Importing supertex MOSFET model

[rlaury]

Hi Group:
I've just started working with Multisim 11. After using another simulator for 12 years, I just needed
more flexibility. I've been trying to import a Supertex MOSFET for days now. I've watched every youtube
video I can find on the subject and read the manual. I just can't make the model work.
The model is from Supertex's web site just as I down loaded it.

Can anyone see something I need to change to have the correct Multisim syntax??
Or can someone tell me what might be wrong. I've tried importing it through database manager.
Any help appreciated.

RonL

.MODEL DN2535   NMOS (LEVEL=3   RS=1.05            NSUB=5.0E14
+DELTA=0.1        KAPPA=0.20      TPG=1              CGDO=3.1716E-10
+RD=11              VTO=-1.50       VMAX=1.0E7         ETA=0.0223089
+NFS=6.6E10      TOX=725E-10     LD=1.698E-9        UO=862.425
+XJ=6.4666E-7   THETA=1.0E-5    CGSO=2.50E-9       L=4.0E-6
+W=59E-3)
.ENDS

[_user32]

rlaury,

Here is the working model within a circuit (right-click and select 'Save Component to DB...).

What is the likely problem is the fact that the default NMOS/DMOS device in SPICE is a 4 terminal device (4th pin is the substrate) and if you are trying to configure as a 3 terminal device you'll typically need to wrap it around with a .subckt statement with the 3 terminals with the Source and Substrate connected together (see below).  

Also another thing to keep in mind is that the pin mapping order is crucial to getting the part to function and sometimes this is often times an error prone step (symbol - model pin mapping).   The default order for native SPICE mosfet devices is Drain, Gate, Source, Substrate.

The model in Multisim with the appropriate header information as configured in a 3 terminal device would look like this:

.subckt DN2535X 1 2 3

m1 1 2 3 3 dn2535
.MODEL DN2535 NMOS (LEVEL=3 RS=1.05 NSUB=5.0E14
+DELTA=0.1 KAPPA=0.20 TPG=1 CGDO=3.1716E-10
+RD=11 VTO=-1.50 VMAX=1.0E7 ETA=0.0223089
+NFS=6.6E10 TOX=725E-10 LD=1.698E-9 UO=862.425
+XJ=6.4666E-7 THETA=1.0E-5 CGSO=2.50E-9 L=4.0E-6
+W=59E-3)

.ends

For the symbol, if you selected / copied one of the existing Depletion mode mosfet devices, on the next to the last step (the mapping step), the mapping should look like this as shown below(note the order is not 1, 2, 3).  (I reused the symbol by selecting the BSV81 device in step 3):

Attached is the functional DN2535 part within a schematic configured as a constant current source.

Note: I also had some issues when I first imported this device model when I copied and pasted it directly from this forums page - this was due to the fact there were some extended unicode characters (embedded, hidden) that are included in copy/paste actions.   This can sometimes cause problems as well.   When I copied this into a new document and saved it (MS Notepad is best), this removed the special hidden unicode characters and allowed for a smoother import.

Not sure which issue you had, or maybe a combination of them... but this should now work.  Thanks for using Multisim!

Regards,

Pat Noonan

National Instruments

[rlaury]

Thanks Pat:

I knew this was the problem. I really want to get good at doing this

and this will help.

Thanks for your help.

RonL