Generic Parts

In this Topic ShowHide

As explained in the overview generic parts are devices that are defined by one or more parameters entered by the user after the part is placed. The following generic parts are available:

SIMPLIS Primitive Parts

The following parts are only available with the SIMetrix/SIMPLIS product and when in SIMPLIS. They can all be found under the menu Place ▶ SIMPLIS Primitives. For full details, see the SIMPLIS Reference Manual.

Saturable Inductors and Transformers

SIMetrix is supplied with a number of models for inductors and transformers that correctly model saturation and, for most models, hysteresis. As these parts are nearly always custom designed there is no catalogue of manufacturers parts as there is with semiconductor devices. Consequently a little more information is needed to specify one of these devices. This section describes the facilities available and a description of the models available.

Core Materials

The available models cover a range of ferrite and MPP core materials for inductors and transformers with any number of windings. The complete simulation model based on a library core model is generated by the user interface according to the winding specification entered.

Placing and Specifying Parts

1. Select the menu Place ▶ Magnetics ▶ Saturable Transformer/Inductor... You will see the following dialog box:

   

2. Specify the number of windings required for primary and secondary in the Configuration section. If you just want a single inductor, set primary turns to 1 and secondaries to 0.
3. Specify turns ratios in the Define Windings section. You can select the winding to define using the Select Winding drop down box then enter the required ratio to primary 1 in the edit box below it.
4. Specify the number of turns for the primary and coupling factor. The coupling factor is the same for all windings. You can define different coupling factors for each winding by adding ideal inductors in series with one or more windings. In some instances it may be necessary to add coupled inductors in series. This is explained in more detail in Coupling Factor.
5. Specify the core characteristics in the Define Core section. A number of standard core sets are pre-programmed and can be selected from the Select Core Type list at the top. If the part you wish to use is not in the list or if you wish to use a variant with a - say - different air gap, you can manually enter the characteristics by clicking on the Manual Entry check box.

Model Details

The models for saturable magnetic parts can be found in the file cores.lb. Most of the models are based on the Jiles-Atherton magnetic model which includes hysteresis effects. The MPP models use a simpler model which does not include hysteresis. These models only define a single inductor. To derive a transformer model, the user interface generates a subcircuit model that constructs a non-magnetic transformer using controlled sources. The inductive element is added to the core which then gives the model its inductive characteristics.

The model does not currently handle other core characteristics such as eddy current losses nor does it handle winding artefacts such as resistive losses, skin effect, inter-winding capacitance or proximity effect.

Ideal Transformers

Ideal transformers may be used in both SIMetrix and SIMPLIS modes. Note that SIMPLIS operation is more efficient if the coupling factors are set to unity.

To define an ideal transformer, select the menu Place ▶ Passives ▶ Ideal Transformer.... This will open the following dialog box:

Configuration

Specify the number of primaries and secondaries. You can specify up to 20 of each.

Define turns ratio

Inductance and coupling

This method of implementing an ideal transformer is not totally general purpose as you cannot arbitrarily define inter winding coupling factors. If you need a configuration not supported by the above method, you can define any ideal transformer using ideal inductors and the Mutual Inductance device. The SIMetrix version is explained in the next section. For the SIMPLIS equivalent, see the SIMPLIS reference manual.

DC Transformers

The DC transformer model is like a normal transformer except that it has - in effect - infinite inductance. So it will work at DC and has zero magnetisation current. To place a DC transformer, select menu Place ▶ Magnetics ▶ Ideal DC Transformer.... This will open the following dialog box:

Configuration

Specify the number of primaries and secondaries. You can specify up to 20 of each.

Define turns ratio

Coupling Factor

The standard user interface for both saturable and ideal transformers provide only limited flexibility to specify inter-winding coupling factor. In the majority of applications, coupling factor is not an important issue and so the standard model will suffice.

In some applications, however, the relative coupling factors of different windings can be important. An example is in a flyback switched mode supply where the output voltage is sensed by an auxiliary winding. In this instance, best performance is achieved if the sense winding is strongly coupled to the secondary. Such a transformer is likely to have a different coupling factor for the various windings.

You can use external leakage inductances to model coupling factor and this will provide some additional flexibility. One approach is to set the user interface coupling factor to unity and model all non-ideal coupling using external inductors. In some cases it may be necessary to couple the leakage inductors. Consider for example an E-core with 4 windings, one on each outer leg and two on the inner leg. Each winding taken on its own would have approximately the same coupling to the core and so each would have the same leakage inductance. But the two windings on the centre leg would be more closely coupled to each other than to the other windings. To model this, the leakage inductances for the centre windings could be coupled to each other using the mutual inductor method described in the next section.

