ofet / tft simulation

[rob_xx17]

hello,

I have multisim version 10 and I'm trying to simulate an OFET (it has a really small current for really large voltages. ie. for Vg=40V, and Vd=50V, Id=1uA) that I made in my lab. is there a simple way of creating this in multisim so that I could incorporate it with other elements in a simulation? I tried modifying parameters of existing transistors (MOSFET ), such as Vdss, Vdgr, Id, or Rds. but I can't obtain the results that I'm looking for. also, when I created a custom component using the Component Wizard that also didn't work. I'm sure there's some easy way of doing it, but I just haven't found it yet. thanks for any suggestions.

r. 

[yyao · Accepted solution]

Hi Rob,

If you have a good mathematical model to work from, you can try using a NONLINEAR_DEPENDENT source. You can find it in the Sources group under the CONTROL_FUNCTION_BLOCKS family. Connect your input voltages and currents on the left and enter an expression for the current or voltage which appears on the right.

Hope that helps.

[rob_xx17]

thanks a bunch for your suggestion. that worked terrifically well. kudos to you.

I have another question, but I'm not sure if I should post it here or make a new post. I have a SPICE code and I'm trying to build a multisim component that I could connect with other components for later analysis/simulation. a user guide that I'm using (multisim user guide, section 6.6.2.3 creating a subcircuit model) says that I should "type it (the SPICE code, I suppose) into the model data window" - how do I find this model data window? 

the guide says that I can also 'first draw the circuit in multisim and export the SPICE netlist and then modify it' - when I create the circuit in multisim, do I save it just as a regular circuit file, with .ms10 extension? if so, how do I then export the SPICE netlist? and then modify it?

I'm sure that this is a rather simple task. yet, I've been unable to accomplish it. so, I thank you, in advance, for your help. 

r. 

[yyao]

To get a SPICE model of your circuit, click Transfer>>Export Netlist. It is up to you to take the contents of the netlist, wrap it in a .subckt and make sure that all the node names match up.

Once you have done that, use the component wizard to create your component. Here's a tutorial on how to do that. You don't have to make a component which maps to a footprint if you don't want to. You will have the opportunity to set the SPICE netlist in this wizard. Remember to specify the model name for your SPICE model (step 6 of the tutorial). People forget to do this and it won't work otherwise.

Once you've done that, you will save it to your database and be able to use it.

[rob_xx17]

thanks a million. it really helps.

what I'm trying to do is to import a model of an element (memristor) from another software (micro-cap). how do I name nodes in a file for a later reference? for instance, here I'd need five nodes: Plus, Minus, x, flux, and charge.

r. 

[yyao]

You should be able to read (and edit) the node names by just looking at the contents of the SPICE netlist. For example, a Resistor can appear as the following in a netlist:

R1 N1 N2 Val

where:

• R1 is the name or RefDes of the resistor
• N1 and N2 are the names of the nodes connected to R1
• Val is the value of the resistor (e.g. 1k)

You can just change the value of N1 and N2 to change the node name. Just make sure that the node name is unique and you change the node name with every component that is connected.

Here are two good SPICE references to get you started:

http://zone.ni.com/devzone/cda/tut/p/id/5413

http://newton.ex.ac.uk/teaching/CDHW/Electronics2/userguide/

You can also change the name of any node inside Multisim. Node names are also known as net names in Multisim. Simply double click on any wire on the node. Click on the Net Setttings tab in the dialog that appears. Change the Preferred net name and click OK. This will update the name of the node and updates all occurrences of the node name in the SPICE netlist.

[rob_xx17]

Yi,

thanks a bunch for your help. I did exactly what the tutorial said (including changing the model name) but I'm getting an error when I'm trying to simulate the component. apparently multisim is not happy with inclusion of a function (.func f(x,p)={1-(2*x-1)^2*p)}. how do I explicitly include a function (I have a component and it's voltage is a function)?

as always, thanks a million.

r. 

[yyao]

Hi Rob,

I took a look at your SPICE model for the memrister and I think you got the SPICE modeling down pretty well.

I think you tried to simulate your circuit in Multisim 10.0. The .func (user defined functions) command wasn't available in Multisim 10.0. It was a new feature for Multisim 10.1. But you also use SDT (numerical integration) which is a new feature which we just added for Multisim 11.0. So, in short, you need at least Multisim 11.0 to simulate your circuit. If you haven't done so already, you can download and try Multisim 11.0 here:

http://www.ni.com/multisim/

Your schematic simulated in Multisim 11.0 without problems, however, I cannot say if it is behaving the way you expect it to. Give Multisim 11.0 a try and tell us how it goes.

Hope that helps.

Message Edited by yyao on 05-12-2010 03:31 PM