Liang,

I'm assuming you use the Analog Design Environment?

If so,  then the first thing you would do is to set up
the expression to measure the delay. Do a transient
simulation to get the waveforms you want, and then
using the Calculator (Tools->Calculator), use the "vt"
button and select the two nodes. Then use the
Special Functions->delay item on the calculator and
specify the threshold values and edge numbers for
the two waveforms.
The resulting calculator expression can be added to
the ADE outputs pane by using the  Outputs->Setup
menu in ADE, and hitting the Get Expression button.

Having got it in the outputs pane,  hit the  Plot Outputs
icon (bottom right) - this should show the delay in the
output pane.

OK, having got the expression OK and working, then
move onto monte-carlo.

For this you need to have statistical models of
course (with statistics blocks, which describe
the distribution of various parameters - see the Spectre
User and Reference Guides for more details).

Then use Tools->Monte Carlo in the ADE window.
You can use Get Expression here to get the expression
for delay from the calculator.
Choose the number of runs you want to do, choose
whether you want Process Only, Mismatch Only or
Process and Mismatch, and do Simulation Run.

You can then use Result->Plot->Histogram to plot
the resulting distribution.

Of course, this is a bit of a high level glib overview, and
I'd suggest you read up on this in the documentation,
but hopefully enough to get you started.

One other point - you need product 32120 (Electronic
Design for Manufacturability option - shows up as
FEATURE Artist_Statistics in your license file) to do this.
You can also run Monte Carlo from the new Aptivia tool
(I won't cover that here, because I suspect you're
not using that since it is so new).

Regards,

Andrew.