INSTANTIATE (MOSFET) MODEL PARAMETERS and

DISPLAY and ANALYZE MODEL CHARACTERISTICS Version 2

NEW START:

Step #1: Invoke pSPICE by double-click of the left mouse button (DCL) on the pSPICE ‘design manager’ icon as was done for startup under tutorial #1. The double-click left (DCL)on the schematics icon for which the blank pSpice schematics screen will appear. Assuming that you have walked through the previous tutorials, this process should be fairly routine by now.

And, as has been done before, (Step #2) go to the Parts menu. In this case you have need to select the MOS part called MbreakN, as illustrated by the screen shown

Place and Close a copy of this part on the Schematics screen and leave it highlighted, since the next step will call for you to make this part into one that is appropriate to performing designs in a current manufacturing technology.

Step #3: Pull down the Edit > Model menu, for which you will immediately get a message that says ‘New schematics must first be saved’. So you will now need to save you file under whatever name you choose. For this illustration, we will save it under ‘nMOSa7’ and move on. Once you have saved your file, then the ‘Edit model’ option will be enabled for which you should see the pop-up screen

You will need to select ‘Edit Instance Model (ModelEditor)’ and for which you will now have the screen

Since this screen is an ‘edit’ window, you can make changes that will stick. This is accomplished by highlighting the text and overwriting, which is the usual operation for editors created in the MS windows environment.

Step #4: Now we get the parameters needed for our MOSFET.

Go to the URL http://www.mosis.org/Technical/Testdata/menu-testdata.html

which looks like

Although the appearance of this site page may change, and surely the parameter and technologies will change, you note that there are several fabrication processes identified. Since universities are usually confined to only a few processes, let us choose the one identified as ‘AMI 0.50 micron (C5N) and see what is there. This technology is one for which the smallest feature size is L(ength) = 0.5um. As well as the active n- and p- layers this technology has 5 interconnect layers, two of which are polysilicon (poly) and three of which are metal, probably of various refractory alloys conducive to high temperatures and that have a reasonable conductivity. The two polysilicon layers are used to form embedded capacitances.

Under this menu we will find that there is a long list of process runs, and we will select the one called T22Y.

Selection of this process run displays a data sheet that indicates values of various extracted data and parameters, such as sheet resistance, area capacitances, and various thresholds. But the part of the data sheet that is of primary interest to the transistor is the part that contains the transistor parameters. And here we encounter a situation.

Given the very small size of the transistor, the electric fields therein are enormous, and therefore there are many physical effects that take place. And each effect has its own equation. And each equation has its own parameter. And there are several different mathematical models that can be assumed. And often these are a mathematical mess. And so the parameter list is often long.

Well let’s not get entangled by the descriptions of MOS transistor models. We will cut to the chase and pick one. The one that is most often used is a semi-empirical, semi-statistical model called BSIM3V3 (or a later version called BSIM3v4). It is godawful, and often disliked. But it is available.

And its parameters, as available under the file that we have accessed are shown below.

Notice that they fill the page. Ugh! What a mess.

but if they can be displayed, then they can also be highlighted and captured (Ctrl-c). Do so, and be sure that you have them all, beginning with ‘LEVEL = ‘ and down to ‘*’. Capture only the parameters associated with the NMOS device.

Step #5: Now find the edit window for the nMOS transistor that you left active, position your cursor, and paste (Ctrl-v) these parameters into the space after the left parenthesis. Assuming that the copy/paste operation has been successful, you should see them in place.

But there is still some work that must be done before you have completely instantiated these parameters into the model file. And you will also need to make some changes. Change LEVEL = 49 to LEVEL = 7. When operated in the VLSI environment, BSIM3 is level 49. But pSPICE is a maverick, and calls this model level (LEVEL = 7). If you digress to some other simulation platform you will have to ascertain for yourself which level corresponds to which model.

Also change the model name CMOS to a handle appropriate to the technology that you have instantiated. In this case it is recommended that this be ‘MnT22Y’, since that is the process for the parameter set that you have captured and your device is an nMOS.

Once upon a time, when the industry was young, there were only 2- 3 MOS transistor models. These are the ones that we use in the classroom since they are simple and direct. But they are regrettably inaccurate for sub-micron feature size MOS transistors. So now we have more MOSFET transistor models than a dog has fleas.

Once you have made these changes you should now save the file. When you do so the model editor window should look like

You have now created the parameter file for a part called MnT22Y. To save this part file in a common space pull down the menu (indicated in the header bar above) Model>Export for which you will see the window

and under File name type in the name MnT22Y, which will then save your part file in a common space that you can access (import) anytime.

Step #6 You have one further task to do. Your part is still the template part MbreakN. You must highlight your transistor again, and call up the menu Edit >Model >Change Model reference

For which you must change MbreakN to MnT22Y.

As a check, highlight the part once again and call up the menu Edit >Model >Edit Instance Model (text) which will tell you what model parameters are assigned to your transistor. They should be as expected from your download process.

Step #7: Now return to the Schematics screen, for which you have the one little nMOS part. Before any further use of this part, double click on it to present its sizing options:

We will assume that this transistor will have W/L = 10mm/1mm, which is pretty durn small, but large relative to the minimum feature sizes. We will also assume source and drain areas to both be 10mm x 1 mm = 10 p, and the source and drain perimeters to both be 20 mm. Note that we use ‘u’ as the prefix for ‘micro’. The values are assigned by typing in the values and executing a ‘Save Attr’ in each case.

Use the ‘OK’ to save these sizing features for this transistor.

Now Mr. Transistor is ready and you are ready to put it to work. It can be copied into any other schematic that you might desire, and will retain these process parameters and sizes.

You have created an instance (‘instantiated’) this transistor into your working environment.

In this case we will merely test its behavior. So as step #8: Go to the Parts menu and capture and place a few parts as shown. You might also change a few names, such as VGS, VDS, Vsens. And change the value of the resistance to one that is symbolic as {Rx}, as shown, with a PARAMETERS listing that defines Rx as 10k. The use of the PARAMETER part was outlined in a previous tutorial.

Connect up the device test circuit as shown:

Go to the Analysis > Setup > DC Sweep menu and select values as indicated:

and invoke the nested sweep and setup values as indicated:

Click ‘OK’ . You are now ready to display performance characteristics of the transistor, and they can be invoked by the hotkey F-11 or by the simulation icon.

It should be no surprise that the I(Vsens) vs VDS characteristics look fairly reasonable. There are a few aspects that identify it as a short-channel device, if you are experienced in such characteristics. But otherwise you should see that the device is functional and has fairly regular characteristics.

Your own PROBE output might be a little more colorful than that represented here. In order to eliminate the black background and avoid the problems that it gives a printer, the copy of pSPICE used here has had its ‘pSPICE.ini’ file edited so that the PROBE background is BRIGHT WHITE instead of BLACK. It is recommended that you might do so also for those files that you plan to turn in as hardcopy. Also your printer cartridge will last longer. The file looks something like that shown in the screen below