Spectrum Software
spacer
Industrial Strength Simulation
select:

divider

 

News:

Spectrum Software has released Micro-Cap 11, the eleventh generation of our SPICE circuit simulator.

For users of previous Micro-Cap versions, check out the new features available in the latest version. For those of you who are new to Micro-Cap, take our features tour to see what Micro-Cap has to offer.

 

divider

 

Using the Make Subcircuit Option

 

There are two model types within Micro-Cap that let the behavior of a complex circuit block be incorporated into and represented by a single component in a schematic. These model types are the macro and the subcircuit. The main difference between these two types is that a macro has its circuitry defined through a schematic whereas the subcircuit has its circuitry defined through a SPICE text netlist.

While the macro is typically the easier model type to create, it is limited to use in only the Micro-Cap simulator. Though the text description of a subcircuit model is more difficult to develop, a subcircuit can be transferred to any other application that is capable of handling the SPICE netlist format. This portability is the main advantage to using a subcircuit model.

To ease the difficulties in creating a SPICE netlist, Micro-Cap provides a translation feature to convert schematic files into SPICE netlists. One of the options within this translate to SPICE feature is the ability to create a subcircuit model out of the schematic rather than the full SPICE circuit file that is normally produced. This article will describe the process of taking a schematic and converting it into its subcircuit equivalent.

The first step is to create the schematic that will represent the appropriate model. The schematic should only contain the components that will be part of the model as all of the components within the schematic will be incorporated into the subcircuit. For this example, the schematic to be used appears below. This schematic models a basic Wien bridge oscillator that produces about a 9kHz output sine wave. The desired input and output nodes for the model have been labelled with text. The power supplies for the opamp have been called Vcc and Vee, and the output is simply labelled Out.

Wien Bridge Oscillator

Once the schematic is ready, click on the File menu, select Translate and choose the Schematic to SPICE Text File option. The Translate to SPICE dialog box that is invoked is displayed in the figure below.

Translate to SPICE Dialog Box

Enabling the Make SUBCKT in the Options section will force the translation to create a subcircuit model in a library file. Both the Analysis section and the .Options option will be disabled since these are only available for a full circuit netlist.

The Spice type section determines the SPICE format that the subcircuit will be created in. The three options are: SPICE 2G, PSpice, and SPICE3. The selection here would depend on the type of syntax that any other programs that may access the subcircuit can handle. Micro-Cap is capable of handling all three of these formats.

The Report option will place a section of comments in the library file detailing the components that the subcircuit is comprised of. This will have no effect on the actual operation of the subcircuit. The Expand SUBCKT option will place all subcircuit or macro models that the active schematic references into the library file as separate subcircuit models. This option localizes all the model information for the main subcircuit model into the specified library file. The Add To Nom.lib option will add a reference for the library file that is being created into the NOM.LIB file. The NOM.LIB file contains a list of library files that Micro-Cap will automatically access. This option should be enabled if the new subcircuit model may be used within Micro-Cap.

The File field contains the path and name of the library file to be created. For Micro-Cap use, the library file should be created with a .LIB extension.

The SUBCKT Name field specifies the name of the subcircuit model. The name must be a single string with no spaces.

The SUBCKT Pins field defines the nodes that the subcircuit will use for its input and output connection pins. The pins should be node names or node numbers from the schematic and should be separated by commas or spaces in the list. If you have named the node in the schematic with a text label, you must use the name rather than the corresponding node number since the text name has priority when the translation occurs.

Clicking on the OK button initiates the translation with the specified settings. The new library file will then be loaded in Micro-Cap. For the Wien Bridge Oscillator example, the subcircuit produced is:

.SUBCKT Wien Vcc Vee Out
C1 Out 4 16N
C2 3 0 16N
R3 3 4 1K
R4 0 3 1K
RA 0 1 1K
RF 1 Out 2.1K
X1 3 1 Vcc Vee Out UA741_TI
.ENDS Wien

Note that in the .SUBCKT line above the name of the model is Wien and the pin names are Vcc, Vee, and Out as was specified in the Translate to SPICE dialog box. To include the UA741_TI model that the Wien subcircuit references in the same library file, the Expand SUBCKT options would have needed to be enabled.

When the Make SUBCKT option is selected, the translation will also create an entry for the new subcircuit in the component library so that this part will be available for placement in a schematic. The new entry is placed in the SUBCKT.CMP file in the main MC8 directory, and the component will now be accessible through a Subckt group on the first level of the Component menu.

Since Micro-Cap does not inherently know the function of the subcircuit, the new component entry uses the AutoMacro shape. This shape provides a resizeable rectangle where the pins can be moved through a drag operation. Typically, one would want to edit the entry so that it uses a more recognizable shape that exists in the shape library prior to placing this part in a schematic. To do this, just enter the Component Editor, and select the entry that was created for this subcircuit. It will be present in the Subckt.cmp section of the component tree on the right hand side of the dialog box. Once selected, just change the Shape reference for the part and then move the pin connections to the appropriate parts of the shape. If none of the existing shapes are appropriate for the subcircuit, a new shape would need to be created in the Shape Editor.

Assuming the Add To Nom.lib option was enabled for the translation, this subcircuit is now ready to be used in a Micro-Cap simulation. If the Add To Nom.lib was disabled, the Nom.lib file would then need to be manually edited or an explicit reference to the new library, such as with a .lib statement, would need to be defined in the schematic that is using the subcircuit component before this subcircuit would be available for simulation.

A simple test circuit has been set up to test the Wien bridge oscillator. Fixed Analog components have been used to place twelve volts at the Vcc pin and minus twelve volts at the Vee pin. The transient analysis output of the oscillator is displayed below.

Wien Bridge Oscillator Output

The transient simulation has been run over a time range of 20ms. The output produces a sine wave shape whose peaks and valleys are flattened due to saturation at the output rails of the UA741 opamp referenced within the oscillator. The output frequency of the sine wave is measured to be approximately 8.74kHz.

 
Return to the main Newsletter page