Multisim MOS tutorial

[Monib]

Hi,

I am new to Multisim, I have been using PSpice and Cadence (Virtuoso, SpectreS), for circuit simulations at school. I need something I can use at home. PSpice is good for smaller circuit, but since I started my Masters, I am looking for something to simulate bigger circuits, as well as give me more simulation options. I have a few questions:

I two models for TSMC35 that I am trying to use within multisim. Here are the models:
http://www.public.asu.edu/~mahmed3/tsmc35P.m
http://www.public.asu.edu/~mahmed3/tsmc35N.m

Can I load these directly, or do these need to be modified?

Secondly, in Cadence I am able to sweep the widths or length parameter, will I be able to do this in Multisim?
Third question, am I able to assign variables to various widths and lengths throughout my circuit and edit this from one source?

Last question is about the various version of Multisim. Currently I am using the student version and it has a 50 component limit. Do components include all devices, such ground, voltage sources, transistors, diode, and passive component? Are their version available to increase the component limit?


Thank you for your time and responses.

[Monib]

I changed the Virtual model NMOS/PMOS using my M-files, but I had to change the LEVEL to 6 in order for it to work. How will this affect my simulations, versus LEVEL 11?

Monib

[OStep]

Monib,

There's really no standard among spice simulators as to what "level" corresponds to what MOSFET device model (except for the basic levels 1,2 and,3). Multisim supports the following MOSFET device models:

Level Value	Description
1  or  MOS1	Shichman-Hodges model (DEFAULT model)
2  or  MOS2	More complex model than LEVEL 1 based on actual device physics
3  or  MOS3	Semi-empirical model good for simulating short channel effects
4  or  BSIM1	BSIM1
5  or  BSIM2	BSIM2
6  or  MOS6	N-th power law MOSFET model
8  or  BSIM3	BSIM3 (version 3v3)
14 or  BSIM4	BSIM4 (version 4v5)

You have to find out whether this TSMC35 model is based on any of the above.  If so, adjust the level parameter accordingly. If not, please provide us some reference. But my guess is that its one of the BSIM models.

Regarding your question about adjusting parameters globally - yes, there's a way to do this using circuit parameters. I can help you set this up once you straighten out the mosfet model issue.

[Monib]

I beleive it is a BSIM3 model. When I run it using Cadence, BSIM3 3v3 shows up. What paremeters will I need to change?

Is there a tutorial anywhere that shows how to create an CMOS inverter w/o using  the Virtual transistors? It seems that there aren't that many tutorials available, which is a shame, because it seems like a very intuitive program.

Monib

[OStep]

Monib,

So set level to 8. If you dont want to use virtual transistor, you can create your own component. The best way to do that is using the component wizard, but I have done that for you. I have also added an ability to parametrize length and width using the arbitrary spice block and subcircuits parameter passing ability.

Cheers

[Monib]

Hi,

Thanks for your help, but I get the following error when I try to simulate. I am attaching the error log. I haven't had time to look through it yet, I will let you know if I make any progress. xl, and xw are ignored. The forum won't let me upload .log files, I am renaming it to a file type it will let me upload. Please rename it to .log.

For the arbitary spice block, that is used to set the W, L globally, right, ie only to one W and L value for all the transistors? All I would have to do is assign different variables names in each transistor on my circuit, to be able to control each value W, L individually.

Monib

[OStep]

Monib,

I am not sure why those two parameters aren't supported. Perhaps its some modified BSIM3.3 model or even a different one all together.

The arbitrary spice block contains 2 parameters: "len" and "wid". These are used in the subcircuit instance to assign a value to subcircuit parameters "l" and "w" which are then used to assign a value to the actual mosfet parameters "l" and "w"

Thanks