Mutual Inductors

You can specify coupling between any number of ideal inductors, using the mutual inductor device. There is no menu or schematic symbol for this. It is defined by a line of text that must be added to the netlist. (See Manual Entry of Simulator Commands). The format for the mutual inductance line is:

Where:

Note

If more than 2 inductors are to be coupled, there must be a K device to define every possible pair.

Examples

Resistors

Resistors may be used in both SIMetrix and SIMPLIS modes. Note that in SIMetrix mode a number of additional parameters may be specified. These will not work with SIMPLIS and must not be specified if dual mode operation is required.

Select from Place ▶ Passives menu.

To edit value use F7 or select popup menu Edit Part... menu as usual. This will display the following dialog for resistors.

Additional Parameters

Press Parameters... button to edit additional parameter associated with the device such as temperature coefficients (TC1, TC2). Refer to device in the Simulator Reference Manual for details of all device parameters.

Ideal Capacitors and Inductors

Capacitors and inductors may be used in both SIMetrix and SIMPLIS modes. Note that in SIMetrix mode a number of additional parameters may be specified. These will not work with SIMPLIS and must not be specified if dual mode operation is required.

The following dialog will be displayed when you edit a capacitor or inductor:

The device value is edited in the same manner as for resistors. You can also supply an initial condition that defines how the device behaves while a DC operating point is calculated. For capacitors you can either specify that the device is open circuit or alternatively you can specify a fixed voltage. For inductors, the device can be treated as a short circuit or you can define a constant current.

Infinite Capacitors and Inductors

The infinite capacitors and inductors are often useful for AC analysis.

To place an infinite capacitor, select menu Place ▶ Passives ▶ Infinite Capacitor To place an infinite inductor, select menu Place ▶ Magnetics ▶ Infinite Inductor

The infinite capacitor works as follows:

1. During the DC bias point calculation, it behaves like an open circuit, just like a regular finite capacitor.
2. During any subsequent analysis it behaves like a voltage source with a value equal to the voltage achieved during the DC bias point calculation.

1. During the DC bias point calculation, it behaves like a short circuit, just like a regular finite inductor.
2. During any subsequent analysis it behaves like a current source with a value equal to the current achieved during the DC bias point calculation.

The infinite capacitor is a built in primitive part and is actually implemented by the voltage source device. The infinite inductor is a subcircuit using an infinite capacitor and some controlled sources.

Multi-Level Capacitors

The Multi-Level Capacitor has four model levels. As the level increases, additional parasitic circuit elements are added. This capacitor, available with Version 8.0 or later, is used to model a wide variety of capacitor types where the number and type of parasitic circuit elements can be configured.

Editing the Multi-Level Capacitor

To configure the Multi-Level Capacitor, follow these steps:

1. Double click the symbol on the schematic to open the editing dialog to the Parameters tab.
2. Choose a model level, and then make the appropriate changes to the fields described in the table below the image.

1. Click on the Monte Carlo Parameters tab.
2. Make the appropriate changes to the fields described in the table below the image.

Multi-Level Capacitor Model Levels

The Multi-Level capacitor has four levels: 0, 1, 2, and 3. As the model level increases, additional parasitic circuit elements are added to the model.

The diagram below shows the circuit used for each of the four levels:

Quantity Implementation - SIMPLIS Mode

The Multi-Level Capacitor model has two quantity parameters, USE_QTY and QTY, which specify the number of capacitors in parallel.

Configuring these parameters minimizes the number of reactive circuit elements in the model and, therefore, provides a maximum simulation speed.

The implementation of the quantity parameter uses a "DC Transformer" technique where the capacitor's terminal current is multiplied by a constant using a Current Controlled Current Source (CCCS). This technique effectively divides all resistance and inductance values by the quantity parameter (QTY) and multiplies the capacitance by that same value. This circuitry is added if the USE_QTY parameter is set to 1.

A schematic of the quantity implementation for a Level 0 Multi-Level Capacitor is shown below:

Quantity Implementation - SIMetrix Mode

In SIMetrix, the quantity parameter is implemented with the "M" parameter which is common to the primitive SPICE components. This improves SIMetrix simulation speed and correctly scales resistances for noise analysis.

Electrolytic Capacitors

The electrolytic capacitor model has been superseded by the Multi-level Capacitor. The electrolytic capacitor is still available from the parts selector at locations Passives -> Capacitors, Simple (Legacy) and Passives -> Capacitors, Detailed (Legacy)

Electrolytic capacitor models are shown below:

Passives -> Capacitors, Simple (Legacy)

Potentiometer

The potentiometer may be used in both SIMetrix and SIMPLIS modes. To place, select the menu Place ▶ Passives ▶ Potentiometer. This device can be edited in the usual manner with F7/Edit Part... popup. This will display:

Check Run simulation after position change if you wish a new simulation to be run immediately after the wiper position changes.

