Simulation Troubleshooting

Old Content - visit altium.com/documentation

When a circuit will not simulate you must identify if the problem is in the circuit, or the process of simulation. Follow the information contained in this section of the reference and work through the suggested points, trying one at a time.

Sometimes during a simulation a message will be displayed reporting errors or warnings. These messages are listed in the Messages panel.

Warning Messages

Warning messages are not fatal to the simulation. They generally provide information about changes that SPICE had to make to the circuit in order to complete the simulation. These include invalid or missing parameters, and so on. Digital SimCode warnings may include information such as timing violations (tsetup, thold, trec, tw, etc.) or significant drops in power supply voltage on digital components. Valid simulation results are normally generated even if warnings are reported.

Error Messages

Error messages provide information about problems that SPICE could not resolve and were fatal to the simulation. Error messages indicate that simulation results could not be generated, so they must be corrected before you will be able to analyze the circuit.

Troubleshooting netlist generation failure

When you run a simulation, the first thing that happens is the circuit is analyzed and a SPICE netlist is generated. This netlist is then passed to the SPICE engine, which simulates the circuit and generates the results.
Any errors that are detected during netlisting are listed in the Messages panel. Likely causes of netlisting errors include:

  • A component in the schematic source document(s) not containing simulation information. To check if a component is suitable for simulation, double-click on the component in the schematic to open its Component Properties dialog and confirm that there is a linked simulation model, in the Models region of the dialog.
  • The simulation model file that a component references is not in the location specified iin the Model Location region on the Model Kind tab of the Sim Model dialog. This could happen if the associated integrated library in which the model is stored is not installed, or it has been moved from its original install location.

All source component libraries are installed to the following location:

\Library

This root folder includes various sub-folders containing component integrated libraries from specific manufacturers, as well as two general integrated library files (Miscellaneous Devices.IntLib and Miscellaneous Connectors.IntLib) providing general schematic components (many of which are simulation-ready).

The \Library\Sim folder contains various .txt and .scb files, for SimCode-based simulation models, such as CMOS and 74XX series digital component models.

The \Library\Simulation folder contains the following specific simulation-ready component integrated libraries:

Simulation Math Function.IntLib
Simulation Sources.IntLib
Simulation Special Function.IntLib
Simulation Transmission Line.IntLib

  • The path to the Digital SimCode model (uncompiled source file (*.txt) or compiled file (*.scb)), referred to as {MODEL_PATH}, does not match the location of the model. This could happen if the model is moved to a different location on the hard drive. The model path is defined in the Simulation Preferences dialog and is relative to the Library folder of the installation. By default, the path is \Library\Sim\.

Trouble-shooting simulation analysis failures

One of the challenges of all Simulators is convergence. What exactly is meant by the term, "convergence"? Like most Simulators, the Altium Designer-based Simulator's SPICE engine uses an iterative process of repeatedly solving the equations that represent your circuit, to find the quiescent circuit voltages and currents. If it fails to find these voltages and current (fails to converge) then it will not be able to perform an analysis of the circuit.

SPICE uses simultaneous linear equations, expressed in matrix form, to determine the operating point (DC voltages and currents) of a circuit at each step of the simulation. The circuit is reduced to an array of conductances which are placed in the matrix to form the equations (G * V = I). When a circuit includes nonlinear elements, SPICE uses multiple iterations of the linear equations to account for the non-linearities. SPICE makes an initial guess at the node voltages then calculates the branch currents based on the conductances in the circuit. SPICE then uses the branch currents to recalculate the node voltages, and the cycle is repeated. This cycle continues until all of the node voltages and branch currents fall within specified tolerances (converge).

However, if the voltages or currents do not converge within a specified number of iterations, SPICE produces error messages (such as singular matrix, Gmin stepping failed, source stepping failed or iteration limit reached) and aborts the simulation. SPICE uses the results of each simulation step as the initial guesses for the next step. If you are performing a Transient analysis (that is, time is being stepped) and SPICE cannot converge on a solution using the specified timestep, the timestep is automatically reduced, and the cycle is repeated. If the timestep is reduced too far, SPICE displays a Timestep too small message and aborts the simulation.

General simulation convergence troubleshooting

When a simulation analysis fails, the most common problem is failure of the circuit to converge to a sensible operating point. Use the following techniques to solve convergence problems.

