,

Fatima

Dear Fatima,

The difference between spectre  APS (spectre +aps) and spectre is a known issue and to be expected. For most circuits, the difference in the two simulator's accuracy is quite small. However, spectre (without its +aps option) is considered the " golden standard". Spectre ++aps shows provides less accuracy than both spectre and spectre +aps.

There is a document entitled "Optimizing Spectre APS Performance" on the Cadence On-line support portal that describes the  differences between the three simulators and the trade offs each allow.

I hope this was useful to you Fatima!

Shawn

One example of such a difference is the default value for rabsshort, which is 0 in Spectre and 0.001 in APS, see https://support.cadence.com/apex/ArticleAttachmentPortal?id=a1Od0000000nX06EAE. Another difference is the default value for rcut (see the output of 'spectre -h options').