Circuit Simulation Techniques in Altium Designer

Altium Designer's mixed circuit signal simulation tool implements functional design simulation of mixed-signal circuits in the circuit schematic design stage, and completes analysis based on various data such as timing, discreteness, and signal-to-noise ratio with a simple and easy-to-use parameter configuration window. Altium Designer can provide comprehensive mixed-signal circuit simulation functions in schematics. In addition to supporting the XSPICE standard, it also supports simulation of Pspice models and circuits. The circuit simulation in Altium Designer is a true mixed-mode simulator that can be used for circuit analysis of analog and digital devices. The simulator uses an enhanced event-driven XSPICE simulation model developed by the Georgia Institute of Technology (GTRI), which is based on the Berkeley SPICE3 code and is fully compatible with SPICE3f5.

SPICE3f5 simulation device models: including resistors, capacitors, inductors, voltage/current sources, transmission lines and switches. Five major types of common semiconductor device models, such as diodes, BJTs, JFETs, MESFETs and MOSFETs.

XSPICE simulation device models are complex, nonlinear device characteristic model codes designed for some lengthy local circuits that may affect simulation efficiency. They include special functions such as gain, hysteresis, voltage and current limits, s-domain transfer function accuracy, etc. Local circuit models refer to more complex devices, such as operational amplifiers, clocks, crystals, etc., which are described in local circuit syntax. Each local circuit is downloaded in a *.ckt file, and a capital X is added in front of the model name.

The digital device model is written in the digital SimCode language, which is a special description language extended from the event-driven XSPICE model and specifically used to simulate digital devices. It is a C-like language that describes the behavior and characteristics of digital devices. Parameters can include information such as transmission delay and load characteristics; behavior can be controlled by truth tables, mathematical functions, and conditional parameters. It is derived from the standard XSPICE code model. In SimCode, simulation files use ASCII code characters and are saved as files with a .TXT suffix. After compilation, *.scb model files are generated. Multiple digital device models can be written in the same file.

1. Establishment of simulation circuit and connection with simulation model

Since AD ​​uses integrated library technology, the corresponding simulation model is included in the schematic symbol, so the schematic can be used directly as a simulation circuit, while the simulation circuit in 99SE needs to be established separately and the simulation model of each component needs to be loaded separately.

2. Addition of external simulation models

AD provides a large number of simulation models, but in actual circuit design, the simulation model set still needs to be supplemented and improved. On the one hand, users can edit the simulation model files that come with the system to meet simulation needs. On the other hand, users can directly import external standard simulation models into the system as part of the integrated library and then perform circuit simulation directly in the schematic diagram.

3.Simulation function and parameter setting

Altium Designer's simulator can perform various forms of signal analysis. In the simulator's analysis settings dialog box, the global settings page allows users to specify the scope of the simulation and automatically display the simulated signals. Each analysis type can be completed in a separate settings page. The analysis types allowed in Altium Designer include:

1. DC operating point analysis

2. Transient analysis and Fourier analysis

3. AC small signal analysis

4. Impedance characteristics analysis

5. Noise analysis

6. Pole-Zero (critical point) analysis

7. Transfer function analysis

8. Monte Carlo Analysis

9. Parameter Sweep

10. Temperature scanning, etc.

1. DC operating point analysis: DC operating point analysis is used to determine the DC operating point of a circuit with short-circuit inductance and open-circuit capacitance.

When determining transient initialization conditions, DC operating point analysis takes precedence over transient analysis, except when the Use Initial Conditions parameter has been enabled in Transient/Fourier Analysis Setup. Also, DC operating point analysis takes precedence over AC small signal, noise, and Pole-Zero analysis, to ensure linearity of the determination, all nonlinear small signal models in the circuit. Any interference from AC sources will not be considered in the DC operating point analysis.

2. Transient analysis: Transient analysis describes the values ​​of transient output variables in the time domain. When the Use Initial Conditions parameter is not enabled, for fixed bias points, the initial values ​​of the circuit nodes are also taken into account when calculating the bias points and small signal parameters of nonlinear elements. Therefore, capacitors and inductors with initial values ​​are also considered as part of the circuit and retained.