The potentiometer's wiper position may also be altered using the shift-up and shift-down keys while the device is selected. Edit Inc/dec step size to alter the step size used for this feature.

Lossless Transmission Line

Select from menu Place ▶ Passives ▶ Trans. Line (Lossless) or press hot key 'T'. Editing in the usual way will display:

Lossy Transmission Line

Select from menu Place ▶ Passives ▶ Trans. Line (Lossy RLC). Editing in the usual way will display:

Enter parameters as indicated. The absolute tolerance and relative tolerance parameters control the accuracy/speed trade-off for the model. Reduce these values for greater accuracy.

Fixed Voltage and Current Sources

See Circuit Stimulus.

Controlled Sources

There are four types which can be found under menu Place ▶ Controlled Sources:

• Voltage controlled voltage source or VCVS
• Voltage controlled current source or VCCS
• Current controlled voltage source or CCVS
• Current controlled current source or CCCS

These have a variety of uses. A VCVS can implement an ideal opamp; current controlled devices can monitor current; voltage controlled devices can convert a differential signal to single ended.

They require just one value to define them which is their gain. Edit value in the usual way and you will be presented with a dialog similar to that used for resistors, capacitors and inductors but without the Parameters... button.

Voltage Controlled Switch

This is essentially a voltage controlled resistor with two terminals for the resistance and two control terminals. Place one on the schematic with Place ▶ Analog Functions ▶ Switch. Editing using F7 or equivalent menu displays:

If the control voltage lies between the On Voltage and Off Voltage the resistance will be somewhere between the on and off resistances using a law that assures a smooth transition between the on and off states. Refer to Simulator Reference Manual/Analog Device Reference/Voltage Controlled Switch

Switch with Hysteresis

An alternative switch device is available which abruptly switches between states rather than following a continuous V-I characteristic. This device can be used with both SIMetrix and SIMPLIS although the behaviour is slightly different in each. The switching thresholds are governed by an hysteresis law and, when used with the SIMetrix simulator, the state change is controlled to occur over a defined time period which can be edited.

This device can be placed on a schematic with the menu Place ▶ Analog Functions ▶ Switch with Hysteresis.

Parameters are:

If you need to control switch on times and switch off times independently, you can use the delayed switch model. See Delayed Switch.

Delayed Switch

Implements a voltage-controlled switch with defined on and off delay. This model can be used to implement relays. Switch action is similar to the Switch with Hysteresis described above. The delayed switch model has all the functionality of the hysteresis switch with the addition of time delay parameters and separate parameters for switch on and switch off times. Unlike the hysteresis switch, this device does not have an exact SIMPLIS equivalent.

This device can be placed on a schematic with the menu Place ▶ Analog Functions ▶ Delayed Switch.

Parameters are:

Parameterised Opamp

Implements an operational amplifier and is available from menu This is available from menu Place ▶ Analog Functions ▶ Parameterised Opamp. It is defined by the parameters listed below.

Parameterised Opto-coupler

Implements a 2-in 2-out optically isolated coupler. This is available from menu Place ▶ Analog Functions ▶ Parameterised Opto-coupler. It is defined by just two parameters described in the following table:

Parameterised Comparator

Implements a simple differential comparator. This is available from menu Place ▶ Analog Functions ▶ Parameterised Comparator. Its parameters are defined in the following table:

VCO

Implements a simple voltage controlled oscillator with a digital output. You can place a VCO on the schematic using menu Place ▶ Digital Generic ▶ VCO (Analog in, digital out). Its parameters are:

Verilog-A Library

If you have a SIMetrix Pro or SIMetrix Elite you may also use one of the Verilog-A implemented devices available under the Place ▶ Analog Functions ▶ Verilog-A Library. These devices are defined using the Verilog-A language. The Verilog-A code for these devices may be found in the support\ valibrary directory under the SIMetrix root.

Currently there are 4 Verilog-A library devices as described in the following paragraphs.

Voltage Controlled Delay

Implements a variable analog delay.

This device has three parameters as defined in the table below. Double click the device to edit its parameters.

Fixed Delay

Implements a fixed analog delay

This device has just a single parameter defining its delay in seconds. Double click the device to edit.

Sinewave VCO

Implements a sinewave voltage controlled oscillator. This has four parameters as defined below:

Pulse Width Modulator

Implements a voltage controlled pulse width. Defined by 6 parameters as follows:

Generic ADCs and DACs

Generic data conversion devices are available from the menus Place ▶ Digital Generic ▶ ADC... and Place ▶ Digital Generic ▶ DAC...

The controls in these boxes are explained below.

Number of bits

Resolution of converter. Values from 1 to32

Convert time (ADC)

Time from start convert active (rising edge) to data becoming available

Max conversion rate (ADC)

Max frequency of start convert. Period (1/f) must be less than or equal to convert time.

Output slew time

Whenever the input code changes, the output is set on a trajectory to reach the target value in the time specified by this value.

Offset voltage

Self-explanatory.

Range

Full scale range in volts.

Generic Digital Devices

A number of generic digital devices are provided on the Place ▶ Digital Generic menu. Each will automatically create a symbol using a basic spec. provided by your entries to a dialog box. Functions provided are, counter, shift register, AND, OR, NAND and NOR gates, and bus register.

Functional Blocks - Overview

The simulator supports a number of devices that are arbitrary in nature and which are used to define a device in terms of its function or behaviour. Functional blocks have a number of uses. Here are two examples:

1. System level simulation. You are investigating the viability or characteristics of a complete system before actually considering its implementation detail. Your system may consist of a number of interconnected blocks each with an easily defined function.
2. Device model implementation. Functional models can be used to actually create device models. Suppose you wish to use an op-amp for which no model is available. The only characteristic that affects the performance of your circuit is its gain bandwidth product. So instead of creating a detailed model you simply use a differential voltage amplifier with the appropriate GBW.

The simulator provides three devices that can be defined in a completely arbitrary manner. These are defined in the following table. See the Simulator Reference Manual for full details on these devices.

Schematic support for functional blocks is provided by a number of devices under the menus Place ▶ Analog Behavioural, Place ▶ Digital Generic. Devices currently provided are shown in the following table.

Non-linear Transfer Function

Select menu Place ▶ Analog Behavioural ▶ Non-linear Transfer Function. This displays:

You may specify an equation that defines an output voltage or current in terms of any number of input voltages and currents. Input voltages are specified in the form V(a) or V(a,b) where a and b may be any arbitrary name of your choice. Input currents are specified in the form I(a). On completion, SIMetrix will generate a schematic symbol complete with the input voltages and/or currents that you reference in the equation. Unlike earlier versions, there is no need to specify how many input voltages and currents you wish to use. SIMetrix will automatically determine this from the equation.

As well as input voltage and currents, you can also reference the output voltage or current in your equation. A single ended output voltage is accessed using V(out) while a differential output voltage is accessed using V(outp,outn). If you specify an output voltage, you may also access the current flowing through it using I(out).

In the example above, the expression shown - V(vina,vinb)*I(iin) - multiplies a voltage and current together. This could be used to monitor the power in a two terminal device as shown in the following schematic.:

In the above, ARB1 is the device created from the Non-linear Transfer Function menu. ARB1-OUTP will carry a voltage equal to the power dissipation in R1.

Expression

The expression may use arithmetic operators and functions as defined in Simulator Reference Manual/Simeulator Devices/Using Expressions.

Verilog-A Implementation

If you have SIMetrix Pro or SIMetrix Elite you may select the Compile to binary using Verilog-A option. This will build a definition of the device using the Verilog-A language then compile it to a binary DLL. This process takes place when you run the simulation. The benefit of using Verilog-A is that there is a wider range of functions available and for complex definitions there will also be a performance benefit. Refer to the Verilog-A Manual for details of available functions.

Laplace Transfer Function

Selecting the menu Place ▶ Analog Behavioural ▶ Laplace Transfer Function brings up the following dialog

Definition

Enter an expression using the 'S' variable to define the frequency domain transfer function. The above shows the example of a second order response. See Laplace Expression for details of the expression syntax.

Frequency scale factor

Multiplier for frequency

Device type

Input

Input configuration for transfer function

Output

Output configuration for transfer function

Laplace Expression

When you close the box, a symbol will be created according to the selections you make for device type, input and output.

As seen in the above examples, the transfer function of the device is defined by the model parameter LAPLACE. This is a text string and must be enclosed in double quotation marks. This may be any arithmetic expression containing the following elements:

Operators

Constants

Any decimal number following normal rules. SPICE style engineering suffixes are accepted.

S Variable

This can be raised to a power with '\^' or by simply placing a constant directly after it (with no spaces). E.g. s^2 is the same as s2.

Filter response functions

These are described in the following table:

Using Parameters with Laplace Devices

Currently it is not possible to use parameters (defined with .PARAM) in Laplace expressions. You can, however, use parameters in the underlying simulator device if you define the expression in terms of the numerator and denominator coefficients. Refer to the S-domain Transfer Function Block in the Simulator Reference Manual for further details.

Arbitrary Non-linear Passive Devices

Each of these will place a part which looks exactly like its linear counterpart. The difference is that when you try and edit its value with F7 or menu Edit Part... you will be prompted to enter an expression. In the case of the resistor and capacitor, this relates its value to the applied voltage and for inductor the expression relates its inductance to its current. For resistors and capacitors, the terminal voltage is referred in the equation as 'V(N1)' and for inductors the device's current is referred to as 'I(V1)'.