EE241: Advanced Digital Integrated Circuits

HSPICE Tips

• In HSPICE simulation, to accurately calculate the DRAIN/SOURCE junction capacitances, usually either AD, AS, PD, PS parameters are specified by user or ACM = 0,1,2,3 parameter is specified in the model. For example, an NMOS FET of size 10um/0.5um looks like,

                            MN1    vd vg vs gnd  NMOS  L=0.5u W=10u  AD=5p AS=5p PD=11u PS=11u

• To reduce effort in writing HSPICE input file, the original TSMC models are modified and parameters ACM=3 and HDIF=0.5um/0.35um (for 0.35um/0.25um technologies respectively) have been added to the model. Now the same transistor looks like,

                            MN1    vd vg vs gnd  NMOS  L=0.5u W=10u

• To further exploit the feature of the ACM parameter, HSPICE provides another parameter GEO for ACM = 3. GEO usually equals 0-3 with associated meanings as,

                    GEO = 0    indicates the drain and source of the device are not shared with other devices. (default)

                    GEO = 1    indicates the drain of the device is shared with another device.

                    GEO = 2    indicates the source of the device is shared with another device.

                    GEO = 3    indicates the drain and source of the device are both shared with other devices.

• For example, two NMOS transistors in a NAND gate pull-down network share their drain/source. To accurately count for this, the HSPICE netlist may look like,

                            MN1    out A mid gnd  NMOS  L=0.5u W=2u  GEO=2

                            MN2    mid B gnd gnd  NMOS  L=0.5u W=2u  GEO=1

• NOTE!    GEO parameter should be specified with respect to the drain/source terminal definition, i.e., do not mix drain and source.

• How to ask HSPICE for Threshold voltage, Gamma factor, etc.?

            Under given bias condition, HSPICE is able to tell certain device operation parameters. This is done through the so-called "Element Template Output". For example, suppose our input file contains one NMOS FET, something like this,

                            MN1    vd vg vs gnd  NMOS  L=0.5u W=10u

            Then the following statement asks HSPICE to plot the small-signal transconductance of this transistor,

                            .probe gm_of_mn1=GMO(MN1)

            A continuous plot of gm as a function of some input variable (for example, gate voltage) can be generated by sweeping that variable. It is always insightful to compare the results obtained from extrapolation and those from HSPICE template output.

              To learn more about "Element Template Output" format, refer to HSPICE manual Chapter 4.

• Transmission Line in HSPICE

            We use precomputed model parameters to define the U element of lossy transmission lines in HSPICE. It looks like the following,

                            utl        in  0  out  0   tline   l=10m

                            .model    tline    u  level=3  plev=2  elev=2  R11=100  L11=0.2u  CR1=0.4n

            This defines a piece of 10mm long coaxial transmission line with precomputed unit parameters R, L, and C specified by R11, L11, and CR1 respectively. You need to fill in the correct numbers.

              To probe further, refer to HSPICE manual Chapter 21.