Qucs Tutorial - DC Parameter Sweep
          This tutor aims at giving the feeling of how to use Qucs to people -especially to students like me- who would like to be independent from comercial or impossible to obtain tools. In this tutorial we will sweep Vds of an nMOS transistor while keeping the Vgs constant to produce the caracteristic I-V curve. See the web page of the tool; there you can find lots of usefull stuff, in terms of both theoric and practic. Click on the image on the left to see what we will achieve. We will use DC analisys, parameter sweep and equation functions of the tool. The project directory is also available here (must be copied to .qucs directory at the users home). Click here for Türkish version.
 
Assuming that you have Qucs installed, start the application. The main window which is very user friendly comes up. Here the tabs "Projects, Content, Components" are especially important; they hide a great amount of functionality.

The names listed as LLD, Mirrors and so on are my previous projects already developed.
Using Project > New Project menu item, create a new project in which our circuits will reside. Give a new as you wish.
See, on the Content tab, Schematics-DataDisplays-DataSets lines which will contain the schematics, the plots of our simulation results and the data sets respectively. Now we have a schematic entry window named untitled onto which we will put the circuit.

If you activate Projects tab, you must see the additional name silBeni since it is the last project created.
Using the Components tab, put all the items seen in the schematic :
  • nonlinear components > n-MOSFET
  • lumped components > Ground
  • sources > dc Voltage Source
  • simulations > dc simulation
  • simulations > Parameter sweep
Then wire them by using the wire tool box button which shows a 45 degree blue straight line (the one on the left side of "NAME" button).
Now we will set the parameters of the components. Double click on V2 and set U variable of the ideal dc voltage source to Vsweep; this is the parameter that we want to be swept. Redo the same thing for V1 but the value would be 0.6 V. (Note that one must click on Apply, OK does NOT apply before closing the window; I used QucsV07)
Set nMOS parameters. Double click on it, list of the modelled parameters and their current values comes up. Set Lambda to 0.4 and click Apply. As seen from the list, if one does not set parameters like that (they are either 1 or 0, that is, un-effective) simply they are not used. I find this very usefull because one can observe the effects of each model parameter on the simulation results. If you keep the initial value of Lambda as it was (zero) a perfect I-V curve would be produced.
Setting the dc simulation parameters. Double click on the dc simulation box that we just put on the left bottom side in the schematic view. I kept the inital values as they are here since they look convenient. The name of our dc simulation is DC1 that is to be used in the next step.
Selsect the parameter sweep options. Double click on the related box within the schematic view. Set the name of the simulation to DC1 that tells Qucs that the dc parameters will be calculated by DC1 object so that Qucs will know who to ask for the dc calculation. Then set the parameter name as Vsweep; this is the value of V2 ideal voltage source in our schematic. I wanted Vdd to be 1.5V. Set the start-stop-step values and the Number is calculated automatically. This is basically the resolution of our simulation. The bigger this number is, the longer you wait :) but the better results you would have.
Use the Simulation > Simulate menu item on the menu bar to start the simulator. If everything is ok, you can browse the output log by Simulations > Show Last Messages. According to this output, there is no error.
After lightning-fast simulation step, a new tab named *.dpl becomes visible. This view waits us to put plots on it.

Using the Components > diagrams, select a Cartesian object. Click on the empty area. An empty plot is created. Double click on the empty plot and see the next step.
You will see the plottable variables on the left side and selected variables on the right. Double click on V2.I (or on whatever the name of your item) on the left and it is transfered to the right side. Set other trivial parameters like color and thickness and click on Apply. You can also set the limits of the plot by hand but now we do not need such an operation that can be very annoying sometimes.
And we have the plot. The polarity of current depends on how you plot the valiable. This is the current that is sinked from V2 source in the schematic. Note that the transition between lineer and saturation regions is not as smooth as we expect. This is basically because of the number of steps of the dc sweep. We will fix this later.
Using the related tool bar button (the one on which M1 is written), you can put markers on the curves plotted. At this point you can verify, from the two points that the variable lambda is 0.4; this is where this tool is very handy for me : it gives exactly what you calculate by hand, provided that you set device parameters accordingly. Event hough, this sounds very normal, it is never the case for commercial simulators since they use extremely complicated models that are extracted for a specific technology. So sometimes you loose the taste of the initial design phase :) in which everything is under control.

For having the idea on how to do the verification mentioned above, you can also see another tutorial performed with another tool but the idea is exactly the same. (See especialy Method #1 in that tutor)

But we will do the same thing here in this tutorial as well. It is at the end of this page. We will use the equation functionality of the tool. Now just continue with the next step.
To improve the result, now set the Number to 160 in the dc sweep simulation box as we did one of the previous steps. See that the Step field is re-calculated automatically.
Re-simulate as you did before and see that the transition is better. (Set lambda to zero again and re-simulate to see a "perfect" I-V curve)
Play with the tool; the best way to learn a tool is to use it. Not all the plot types are possible for all types of simulations but as an example I put Components > Diagrams > Tabular object. It shows the numerical values for V2.I, that is, the current flowing through ideal dc voltage source V2.
Using the equation functionality : put an equation entry by using the related tool bar button (the one on the right of "NAME" button).

Background : Remember the simplified saturation region Id expression :

solve this for lambda :

We will use this expression to plot lambda as a function of Vds. Now double click on the equation box and see the next step.
Enter the equations. On the right side of the window, there are two entry spaces. The above one represents the left side of the equation and the below one represents the right side of the equation. In this window, Id=V2.I means that we declare Id as the current flowing through the ideal voltage sourge named V2. Id itself is used in the lambda expression. Diff is one of the functions the tool provides, stands for differentiation. See the official documents of Qucs for a complete reference.
Re-simulate the circuit. This time the equations will be handled. Create a plot as you did in one of the previous steps. Double click on it and you will see the items from the equation entry in the plot details window as seen here. Select lambda by double clicking on it.
Here is the result. The lamda is what we set which is 0.4; it is constant over a wide range. You can also put plots on the schematic view in case of pretty output on one page is required. Also see another tutorial performed by a commercial simulator here. See especially the Method #2 in that tutor.
 
Özgür Çobanoğlu