AnsweredAssumed Answered

Walkthrough: DC, Linear, HARBEC, parameter sweeps

Question asked by pkarasev on Aug 2, 2005
Latest reply on Aug 2, 2005 by pkarasev
The following is a walk-through on using DC analysis, basic HARBEC functions, and parameter sweeps. This is contained in the simulation manual (available in online help) but there is no workspace file and  this post contains some more detail. At the end of the post you can find the workspace, and all instructions are also in the notes in the .wsp

1) From the non-linear toolbar or parts selector add a "NPN Bipolar Gummel-Poon"

2) Add a DC current source from the "basic" menu in the parts selector. Change the 'Designator' to "IB" and set the 'DC Current' to "IDC".

3) Add a 'Current Probe (Ammeter)' from the basic menu in the parts selector. Change the 'Designator' to "IC".

4) Add a 'Signal Ground' from the basic menu in the parts selector. Change the 'Designator' to 'VC' and reference a variable for the 'DC Voltage' by typing in 'V'.

5) Create the equations:


6) Add a DC analysis by clicking the "new" icon in the design manager. Check "annonate" in the properties. If it does not automatically run, right click "DC1" in the analysis folder and delete internal data,  then re-run it. You should see the voltages at each node at DC appear on the schematic.

7) Create a parameter sweep using the 'new' button and 'Add Parameter Sweep' under the analysis sub-menu. Name the Sweep "Vc Sweep". Sweep simulation DC1 and variable "V" from 0 to 3 with 20 points linear.

8 ) Create another parameter sweep and name it "IB Sweep" which will sweep the other sweep. The simulation to sweep is then "Vc Sweep" and the variable is "IDC" from 2e-6 to 10e-6 with 5 points linear.

9) Click New -> Output -> Add rectangular graph. Double click it to setup the properties. Change the simulation to use to "IB Sweep.Sch1". You can enter "iic" which means current in IC (remember that we named the current probe's designator IC") or you can click the measurement wizard, select the second sweep, then choose "current at node" and select "IIC" (or any other measurement you wish to see). Un-check autoscale on the left y-axis and set it to go from 0 to 1.25e-3; the resulting graph is shown in this workspace.

Part II

Copy the schematic that was made into a new schematic called "DC Bias". Here we are using a collector voltage of 2.5 volts and an Ic of 10mA.

1) Modify the schematic as seen here; the resistors are both set to 300 ohms and are made tuneable in their property windows. The supply voltage should now be fixed to 5 volts; double click it in the second schematic and set it equal to 5 volts instead of V. (If you just change V in the equations to 5 non-tuneable, you'll break the parameter sweeps from before)

2) Double click the DC analysis to open the properties and check "annotate" for the second schematic. You should see the voltages at each node appear; notice that the collector node is currently not 2.5 V as we want to make.

3) Add an optimization by clicking on "New" , "add optimization". In the properties, the simulation to use by default is DC1.DC Bias    (AnalysisName.SchematicName). We want the voltage at node 4 (v4) to equal 2.5, while the current at "IC" is to be made 10mA. So the setting are:

v4 = 2.5   with weight of 1
iic = 10e-3 with weight of 100 (we increase the weight because we care about it more)

Click optimize now, least squares automatic. (About different ways of optimizing: ... ic?id=1454 )

When the rate of change of error is so small that it would not be practical to implement physically, click stop on the optimizer.

Part III:

1)Copy the DC Bias schematic into a new schematic called "Amplifier".

2) Set the resistors to whole numbers, ie 16500 and 250.

3) Add 100pF capacitors in series with the input and output ports to block the DC.

4) Add an input port that is AC Power (from the 'Basic' menu in the parts selector), with a frequency of 900MHz and pow