Parameter settings

Transient Start Time: The starting value of the time interval set during analysis (unit: seconds)

Transient Stop Time: The end value of the time interval set during analysis (unit: seconds)

Transient Step Time: Time increment (step length) value during analysis

Transient Max Step Time: The maximum change in the time increment value; by default, its value can be Transient Step Time or (Transient Stop Time – Transient Start Time)/50.

Use Initial Conditions: When enabled, the transient analysis will start from the initial conditions defined in the schematic, bypassing the DC operating point analysis. This option is usually used to start a transient analysis from a static operating point.

Use Transient Default: Call the default settings

Default Cycles Displayed: The number of sine wave cycles displayed by default. This value will be determined by the Transient Step Time.

Default Points Per Cycle: The number of data points displayed per sine wave cycle.

If the user has not determined the specific input parameter values, it is recommended to use the default settings; when using the initialization conditions defined in the schematic, it is necessary to make sure that the initialization conditions have been defined on each appropriate component in the circuit design, or to place .IC components in the circuit.

3. Fourier Analysis: Fourier analysis of a design is done based on the data from the last cycle of the transient analysis.

Parameter settings

Enable Fourier: Perform Fourier analysis in the simulation (Disable by default)

Fourier Fundamental Frequency: The signal frequency value approximated by the superposition of sine curve waves

Fourier Number of Harmonics: The number of harmonics to be considered in the analysis; each harmonic is an integer multiple of the fundamental frequency.

After performing the Fourier analysis, the system will automatically create a .sim data file containing detailed information about the amplitude and phase of each harmonic.

4. DC sweep analysis: DC sweep analysis is the DC transfer characteristic, which outputs a curve trajectory when the input changes within a certain range. By performing a series of DC operating point analyses, the voltage of the selected source signal is modified to obtain a DC transfer curve; users can also specify two working sources at the same time.

Parameter settings

Primary Source: The name of the independent power source in the circuit

Primary Start: The starting voltage value of the main power supply

Primary Stop: The stop voltage value of the main power supply

Primary Step: The increment value specified within the scan range

Enable Secondary: Performs a scan analysis of each slave power supply value based on the master power supply.

Secondary Name: The name of the second independent power supply in the circuit

Secondary Start: Starting voltage value from the power supply

Secondary Stop: Stop voltage value from the power supply

Secondary Step: The increment value specified within the scan range

In DC sweep analysis, a primary source must be set, while a second source is optional; usually the interval covered by the first sweep variable (primary independent source) is the inner loop, and the second (secondary independent source) sweep interval is the outer loop.

5. AC small signal analysis: AC analysis is to calculate the circuit and response within a certain frequency range. If the circuit contains nonlinear devices or components, the AC small signal parameters of this component should be obtained before calculating the frequency response. Before performing AC analysis, it is necessary to ensure that there is at least one AC power source in the circuit, that is, set a value greater than zero in the AC attribute field in the excitation source.

Parameter settings

Start Frequency: Initialization frequency for the sine wave generator (unit: Hz)

Stop Frequency: The cut-off frequency used for the sine wave generator (unit: Hz)

Sweep Type: determines how to generate the number of test points; Linear-all test points are evenly distributed within the linear test range, and are linearly swept from the start frequency to the end frequency. The Linear type is suitable for narrow bandwidths; Decade-test points are arranged in a logarithmic form of 10, and Decade is used for particularly wide bandwidths; Octave-test points are arranged in a logarithmic form of 8 times 2, and the frequency is logarithmically swept in octaves. Octave is used for wide bandwidths;

Test Points: Define the incremental value within the scan range according to the selected scan type;

Total Test Point: Displays the number of all test points;

Before performing AC small signal analysis, the circuit schematic must contain at least one signal source device and a value should be entered in the AC Magnitude parameter. Use this signal source to replace the sine wave generator during simulation. The amplitude and phase of the sine wave used for the sweep must be specified in the SIM model. Enter the amplitude value (Volt) and the phase value (Degrees). No unit value is required. Setting the AC Magnitude to 1 will cause the output variable to display a correlation of 0dB.

6. Impedance characteristic analysis: Impedance characteristic analysis will display the impedance characteristics between any two terminal sources in the circuit. This analysis does not have an independent setting page and is usually only used as a part of AC small signal analysis.

