The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> ron in Spectre = 1/gds in HSPICE???
https://designers-guide.org/forum/YaBB.pl?num=1176261122

Message started by ywguo on Apr 10^th, 2007, 8:12pm

Title: ron in Spectre = 1/gds in HSPICE???
Post by ywguo on Apr 10^th, 2007, 8:12pm

Hi, Guys,

I want to know the output resistance of a MOSFET which is in saturation region.

In Virtuoso Analog Design Environment, choose Results -> Print -> DC Operating Points, then select the MOSFET in schematic, the related operating point parameters is shown in Results Display Window. It reports ron = 36.0259K.

I take a look at the definition of ron using spectre -h bsim3. ron (Ohm) is On-resistance.

However, I simulate using SPICE again. As well known, .op statement gives all parameters of MOSFETs. There gds = 2.034e-7. So rds = 1/gds = 4.916 MOhm.

What's wrong with my simulation?

BTW, I apply a test voltage source at the drain of the MOSFET and run ac simulation using Spectre and SPICE respectively. SPICE gives a reasonable result of the drain current. However, Spectre's result is eccentric. I display the drain current using signal to results display table. Some points is infinity :( , especially at high frequencies.

Best regards,

Yawei

Title: Re: ron in Spectre = 1/gds in HSPICE???
Post by Andrew Beckett on Apr 11^th, 2007, 7:03am

I had a quick experiment here, and I did a sweep of V_DS for a fixed V_GDS and then plotted ron and ids/xval(ids) (the calculator expression was actually:

Code:

(xval(getData("m1:ids" ?result "myanal-dcAnalysis.dc")) / getData("m1:ids" ?result "myanal-dcAnalysis.dc"))

which should show the resistance (I_DS divided by V_DS) and this is identical to ron. The 1/gds was higher.

Didn't have time to investigate the AC results you describe.

Andrew.

Title: Re: ron in Spectre = 1/gds in HSPICE???
Post by Geoffrey_Coram on Apr 12^th, 2007, 4:25am

Andrew Beckett wrote on Apr 11^th, 2007, 7:03am:

the resistance (I_DS divided by V_DS) and this is identical to ron. The 1/gds was higher.

Note that gds is the partial derivative of Ids with respect to Vds, sometimes called the "small-signal conductance." ron in Andrew's experiment is sometimes called a "large-signal resistance" and is the slope of the line connecting (0,0) with (Vds,Ids), rather than the slope of the tangent line at (Vds,Ids). I believe what you want for the "output resistance" is 1/gds, NOT ron, because you care about the incremental change in Ids with respect to Vds.

I'm surprised to hear of infinite values in your results table. Are you sure you have it set up correctly?

Title: Re: ron in Spectre = 1/gds in HSPICE???
Post by ywguo on Apr 12^th, 2007, 6:07am

Geoffray,

You are right. I don't care the large signal resistance, but the small signal output impedance of a MOS transistor/current source.

The online help of spectre lacks of detail information and definition for the parametes. It looks that ron is on-resistance. However, it doesn't tell users that is defined as V_DS divided by I_DS.

About the infinity value in my results table, I will check my circuit and post the schematic later.

Thank you, Geoffrey and Andrew.
Yawei