Post-Layout Simulation with MachTA and EZWave

In this lab, you will use ICStation to extract a Spice representation of the inverter you drew in the previous tutorial. Then you will use the MachTA simulator to simulate the Spice representation.

1.1 Move into the directory you created for lab2. Then start ICStation:

>> cd egre429/lab2
>> ic &

1.2 In ICStation, use the Cell Open item in the Session palette to open the my_inv cell you previously created. In the IC Palettes palette, select ICExtract(M). In the ICExtract (M) palette, select Lumped. An Extract Mask Lumped Parameters dialog box should appear.

1.3 Fill out the dialog box so that it looks like the one below and click OK:

1.3 Exit ICStation.

MachTA is another version of a Spice simulator that is much faster than Accusim.  Unlike Accusim, it does not operate on a schematic, but on a text input file in Spice format like the one you just generated from ICStation. However, the Spice file you just generated from ICStation is not quite complete and needs to be "fixed" before you can simulate it with MachTA.

2.1 Open the Spice file called my_inv.sp generated by ICStation in a text editor. You should see a file like this:
 

* File: /fac/rhklenke/tmp/lab2/my_inv.sp.  Creation time: Tue Aug 31 16:30:39 1999

.subckt my_inv GND in1 out1 VDD
* devices:
m0 out1 in1 VDD VDD p l=0.6u w=5.4u ad=9.72p as=9.72p
m1 out1 in1 GND GND n l=0.6u w=4.8u ad=8.64p as=8.64p
* lumped capacitances:
cp1 in1 GND 2.066f
cp2 out1 GND 2.068f
cp3 VDD GND 2.642f
.ends my_inv
 
 

Notice that the file contains a subcircuit called my_inv that consists of two transistors (the ones you layed out) and several capacitors (paracitics). In order to simulate this circuit, we need to get rid of the subcircuit notation, add voltage sources for VDD and GND, and add model statments for the transistors.

2.2 Close the text editor. From the command line, run the cell_sim_prep script on the my_inv Spice file:
 

>> cell_sim_prep my_inv


This will generate a file called mta_my_inv.sp which is correct for simulation with MachTA.

2.3 Open the resulting mta_my_inv.sp file. You will see a file like the one below:
 

* Model file for MTA
* The following lines have been added
.model p pmos
.model n nmos

Vvdd VDD 0 5
Vgnd GND 0 0

* Here begins the original Spice deck
* File: /fac/rhklenke/tmp/lab2/my_inv.sp.  Creation time: Tue Aug 31 16:30:39 1999

* devices:
m0 out1 in1 VDD VDD p l=0.6u w=5.4u ad=9.72p as=9.72p
m1 out1 in1 GND GND n l=0.6u w=4.8u ad=8.64p as=8.64p
* lumped capacitances:
cp1 in1 GND 2.066f
cp2 out1 GND 2.068f
cp3 VDD GND 2.642f
.END
 
 

Notice that there are two new voltage sources added for VDD and GND, model statments for the devices added, and the subcircuit line has been removed. This file is ready to simulate with MachTA.

2.4 Close the text editor.

 
2.1 Start MachTA on the mta_my_inv.sp file:
 
>> mta -ezw -t $ADK/technology/mta/ami05 -tc TYP mta_my_inv.sp &


You should see a window like this open up:



Notice there is a prompt window in the bottom of the MachTA window. You can type commands to the MachTA simulator here.

2.2Type in the following commands to plot the voltage at the in1 and out1 ports of the inverter:
 

> plot v(in1)
> plot v(out1)


2.3 Type in the following commands to force the in1 input to 0 (low) run the simulation for 10 ns, force in1 to 5V (high), run the simulation for 10 ns, and finally force in1 to 0V again and run the simulation for 10 ns:
 

> l in1
> run 10 ns
> h in1
> run 10 ns
> l in1
> run 10 ns


2.4 Start the waveform viewer by pressing the Wave Viewer button in the MachTA window. A new EZWave window like this will appear and after a few  seconds:



 
2.5 Add the waveforms for V(in1) and V(out1) by double clicking on the run item under mta_my_inv.wdb, and then double clicking on the V(in1) and V(out1) items that appear under that. The result will be a waveform display like the one below:





2.6 In another terminal window, start the Acrobat reader to view the MachTA quick reference guide:
 

>> acroread $MGC_HOME/shared/pdfdocs/mta_qref.pdf &


2.7 Read the sections on the Structure, Signals, and Device viewers. Use them to bring up a picture of the devices connected to the in1 and out1 ports. Does this look like an inverter?

2.8 Take a look at the rest of the quick reference quide. Exit MachTA and Acrobat reader when you are done.


** If you have previously used the older version of MachTA (prior to September 15th, 2004) on your spice file, you need to remove all of the files for your circuit associated with this older version. For example, above, you would need to execute:


> /bin/rm -i mta_my_inv.*


and select "y" (yes) for all of the files EXCEPT mta_my_inv.sp to remove all of the old files. In addition, if you have never used the new version of MachTA and EZWave, you need to execute the following from your command line:


> export MACH_HOME=/mentor/machta/mach_v3307.ss5
> export PATH=$MACH_HOME/bin:$PATH
> export anacad=/mentor/ams_d2
> . $anacad/com/init_anacad.ksh

Or you can add these lines CAREFULLY to the end of your .profile file and logout and log back in again.