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: c35b4

.option scale=0.05u

M1000 n2 out Vdd Vdd modp w=36 l=7
M1001 n2 out GND GND modn w=14 l=7
M1002 n1 out Vdd Vdd modp w=36 l=7
M1003 n1 out GND GND modn w=14 l=7
M1004 out in Vdd Vdd modp w=36 l=7
M1005 out in GND GND modn w=14 l=7
C0 in 0 0.57fF
C1 n1 0 2.34fF
C2 n2 0 2.34fF
C3 out 0 4.40fF
C4 Vdd 0 2.14fF

** 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 v4.7

** Include transistor models for c35b4
.include /opt/cad/designkits/ecs/hspice/c35b4.mod

** 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 Custom WaveView
- execute "wv <cellname>.tr0" from the unix prompt
In the upper "Output View" pane of the newly opened Custom WaveView window, dounble-click on "D0:<cellname>.tr0" and then click on "toplevel" in order to reveal signals in the lower "Output View" pane. You can then either double-click on the required signals (e.g. v(in) and v(out) ) or drag-and-drop them into the right hand "waveview 1" pane.
The result should look like this:

Note that screen captures of waveform windows such as the one above should never be used in a report because the black background obscures the waves while the window border and buttons distract from the information that you are trying to present.
Create a PDF copy of waveform display

First use the Preferences button on the Configuration tab to tell the system that printers exist (we need to do this even if we don't print directly to the printers).
```
    Configuration -> Preferences ...
        
      General
        Printer Devices:     [mono;colour              ]
        Unix Print Command:  [lp -d $printer $file     ]
      OK
```
Next use the Print button of the Waveform tab to create a black and white PostScript (.ps) version of the waveforms:
```
    Waveform -> Print ...
        
      Print Setup
        Printer:                      [mono                     -]
        Paper Size:                   [A4   (210Wx297H mm)      -]
	[ ] Portrait  [ ] Color Print
      PostScript Output File
	[X] Print To File
        Output Path: [ <printfile>.ps                            ]
      Print
```
(select "colour" and "[X] Color Print" for colour printing).
Now convert the PostScript file to PDF using the ps2pdf unix command:
```
    ps2pdf <printfile>.ps
```
Check that the file has been correctly generated using the evince document viewer:
```
    evince <printfile>.pdf &
```
This PDF file can then be included in a report or printed directly to the printer.

Print a copy of the waveform

    print -d <printername> <printfile>.pdf

Measurements

Custom WaveView also includes a facility to take measurements from the waveforms displayed via the Measure Tool which can be invoked from the Utilities menu on the Waveform tab. 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 and the Custom WaveView User Guide are 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

13-10-2022