When I simulate with the netlist, I got a wrong message. when I change FCTRL 6 2 VISRC 1E+0 EVCVS 8 9 5 2 1E+0 into FCTRL 6 2 VISRC 1E-1 EVCVS 8 9 5 2 1E-1 The program can be go on. whats matter? whats different between the numbers? thanks
I know its model of transformer. what I want to know is What meaning of the VISRC and FCTRL and EVCVS are? I search web site and cannt get the answer. thanks at the same. I know the rest terms meanings. they are all standard modeling terms
N+ and N- are the positive and negative nodes, respectively. Note that voltage sources need not be grounded. Positive current is assumed to flow from the positive node, through the source, to the negative node. A current source of positive value forces current to flow out of the N+ node, through the source, and into the N- node. Voltage sources, in addition to being used for circuit excitation, are the 'ammeters' for SPICE, that is, zero valued voltage sources may be inserted into the circuit for the purpose of measuring current. They of course have no effect on circuit operation since they represent short-circuits.
Linear Current-Controlled Current Sources General form: FXXXXXXX N+ N- VNAM VALUE
Examples: F1 13 5 VSENS 5 N+ and N- are the positive and negative nodes, respectively. Current flow is from the positive node, through the source, to the negative node. VNAM is the name of a voltage source through which the controlling current flows. The direction of positive controlling current flow is from the positive node, through the source, to the negative node of VNAM. VALUE is the current gain.
Linear Voltage-Controlled Voltage Sources General form: EXXXXXXX N+ N- NC+ NC- VALUE
Examples: E1 2 3 14 1 2.0 N+ is the positive node, and N- is the negative node. NC+ and NC- are the positive and negative controlling nodes, respectively. VALUE is the voltage gain.
It's whatever you want it to be. As far as a simulator is concerned, the names might as well be random so long as they're unique. If you use a schematic capture package, often the names will just be V1, V2, V3, etc. For "hand-crafted" models, often people will try to use meaningful names so that other (huamans) reading the text have some idea what the function of the part is. E.g., "Lleak" clearly suggests an inductor modeling leakage inductance.
Note that the early simulators in the '70s and some in the '80s only allowed numbers (V1, V2, V3), but as far as I'm aware all contemporary simulators allow named devices (Vsource, Vbattery, etc.)
A "time step to small" error is simply that the spice engine was unable to find a solution. It does not mean that there is a specific error in the circuit. However, unrealistic circuits can produce this failure to converge problem.
Spice is a general purpose non-linear differential equation solver. It does this numerically. There is no guarantee that all circuits can be solved by this technique.
[Independant Source] Vxxx = Dependant Voltage source format V +node -node DC value of 0 volts
[Dependant Sources] Exxx =Voltage Controlled Voltage source format E Gain so device EVCVS has output nodes at 8,9 which is equal to the voltage across node 5,2 multiplied by gain of 1
Fxxx = Current Controlled Current source format F Gain so device FCTRL has output nodes 6,2 which has a values in current equal to current flowing through Ctrl voltage source VISRC times a gain of 1 ** notice that this independent voltage source has no dc voltage value. This acts like an Ammeter
(+) and (-) Output nodes. A positive current flows from the (+) node through the source to the (-) node. The current through the controlling voltage source determines the output current. The controlling source must be an independent voltage source (V device), although it need not have a zero DC value.