Parameter settings

The impedance measurement will be obtained by dividing the input supply voltage by the output current. To obtain an impedance characteristic diagram of the output impedance of a circuit, the following steps must be performed:

Remove source from input

Short-circuit the input power supply and ground

Remove any load connected to the circuit

Connect the source across the output, i.e. the positive supply is connected to the output and the negative terminal is grounded

7. Noise Analysis: Noise analysis uses noise spectral density to measure the noise contribution from resistors and semiconductor devices, usually characterized by V2/Hz. Resistors and semiconductor devices, among others, can generate noise, and the noise level depends on the frequency. Resistors and semiconductor devices generate different types of noise (Note: in noise analysis, capacitors, inductors, and controlled sources are considered noise-free components). For each frequency of the AC analysis, the noise level of each noise source (resistor or transistor) in the circuit is calculated. They are obtained by adding the RMS values ​​as contributions to the output node.

Parameter settings

Output Noise: Output node that needs to analyze noise

Input Noise: The total amount of noise superimposed on the input end will directly affect the noise value at the output end

Component Noise: The sum of the noise caused by each device in the circuit (including resistors and semiconductor devices) to the output multiplied by the gain.

Noise Sources: Select a reference source for calculating noise (either an independent voltage source or an independent current source).

Start Frequency: specifies the starting frequency;

Stop Frequency: specifies the stop frequency;

Test Points: specifies the number of points to scan;

Points/Summary: Specifies the noise range for calculation. In this area, enter 0 to calculate only the input and output noise; enter 1 to calculate the noise of each device at the same time. The latter is suitable for users who want to view the noise of a certain device separately and perform corresponding processing (for example, if the noise of a certain device is large, consider replacing it with a low-noise device).

OutPut Node: specifies the output noise node;

Reference Node: specifies the output noise reference node. This node is usually the ground (also known as the 0 node). If other nodes are set, the total output noise is obtained by V (Output Node) - V (Reference Node);

In the Sweep Type box, specify the sweep type. These settings are similar to those for AC analysis and are only briefly described here. Linear is a linear sweep, which is a linear sweep from the start frequency to the end frequency. Test Points is the total number of points in the sweep, and a frequency value is obtained by adding a constant to the current frequency value. Linear is suitable for situations with narrow bandwidths. Octave is an octave sweep, in which the frequency is swept logarithmically in octaves. Test Points is the number of sweep points within an octave. The next frequency value is generated by multiplying the current value by a constant greater than 1. Octave is used for situations with wider bandwidths. Decade is a ten-fold sweep, which performs a logarithmic sweep. Test Points is the number of sweep points within a ten-octave. Decade is used for situations with particularly wide bandwidths.

Usually the starting frequency should be greater than zero; the Noise Source parameter needs to be specified in the independent voltage source;

8. Pole-Zero (critical point) analysis: In a single input/output linear system, use the circuit's small signal AC transfer function to calculate the pole or zero point and perform stability analysis using Pole-Zero; linearize the circuit's DC operating point and match small signal models to all nonlinear devices. The transfer function can be either voltage gain (ratio of output to input voltage) or impedance (ratio of output voltage to input current).

Parameter settings

Input Node: Positive input node

Input Reference Node: Reference node of the input terminal (default: 0 (GND))

Output Node: Positive output node

Output Reference Node: The reference node of the output terminal (default: 0 (GND))

Transer Function Type: Set the type of AC small signal transfer function; V (output) / V (input) - voltage gain transfer function, V (output) / I (input) - resistance transfer function

Analysis Type: More precise analysis of the peak points

Pole-Zero analysis can be used for resistors, capacitors, inductors, linear controlled sources, independent sources, diodes, BJT tubes, MOSFET tubes and JFET tubes, but does not support transmission lines. Performing Pole-Zero analysis on complex large-scale circuit designs takes a lot of time and may not find all the Pole and Zero points, so it is more effective to split it into small circuits for Pole-Zero analysis.

9. Transfer function analysis (also called DC small signal analysis): Transfer function analysis calculates the DC input resistance, DC output resistance, and DC gain values ​​at each voltage node.

