2 ratings:

3.5 out of 5

Rate this Document

Importing a MOSFET Model into Multisim

Primary Software: Electronics Workbench>>Multisim
Primary Software Version: 10.0.267
Primary Software Fixed Version: N/A
Secondary Software: N/A

Problem:
How do I import a SPICE MOSFET model that starts with a .MODEL statement into a Multisim component?

Solution:
Any SPICE model that starts with .model is a core model and the Multisim SPICE engine already has the pin template defined. The Multisim SPICE engine expects the MOSFET model to have four pins. If you used a three pin symbol, Multisim will simulate with an error message. For example, the model you want to import into a component is similar to this:

.MODEL B4 NMOS VTO=1.7 KP=322E-6 LAMBDA=0.005
+CGSO=2.5E-9 CGDO=2.5E-9

The general form for a SPICE MOSFET is:

Mxxxx D G S B model_name

To use the above model in a three pin symbol, you must use a .SUBCKT statement and tie the S and B pin together internally. Here is an equivalent model:

.SUBCKT MOS D G S
M1 D G S S B4
.MODEL B4 NMOS VTO=1.7 KP=322E-6 LAMBDA=0.005
+CGSO=2.5E-9 CGDO=2.5E-9
.ENDS

Note the two S nodes on the M1 line. This is how you connect the S and the B pin together. If you do not want to modify the model, you must use a four pin symbol.

Related Links:
Developer Zone Tutorial: Creating a Custom Component in NI Multisim
Developer Zone Tutorial: SPICE Simulation Fundamentals

Attachments:





Report Date: 06/07/2007
Last Updated: 06/05/2009
Document ID: 4A6ANQMC

Your Feedback!	Poor  |  Excellent							Yes	No
Document Quality?							Answered Your Question?
	1	2	3	4	5
Document needs work? Please tell us why.
Please Contact NI for all product and support inquiries.