Connect with us

How to deal with (LT)SPICE error messages

How to deal with (LT)SPICE error messages

  1. Harald Kapp
    This circuit does not have a conduction path to ground. Please flag a node as ground.

    What happened?
    Every SPICE circuit needs a dedicated ground. This is the internal reference (0V) for the SPICE algorithms.

    What can I do?
    Add the tiny triangle from the menu bar to your schematic and connect it to your ground.

    figure 1.png
    Figure 1 Don’t forget the GND symbol

    Make sure there is only one GND symbol. Otherwise all nodes having this symbol will be electrically connected to GND (unless you so desire).

    Singular matrix: check node xxx Iteration yyy ...

    What happened?
    Unlike in a real circuit, every node in a SPICE circuit needs a path to ground, at least somehow. This is due to the matrix algorithms employed.

    What can I do?
    Add a path from node xxx to GND, even if the circuit doesn't require it (or even if it would be forbidden in a real circuit e.g. for isolation). In most cases a very large resistor (10MOhm..100MOhm will suffice to satisfy SPICE's need without influencing the desired simulation result. In the example below, R3 (100MOhm) was inserted to give the network to the right of the photocoupler a path to GND (which it obviously due to the nature of the photocoupler normally doesn't have).

    figure 2.png
    Figure -2 Bypassing an insulation barrier

    In case you are not sure where the source of the problem is, you may also be tempted to add additional capacitances (.OPTIONS cshuntintern) or resistors (.OPTIONS gshunt) from every node to GND.

    Time step too small

    What happened?
    This error message can be caused by a variety of problems. There is no general cure.

    What can I do?
    Note that when you've come to this point you are pretty desperate. Before taking a last resort with the measures below, have a look at your circuit. Can you simplify it? Can you do (at least for starters) with a plain vanilla circuit without all the bells and whistles of your design? Are there circuit elements which are not required for the issue you are going to simulate? E.g. can you remove overvoltage protection circuitry while you are simulating normal operation? This will, by the way, speed up your simulation.

    Some other things you may try:
    Add dummy resistors to critical nodes as described in the above scenario. The resistors don't have to be connected to GND. Sometimes bridging a critical component (e.g. a capacitor) may help. Use trial and error to find the right places.
    Increase the tolerances for simulation. Wider tolerances may allow the circuit to converge at the cost of reduced accuracy. In LTSPICE, tolerances may be manually set using the control panel's "SPICE" tab. Good candidates for manipulation are:
    • Gmin
    • Abstol
    • Reltol
    • Chgtol
    You may even try and select an alternative solver engine from the left of the same tab.
    Please remember to reset these values to their defaults after simulation so as not to disturb future simulations.

    More reading: http://www.aboutspice.com/details-208

    SPICE help topics to look at: .OPTIONS, cshuntintern, gshunt

    Harald Kapp, 2014-05-13
Electronics Point Logo
Continue to site
Quote of the day

-