Parameter settings

Source Name: Specifies the small signal input source for the input reference

Reference Node: Specifies the circuit node to use as reference for calculation of each specific voltage node (default: set to 0)

Transfer function analysis can be used to calculate the values ​​of three small signals: DC input, output resistance and DC gain in the entire circuit.

10. Monte Carlo analysis: Monte Carlo analysis is a statistical simulation method. Given a circuit component parameter tolerance that follows a statistical distribution law, a group of pseudo-random numbers are used to obtain a random sampling sequence of component parameters. These randomly sampled circuits are subjected to DC scan, DC operating point, transfer function, noise, AC small signal, and transient analysis. The statistical distribution law of circuit performance is estimated through multiple analysis results. Monte Carlo analysis can perform worst-case analysis. AD6's Monte Carlo analysis has powerful and complete functions for worst-case analysis.

Parameter settings

Seed: This value is randomly generated during the simulation. If you perform a simulation with a different sequence of random numbers, you need to change this value (default: -1)

Distribution: Tolerance distribution parameters; Uniform (default) indicates monotonic distribution. It remains monotonic after exceeding the specified tolerance range; Gaussian indicates Gaussian curve distribution (i.e. Bell-Shaped), and the nominal median deviates from the specified tolerance by -/+3; Worst Case indicates that the worst case is similar to the monotonic distribution, not just the worst point within the tolerance range.

Number of Runs: The number of runs to perform simulations with different device values ​​within the specified tolerance (default: 5)

Default Resistor Tolerance: Default tolerance of resistor components (default: 10%)

Default Capacitor Tolerance: Default tolerance of capacitor components (default: 10%)

Default Inductor Tolerance: Default tolerance of inductor components (default: 10%)

Default Transistor Tolerance: Default tolerance of transistor devices (default: 10%)

Default DC Source Tolerance: DC source default tolerance (default: 10%)

Default Digital Tp Tolerance: The default tolerance of the propagation delay of digital devices (default: 10%). This tolerance will be used to set the range of values ​​generated by the random number generator. For a device with a nominal value of ValNom, the tolerance range is: ValNom – (Tolerance * ValNom) < RANGE > ValNom + (Toleance * ValNom)

Specific Tolerances: User-specific tolerances (default: 0). To define a new specific tolerance, first execute the Add command, select the device with the specific tolerance in the Designator field of the newly added row, set the parameter value in Parameter, set the tolerance range in Tolerance, and Track No. is the tracking number. Users can set specific tolerances for multiple devices. This area is used to indicate the changes between them when setting specific tolerances for multiple devices. If the Tracking No. of the specific tolerances of two devices is the same and the distribution is the same, the same random number will be generated during simulation and used to calculate the circuit characteristics. Select one of uniform, gaussian, and worst case in Distribution. Each device contains two types of tolerances, namely device tolerance and batch tolerance.

When resistance, capacitance, inductance, transistors, etc. change at the same time. But it is conceivable that due to too many changing parameters, it is not known which parameter has the greatest impact on the circuit. Therefore, it is recommended that readers do not "be greedy" and analyze one by one. For example, if readers want to know the impact of transistor parameter BF on the circuit frequency response, then the impact of other parameters on the circuit should be removed, and only the BF tolerance should be retained.

11. Parameter sweep: Parameter sweep can be used with analysis types such as DC, AC or transient analysis to perform parameter sweeps on the analysis performed on the circuit, which is very convenient for studying the impact of circuit parameter changes on circuit characteristics. Similar to Monte Carlo analysis and temperature analysis in terms of analysis function, it sweeps all analysis parameters of the circuit according to the sweep variable, and the analysis results generate a data list or a set of curves. At the same time, the user can also set a second parameter sweep analysis, but the data collected by the parameter sweep analysis does not include the devices in the sub-circuit.

Parameter settings

Primary Sweep Variable: The circuit parameter or device value you want to sweep. Use the drop-down option box to set it.

Primary Start Value: The initial value of the scan variable

Primary Stop Value: The end value of the scan variable

Primary Step Value: The step size of the scan variable

Primary Sweep Type: Set the absolute or relative value of the step length

Enable Secondary: The second scan variable needs to be determined when the analysis

Secondary Sweep Variable: The circuit parameter or device value you want to sweep, set it using the drop-down option box.

