how to simulate Id/W vs gm/Id?

[carlson]

when I design the common source amplifier,I want to plot ID/W as a function of the design variable gm/ID. But I don't know how to set the ciruit state to obtain the results. For example ,I should set which is dc sweep variable and other initial circuit conditions? I wish to have the complete hspice netlist. Thank you!!!

 

[Humungus]

It is easier to plot gm/Id vs Id/W as the inverse function could not have a unique correspondence, that is there could be at least two values of Id/W for the same gm/Id (due to leakage currents).

Bias your transistor at Vd=Vg, keep you Vs=constant and perform a primary sweep of Id. Tell your simulator to plot gm/Id vs Id/W. You could perform a secondary sweep for extreme values of transistor sizes (narrow&short; narrow&long; wide&short; wide&long; in between). Also, you could perform a secondary sweep of your body voltage.

In Eldo, this would read like it follows:

.param width=10e-6, length=0.25e-6
m1 d d s b xmos w=width l=length

Vs s 0 0
.param v_body=0
Vb b 0 v_body

.param id_sweep=1e-3
Ibias 0 d id_sweep

.dc param id_sweep log 20 0 10e-3
.step param v_body -2 0 0.5

.defwave gm_over_id='gm(m1)/id(m1)'
.defwave id_norm='id(m1)/width'

.plot w(gm_over_id) versus w(id_norm)

 

[icx]

Have you ever used this method in hspice and spectre?
I want to know how i can get Id vs id/gm in hspice and spectre.
thanks.