how to define W and L for each mos transistor on the shematic?

[sean93610]

Hi, I am new to Multisim and wondering if anyone can give me some help here. Thanks!

     What I am trying to do is, I want to use Multisim to run a spice simulation with custom mos models. What I did was:

1) use Component Wizard to create a new component. Assume it is called myNMOS;

2) select "simulation only";

3) select single section component; number of pins: 4;

4) for symbol, I used "copy from DB"'. I selected the symbol of "MOS_4TEN_VIRTUAL" as the symbol. Symbol set "ANSI";

5) Set pin parameter;

6) select simulation model. Here I copy and paste my own mos model, which is shown partially below:

     .subckt myNMOS d g s b params: w=1e-6 l=1e-6 ad=0 as=0 pd=0 ps=0 nrd=0 nrs=0 m=1
* variables: w,l,ad,as,pd,ps,nrd,nrs = standard mosfet parameters
*            m = multiplier
*
m1 d1 g s b newmos w={w} l={l} ad={ad} as={as} pd={pd} ps={ps} nrd={nrd} nrs={nrs} m={m}
rd d1 d {(1.841e+03*6.000e-07/(w+(-7.000e-07)))/m} tc=2.500e-03,6.000e-06  

.model newmos nmos level=7

***** here model detail is not shown here ********

.ends myNMOS

   7) Set pin mapping;

   😎 Add family and finsihed;

    But when I tried to use this newly defined component, I found that I have no way to define my parameters such as W, L, etc on the schematic. Assume there are 10 myNMOS transistors, they use the same model but each has their own W, and L. How do I do that? As you can see these parameters are supposed to be passed to the individual transistor in real application.

    I think this is a very basic function. Multisim must have already taken care of it. I just do not know how. What did I miss here?

    Thanks!

Sean

[yyao]

Hi Sean,

Your approach is correct. By attaching params to your subckt, you can modify these values on the instance level of each transistor. Did you remember to give your model a name in step 5? By default, the model name is EMPTY which won't work. Give it a name with which Multisim can store the subckt with.

If you've done that correctly, double click on the component that you've placed. Click on the Value tab and click Edit model. You can now edit the params associated with each transistor. These changes will effect only the transistor that you are editing.

Hope that helped.

Message Edited by yyao on 03-22-2010 02:14 PM

[sean93610]

Hello Yi,

   Thank you for your help. I tried and it worked. Now I can define W and L individually. Another question, can I put W and L on the schematic so that I can see them directly?

   In terms of the model, it seems Multisim does not support my mos model. The model I am using works with PSPICE. It seems Multisim does not support LEVEL 7 model. When I changed it to LEVEl 8 it still has problems. Can you take a look at it? The model file is aattached.

Thanks

Sean

[yyao]

Hi Sean,

We don't have a way of directly reporting model parameters on the schematic. However, you can ask Multisim to draw additional attributes on your schematic. Double click on the component and click on the Label tab. You can add multiple attributes (such as W and L) and set their visibility to show all. To make them visible, click Options>>Sheet Properties and check the Attributes box in the Circuit tab. Please note that these attributes are independent from the SPICE parameters and you need to update both independently.

I am not sure if you are aware, but the MOSFET level parameter is really a misnomer. It should really be considered to specify the "type" of model rather than the "level" of complexity of the model. You can't simply increase the number of the MOSFET level and expect things to work. The PSpice documentation states that their level 7 MOSFET is really BSIM 3.2. Multisim supports BSIM 3.3 and it is designated level 8 in Multisim. It just so happens to work out that you could just increase the number in this case! Just be careful about this. To view the list of MOSFET models that Multisim supports, click Help>>Multisim Help. Activate the contents tab of the help browser and broswe to Simulation>>Multisim SPICE Reference>>Analog Devices Library>>MOSFET.

I took a look at your model and have the following suggestions. The major offending line that is causing Multisim to give up is:
+vth0=8.053e-01 dev/gauss .0023 lot/gauss .05
this line specifies distribution information that is specific to PSpice only for Monte Carlo simulation. Change this line to:

+vth0=8.053e-01

also, you should remove the parameter jssw=1.250e-10. This parameter is not supported for BSIM3.

Attached is the modified version of your model.

Hope that helps.

[sean93610]

Hi Yi,

   I tried your model in a simple transient simulation but it still has problem. It says unknown error. Unfortunately it does not say too much useful about the error. I also changed my model based on your suggestions and I got same error. Is there anything wrong with my multisim setup? Did you try the model on your side?

[yyao]

Hi Sean,

Take a look at the attached file. It seems to work for me. I tried transient and DC operating point simulation and they seemed to work.

[sean93610]

Hi Yi,

   I could not open your file because I am using Multisim10. Can you convert it to ms10 file?

[yyao]

I redrawn the circuit for Multisim 10.1.1 and it works. I tried the circuit in Multisim 10.0.1 without any luck.

Also, Multisim 10.1.1 does not support the M parameter (multiplicity) on MOSFETS. So, all MOSFETS will have M=1 by default. Multisim 11 supports this parameter.

You can download Multisim 11 and check it out. There's been a lot of functional and cosmetic improvements and features that you will find useful. We added more and better transistor and diode support. We've also added a SPICE netlist viewer from which displays a colour coded version of your SPICE netlist from within Multisim. I find this tool very useful in debugging complex circuits for simulation.

You can download Multisim 11 here:

https://lumen.ni.com/nicif/us/evalmultisim/content.xhtml