"Weird" result in MOSFET Capacitance calculation

[Sant0z]

Hi everyone,

I have a problem with the simulation result for calculating N-CH Mosfet capacitance (Cgs, Cgd, and Cdb).  

In this simulation I tried to verify my manual calculation with the Spice result using Multsim 11.0. But, the result in Multism simulation is quit different either from the manual calculation or from Pspice/Hspice simulation.

Manual Calculation:

Multisim Simulation:

Setting Parameters in Multisim:

.DC from Multisim

>DC from PSPICE

From those results, it seems that Pspice gave a close value to the theoretical MOSFET calculation here.  And I got messy result in Multisim.

Can somebody help me solving this problem?..is Multisim not as powerful as other spice software? or I just messed up with the parameters setting form Multisim and ended with the wrong answer?

[OStep]

Sant0z,

We'll investigate and get back to you. Thanks for the detailed report.

[OStep]

Sant0z,

We investigated and found a problem with the reported capacitance values. However this is only a problem with the report - the actual internal capacitance values applied in dynamic analyses (AC and Transient) are different from those reported. For your bias conditions, the internal values are practically identical to the values you cite. We will rectify this problem in the next major release.

Thanks for the report and sorry for the inconvenience.

[Sant0z]

Hi, Max

Thanks for replaying my question. But, I still don’t get it. Your answer looks like in between.  

Is the problem caused by user error? or it is a software error

If it is just a user error, you can point out which error that the user made in that simulation.

But, if it is caused by software error, you can explain that there is an error/bug in Multisim, so I can start using other simulator.

Thanks.

[OStep]

sorry if I was not clear - it is a software error at the reporting stage only. Note that the values calculated internally (not the ones reported) are still correct. So for example, if you run AC analysis (which requires capacitance values at the DC operating point), Multisim will use the correct capacitance values for the actual analysis.

[Sant0z]

I tried to run AC analysis, but capacitance values for Cgs, Cgd, and Cdb are same with the result from .DC analysis.

And a result form Zero Poles analysis also ended up with wrong value, because PZ depends on the value of the CMOS Capacitance.

What I found from that result are:

1. Multisim doesn't calculate Extrinsic Capacitance (Overlap Cap) and calculates Intrinsic Cap only.

2. The default value of Eox (Silicon Oxide permittivity) in Multisim is 1.75fF/um.sqr instead of  3.45fF/um.sqr

If any mistakes occur in my analysis, please let me know.

Thanks

[OStep · Accepted solution]

I believe you are still accessing the device capacitances output variables. Those would be only the reported capacitances and the same as in DC - incorrect. We checked the code and the actual capacitances used for analysis are the correct ones.

To demonstrate this, by using actual circuit variables - voltage and current, I calculated the impedance looking into the gate for a 1Ghz range (Its a bit non-trivial to demonstrate the impedance of specific capacitances because you cannot easily pull out the current of the capacitance). The results are identical to PSpice.

So to reiterate- the actual circuit analysis results will not be affected. For now, we ask that you not look at the capacitance device variable as this is incorrect.

Hope that helps.