Multisim and Ultiboard

Showing results for 
Search instead for 
Did you mean: 

How to change the parameters in virtual MOSFETs in version 10

In Multisim 7, I could easily change VTO, KP, GAMMA, LAMDA, etc.  I am giving some students an assignment that requires this, and it appears that I can't do it in version 10.  I know they couldn't do it in 9 either, but I thought this was going to be fixed, or another model made, etc.   Is there anything like this?
0 Kudos
Message 1 of 5
Which component are you working with?... for example, the 2N6782 if you double-click on it, and then select Edit Model (from the Value tab) you can see on the spice code those parameters so you can just edit them. I'm sure there will be some components whose model will be different so if you tell us which one you are using I can tell you if there is a way to change them or not...
0 Kudos
Message 2 of 5
Virtual 3 Terminal Enhancement Mosfet
Yeah, I know I can go to another model, and/or go to the component wizard, but it used to be easier when you could do it with the virtual ones. 
0 Kudos
Message 3 of 5

I know that changed for virtual mosfets, here is the way you can workaround it, place the virtual mosfet alone on the schematic, then go to Transfer >>  Export Netlist... you will now have a text file with the full model you used to find in version 7. You can use this model to create a new component with the wizard like you said. Or use one of the components from the database, like the one I mentioned, and Edit it so you can save a new component with the new model in your user database, and pass this component to your students. The final model should be something like this

.subckt 12343 1 2 3
m1 1 2 3 IDEAL w=100 l =100
+ LEVEL= 1
+ VTO=   0.0
+ KP=    2.0e-5
+ GAMMA= 0.0
+ PHI=   0.6
+ LAMBDA= 0.0
+ RS=    0.0
+ RD=    0.0
+ CBD=   0.0
+ CBS=   0.0
+ IS=    1.0e-14
+ PB=    0.8
+ CGSO=  0.0
+ CGDO=  0.0
+ CGBO=  0.0
+ RSH=   0.0
+ CJ=    0.0
+ MJ=    0.5
+ CJSW=  0.0
+ MJSW=  0.5
+ JS=    0.0
+ TOX=   1.0e-7
+ NSS=   0.0
+ TPG=   1.0
+ LD=    0.0
+ UO=    600.0
+ KF=    0.0
+ AF=    1.0
+ FC=    0.5
+ TNOM=  27
+ )

I hope that helps...

0 Kudos
Message 4 of 5
This is a known problem and it will be addressed in the next public update of Multisim.

As a workaround,  I suggest you simply create a new MOSFET component with a SPICE subcircuit as its model. Here's the easiest way:

1. Go to component wizard (tools->component wizard)
2. Select single section, 3 pins (or 4 pins)
3. In the symbol selection step (step 3), click 'copy from db'. Browse to the transistor family and pick a transistor whose symbol you wish to use for you new component.
4. In step 5, for the model name file type an arbitrary name. For the actual model field, copy and paste the following template:
* Node 1 -> Drain
* Node 2 -> Gate
* Node 3 -> Source

M1 1 2 3 MyMosfet1 L=100u W=100u

+VTO=4.37181 LAMBDA=0 KP=20.8388
+CGSO=1.76012e-05 CGDO=1e-11

Notice that the mosfet instance call (M1 1 2 3 MyMosfet1 L=100u W=100u) and the .model (.MODEL MM....) are  wrapped in a subcircuit.  The optional substrate pin can be added in the template. Just list it after pin 3.

5. In step 6, make sure to map the drain pin of the symbol to pin 1 of .subckt, gate pin of symbol to pin 2 of .subckt, and source pin of symbol to pin 3 of .subckt
6. Save the component to the User database

Once you place the component, simply double click and hit 'edit model'. From there you can quickly and easily adjust parameters of the MOSFET for the placed instance.

Hope that helps,


National Instruments
0 Kudos
Message 5 of 5