Secondary Start Value: The initial value of the scan variable

Secondary Stop Value: The end value of the scan variable

Secondary Step Value: The step size of the scan variable

Secondary Sweep Type: Set the absolute or relative value of the step length

Parameter sweeps should be performed together with at least one of the standard analysis types. We can observe that different parameter values ​​produce different curves. The size of the deviation between the curves indicates the degree of influence of this parameter on the circuit performance.

12. Temperature scanning: Temperature scanning refers to the calculation of circuit parameters within a certain temperature range to determine performance indicators such as the temperature drift of the circuit.

Parameter settings

Start Temperature: Starting temperature (unit: Celsius C)

Stop Temperature: Stop temperature (unit: Celsius C)

Step Temperature: The temperature increment within the temperature change range.

During temperature scan analysis, a large amount of analysis data will be generated, so it is necessary to set Collect Data for in General Setup to Active Signals.

The basic steps for simulation using Altium Designer are as follows:

1. Load component libraries related to circuit simulation

2. Place simulation components on the circuit (the component must have a simulation model)

3. Draw the simulation circuit diagram. The method is the same as drawing the schematic diagram.

4. Add simulation power supply and excitation source to the simulation circuit diagram

5. Set the initial state of the simulation node and circuit

6. Perform ERC check on the simulation circuit schematic to correct errors

7. Set the parameters for simulation analysis

8. Run circuit simulation to get simulation results

9. Modify simulation parameters or replace components, and repeat steps 5 to 8 until satisfactory results are obtained.

The following is an introduction to the entire process of circuit simulation through a specific example.

1. Run Altium Designer, select FileOpen Project…, and open the ExamplesCircuit SimulationAnalog AmplifierAnalog Amplifier.PRJPCB file in the installation directory, as shown in Figure 1.

Figure 1 Open the schematic file

Double-click Analog Amplifier.schdoc to enter the circuit diagram editing environment, as shown in Figure 2. Right-click Analog Amplifier.schdoc and select Compile Document Analog Amplifier.schdoc in the pop-up menu to check whether there are errors in the file. If there are any errors, correct them first.

Figure 2 Compiled file

2. Load the simulation library:

Click Libraries on the toolbar on the right side of the window and select Libraries in the pop-up window.

3. Briefly introduce how to observe and modify the simulation model. In the circuit diagram editing environment, double-click the component U1, and the device property window shown in Figure 3 will pop up. The simulation model can be seen on the right side of the window. Double-click Simulation under Type to call up the detailed simulation model description of the device, see Figure 4.

Figure 3 Device properties

Figure 4 Simulation model

4. After the simulation model is set, you need to set the simulation nodes. As shown in Figure 5, add network identifiers to the nodes that need to be observed and compile the file. Save it after confirmation, and then save the project file. Then you can perform simulation.

Figure 5 Simulation nodes

5. Select the required analysis method. Click each analysis method and the corresponding simulation parameter settings will appear on the right side of the window.

As shown in Figure 6.

Figure 6 Simulation parameter settings

6. Parameter sweep analysis: The parameter sweep function is very helpful for the early stage of circuit design and can save a lot of manual calculation time. See Figure 7.

Figure 7 Setting scanning parameters.

7. Modify the simulation model parameters. During the design process, if you need to modify the simulation model parameters, click the Projects option in the lower left corner of the window. In the window shown in Figure 8, double-click the UA741.ckt file under Libraries under the Analog Amplifier.PRJPCB project to enter the simulation model file. Modify the corresponding parameter values ​​in this file as needed, then save it and you can proceed to the next simulation.

Figure 8 Modifying simulation model parameters

8. Scan parameters and output simulation results. In the simulation waveform interface shown in Figure 10, select Cursor A and Cursor B in the pop-up menu, and two cursors will be generated on the waveform. Drag the cursor to measure the relevant data. Click the Sim Data option in the lower left corner of the window as shown in the figure, and you can observe the actual measurement results in this interface. You can also select the graph that meets the requirements, and its parameter value will be displayed below the waveform, as shown in Figure 11.

Figure 10 Scan result output

Figure 11 Select simulation parameters