Magic - Simulation with HSpice

Magic designs may be simulated using either HSpice (analog simulation) or Verilog (digital simulation). This document describes the creation of HSpice files and the use of the HSpice simulator.

File creation

Generate ".ext" files for your design
- execute ":extract" from within magic.

Generate ".spice" and ".sp" files for your toplevel cell

execute "ext2sp <cellname>" from the unix prompt.

This creates

"<cellname>.spice"

a transistor level spice netlist of your magic design (included automatically in "<cellname>.sp")

In the case of the loaded inverter circuit designed in the magic hierarchy exercise, the file should look like this:

* HSPICE file created from inv_ld.ext - technology: c035u

.option scale=0.05u

m1000 n2 out Vdd Vdd pmos03553 w=36 l=7
m1001 n2 out GND GND nmos03553 w=16 l=7
m1002 n1 out Vdd Vdd pmos03553 w=36 l=7
m1003 n1 out GND GND nmos03553 w=16 l=7
m1004 out in Vdd Vdd pmos03553 w=36 l=7
m1005 out in GND GND nmos03553 w=16 l=7
C0 in GND 1.0fF
C1 n1 GND 1.3fF
C2 n2 GND 1.3fF
C3 out GND 3.2fF
C4 Vdd GND 1.1fF

** hspice subcircuit dictionary

"<cellname>.sp"

a skeleton spice stimulus file for you to edit

In the case of the loaded inverter circuit designed in the magic hierarchy exercise, the file should look like this:

** HSPICE file for inv_ld
**   - generated by ext2sp v4.1

** Include netlist file for inv_ld
.include inv_ld.spice

** Default 3.3V Power Supply
Vsupply Vdd GND 3.3V

** Specify input signals here
** e.g. for inputs A and B
**   VA A GND PWL(0NS 0V  2NS 0V  2.25NS 3.3V  6NS 3.3V  6.25NS 0V)
**   VB B GND PWL(0NS 0V  4NS 0V  4.25NS 3.3V  8NS 3.3V  8.25NS 0V)

** Default Simulation - Type, Resolution & Duration
.TRAN 10PS 10NS

** Specify ouput signals to measure here
** e.g. rise and fall delays for output Y
**   .measure tran fall_delay TRIG v(Y) VAL='3.3*0.9' TD=0NS FALL=1
**   + TARG v(Y) VAL='3.3*0.1' TD=0NS FALL=1
**   .measure tran rise_delay TRIG v(Y) VAL='3.3*0.1' TD=0NS RISE=1
**   + TARG v(Y) VAL='3.3*0.9' TD=0NS RISE=1

** Save results for display
.OPTIONS POST
** Avoid DC convergence in at unreasonable voltage
.OPTIONS GMINDC=1n

.END

- note that unless you use the "-f" option, the ".sp" file will not be overwritten by subsequent uses of ext2sp on the same cell.

Edit the stimulus information within the ".sp" file.
- edit the "<cellname>.sp" using your favourite editor.
- Power Supply
  
  The default 3.3V power supply, Vsupply, between Vdd and GND should be fine provided that you have labelled your design correctly.
- Input Signals
  
  You must add an input specification for each of your cell's inputs.
  
  For digital cells it is usual to specify the inputs as Piece-Wise Linear voltage sources referenced to the GND node. The example:
  describes a voltage source called VA (all voltage souces begin with a V) between node A and GND. Within the brackets there are a number (in this case 5) of time, voltage pairs which fully describe voltage source.
  
  The figure below shows the waveforms generated at nodes A and B by the two example PWL statements:
  In the case of the loaded inverter example we wish to describe a voltage source on the node labelled in so we might include the line:
  which describes a voltage source called Vin between in and GND with the same Piece-Wise Linear shape as the VA example above.
- Simulation Specification
  
  The default simulation type is .TRAN, a transient analysis, this is suitable for the investigation of simple digital circuits.
  
  The simulation resolution defaults to 10ps. You may change this if you wish.
  
  The simulation duration defaults to 10ns. You should ensure that this time is long enough to observe the response to the last change in the inputs.
- Measurement
  
  Although measurements can easily be made from the waveforms once the simulation is complete, inclusion of .measure commands in the "<cellname>.sp" file provides an automated method of measuring rise, fall and propagation delay times during simulation.
  In each case the command measures the time between a TRIGger time and a TARGet time described in terms of the behaviour of a signal.
  The following measurement for the fall delay on signal out, specifies that the trigger time is the first time the out signal falls past the 3.3v×90% while the target time is the first time the out signal falls past the 3.3v×10%:
  To measure a propagation delay, the threshold voltages will be set at 3.3v×50% and the trigger will be taken from a transition on the input signal:
  For details on writing .measure commands see page 2-92 of the Hspice Command Reference manual.
At the end of this editing process the "inv_ld.sp" file for the loaded inverter is only slightly changed:

Simulation

Run the simulator
- execute "hspice <cellname>" from the unix prompt
View the signal waveforms using CosmosScope
- execute "c_scope -pfiles <cellname>.tr0" from the unix prompt
Using the newly opened "<cellname>.tr0" window, select the voltage signals for display (e.g. v(in) and v(out)) by double clicking the left mouse button over each of the signal names in turn.

The result should look like this:

The black background used here is OK for on-screen viewing but when you generate a printout for your log book or create a figure for a report you need a white background. Select "Graph -> Color Map -> Map 2" from the main CosmosScope window menus for the arrangement shown below (or "Graph -> Color Map -> Mono" for a black and white version):

The resulting waveforms can then be printed directly to a printer:
```
    File -> Print ...
        
      Print
        Printer name:  [ <printername>                -]
      Save
```
Alternatively the waveforms can be exported as a postcript file for subsequent inclusion in a report:
```
    File -> Export Image ...
        
      Export Image
        File name:     [ <cellname>.ps                 ]
        Files of type: [ Postscript (*.ps,*.eps)      -]
      Save
```
CosmosScope also includes a facility to take measurements from the waveforms displayed via the Measurement Tool which can be invoked from the Tools menu. This can be very useful where .measure commands were not included in the spice file.
View the results of the .measure commands
- execute "cat <cellname>.mt0" from the unix prompt
Results are given in scientific notation with no units (e.g. propagation_f = 2.249e-10 ) so you will need to convert them into picoseconds or nanoseconds before presenting them in any report (e.g. Propagation delay from in↑ to out↓ is 0.22ns).
Remember to perform "sanity checking" on your numerical results. If the value provided by the .measure command doesn't make sense when you try to match it to the waveforms then you've probably mis-specified either the TRIGger or the TARGet.

Additional Documentation

The Hspice Command Reference is available on-line.
Further information on spice simulation can be found in the Web document Spice Simulations.
The Spice Manuals are also available on-line.

Iain McNally

7-10-2011