Convergence troubleshooting steps

  • When you have a convergence problem, first turn off all the analyses except the Operating Point analysis.
  • Consult the Messages panel for any errors/warnings relating to simulation.
  • Make sure the circuit is wired correctly. Dangling nodes and stray parts are not allowed.
  • Ensure that the circuit has a ground node, and that every node in the circuit has a DC path to this ground. Components that can isolate a node include transformers and capacitors. Voltage sources are considered a DC short circuit, current sources are considered a DC open circuit.
  • Ensure that zeros have not been confused with the letter O when entering simulation parameters.
  • Ensure that proper SPICE multipliers have been specified (MEG instead of M for 1E+6) for any component values or simulation parameters. Multipliers are not case sensitive. Also, spaces between values and multipliers are not allowed. For example it should be 1.0uF, not 1.0 uF.
  • Make sure all devices and sources are set to their proper values.
  • Make sure the gain of any dependent source is correctly set.
  • Temporarily eliminate series capacitors or current sources and re-run the simulation.
  • Temporarily eliminate parallel inductors or voltage sources and re-run the simulation.
  • On the SPICE Options page of the Analyses Setup dialog (from the schematic select Design » Simulate » Mixed Sim, then click the Advanced Options entry in the Analyses/Options list), increase the value of the ITL1 parameter to 300. This will allow the Operating Point analysis to go through more iterations before giving up.
  • Add .NS (Nodeset) devices to define the node voltages. If the initial guess of a node voltage is way off, the .NS device can be used to predefine a starting voltage that is used for a preliminary pass of the operating point analysis.
  • If the Nodeset device does not assist in convergence, try defining the initial conditions by placing .IC devices. In this case the node voltages are held at the specified values during the Operating Point analysis, then released during the Transient analysis.
  • Enable the Use Initial Conditions option on the Transient/Fourier Analysis Setup page of the Analyses Setup dialog (from the schematic, select Design » Simulate » Mixed Sim, then click the Transient/Fourier Analysis entry in the Analyses/Options list). This option works in conjunction with the .IC devices (or the IC parameter of the components). By setting this option, the Operating Point analysis is not performed and the specified voltages are used as the initial conditions for the Transient analysis.
  • Specify the series resistance parameters of your models and increase the GMIN option (SPICE Options page of the Analyses Setup dialog) by a factor of 10. Specify the initial condition of semiconductor devices, especially diodes, as OFF.

DC Sweep Analysis troubleshooting

When you have a problem with a DC Sweep analysis, first try the steps listed above in the Convergence troubleshooting steps.
If you still encounter problems, try the following:

  • Change the value of the Primary Step parameter on the DC Sweep Analysis page of the Analyses Setup dialog. If discontinuities exist in a device model (perhaps between the linear and saturation regions of the model), increasing the step size may allow the simulation to step over the discontinuity. Making the steps smaller, on the other hand, will allow the simulation to resolve rapid voltage-transition discontinuities.
  • Disable the DC Sweep analysis. Some problems (such as hysteresis) cannot be resolved by DC analysis. In such cases, it is more effective to use the Transient analysis and ramp the values of the appropriate power sources.

Transient Analysis troubleshooting

When you have a problem with a Transient analysis, first try the steps listed above in the Convergence troubleshooting steps. 

If you still encounter problems, try the following.

On the SPICE Options page of the Analyses Setup dialog (from the schematic select Design » Simulate » Mixed Sim, then click the Advanced Options entry in the Analyses/Options list):

  • Set the RELTOL parameter to 0.01. By increasing the tolerance from its default of 0.001 (0.1% accuracy), fewer iterations will be required to converge on a solution and the simulation will complete much more quickly.
  • Increase the value of the ITL4 parameter to 100. This will allow the Transient analysis to go through more iterations for each timestep before giving up. Raising this value may help to eliminate timestep too small errors improving both convergence and simulation speed.
  • Reduce the accuracy by increasing the values of ABSTOL and VNTOL, if current/voltage levels allow. Your particular circuit may not require resolutions down to 1uV or 1pA. You should, however, allow at least an order of magnitude below the lowest expected voltage or current levels of your circuit.
  • Change the Integration Method to one of the Gear methods. Gear integration requires a longer simulation time, but is generally more stable than trapezoidal. Gear integration may be particularly useful with circuits that oscillate or have feedback paths.

Additional things to try:

  • Realistically model your circuit. Add realistic parasitics, especially stray/junction capacitance. Use RC snubbers around diodes. Replace device models with subcircuits, especially for RF and power devices.
  • Increase the rise/fall times of any Periodic Pulse sources in your circuit. Even the best pulse generators cannot switch instantaneously.

 

You are reporting an issue with the following selected text and/or image within the active document:
Request Free Trial

Complete this form to request a free 15 day trial of Altium Designer: