--- In LTspice@yahoogroups.com, "Hendrik Jan Zwerver" wrote: > > --- In LTspice@yahoogroups.com, "ofarrell_simon" wrote: > > > > Hi guys > > > > I am an amature at this but would like to know some details > > on the SPICE settings in LTSpice. > > > > What do Gmin, Abstol, Reltol, CHgtol, Trtol, Volttol and Sstol > > mean. > > > > I am guessing that the "tol" means tolerance. > > > > The other thing is what effect do they have on the simulation. > > Some effects might be far more pronounced that others. > > > > Anyway if some light could be shed on this that would be great. > > I have been tinkering with this for a couple of years now and > > still dont know > > this. > > > > Kind Regards > > > > Simon > > > > Hello Simon, > > You can find your answers in the help file : > LTspice -> Dot commands -> .option > > My experience was that playing around with these settings is asking > for trouble. I recommand to not touch these if you don't know what > you are doing. You can make TRtol, ABStol and VNtol a little bit > higher to speed up simulation but not more than a factor 5. Chance > that the simulator makes garbage is very high. > > I have seen documents from mosfet manufactures to change these > settings in order to make there models work. They claim that the > default settings are often wrong. Infact the models they make are > terrible written and the default settings are ok. > > Here my opinion about the parameters: > Gmin; Don't change this unless you have a realy difficult to solve > circuit. Makes no difference in speed if changed. > > Abstol; Can help speed if you increase this value. > Reltol; same for this one. maximum 0.01. Can cause convergence > problems if too high. > CHgtol; Do not change this. > Trtol; a value between 1-7 can be used. Too high causes problems. > Volttol; I think you mean Vntol; Same as for the abstol. > Sstol; This has nothing to do with normal simulation. > > General if you increase the values the simulator is less accurate > but faster. The chance that the simulator produce simulation > errors and convergence problems also increases. If that happens > the simulator will be slower. > > Greatings, > > Hendrik Jan > Hello Simon, I will upload this message also to the Files section. Peoples are invited to correct any mistakes. Files > FAQ > Simulator_Options.txt A Short Description Of The Most Often Used SPICE Options -------------------------------------------------------- Alternate solver This is the first you can try if your simulation doesn't run at all or if it simulates very very slow. Control Panel -> SPICE Solver:Alternate The DC operating point (.OP) is calculated for any nonlinear circuit at the beginning of a simulation. Inductors are treated as shorts, capacitors are removed. If an initial current is set for an inductor, it will be replaced by a current source. .NODESET Initial guess for the voltages of specified nodes. .NODESET V(xyz)=5 V(3)=0 .IC Set the initial voltages at nodes or the initial currents through inductors. .IC V(7)=3 IL7=1 Example circuit: The first comment line is mandatory for a SPICE netlist. * .IC Test C1 1 0 1 L1 1 0 1 .tran 10 .IC V(1)=5) I(L1)=1 .end ITL1 The number of iterations to find the operating point. .OPTIONS ITL1=500 ITL2 DC transfer curve iteration count limit .ITL2=500 I had sometimes success with .OPTIONS ITL1=500 ITL2=500 GMIN Conductance GMIN is parallel to every PN-junction. This shunt conductance can be increased to reach convergence. .OPTIONS GMIN=1e-9 Transient Analysis ------------------ I am not sure whether ITL4 and ITL6 are really use the same way as in the standard SPICE. ITL4 Number of iterations for gmin-stepping. This gmin-stepping adds a conductance from every node to GND (net 0). It has nothing to do with the GMIN parallel PN-junctions as described above. .OPTIONS ITL4=100 ITL6 Source stepping steps the supply voltages from zero to it's final value to achieve the operating point. I think it's used in all types of simulations. The number of iterations can be increased. .OPTIONS ITL6=100 RELTOL Increase the relative allowed error tolerance. .OPTIONS RELTOL=0.003 I often try with the value 0.003 if I have a convergence problem. The upper useful limit is a value of 0.01 from my experience. TRTOL Step size for transient analysis .OPTIONS TRTOL=7 ; standard value for SPICE, TRTOL=1 in LTSPICE This means LTspice calculates with more precision in the time domain than standard SPICE when using the default setting. ABSTOL, VNTOL ABSTOL and VNTOL(Volttol) are the absolute error limits for voltages and currents. ABSTOL and VNTOL should be many orders of Magnitude below the voltages and currents in the circuit. Current tolerance .OPTIONS ABSTOL=1e-12 Voltage tolerance .OPTIONS VNTOL=1e-6 SSTOL SSTOL is the error tolerance for the for steady state detection of the SMPS-ICs from LTC. .OPTIONS SSTOL=0.003 It's related to the option in the transient-setting "Stop simulating is steady state is detected". .tran 0 .5m 0 10n steady This option is required for the efficiency calculation of switch mode power supplies (SMPS). The next two settings are really a last resort. They can make your circuit totally useless. GSHUNT Add a shunt resistor from every node to GND. Rshunt=1/GSHUNT .OPTIONS GSHUNT=1e-9 CSHUNT Add a shunt capacitor from every node to GND. This can help as a last resort with transient simulations, but you have to check how much it changes the behaviour of your circuit. .OPTIONS CSHUNT=1e-13