Lab: predict and simulate a loaded divider

Prediction before execution

Build the 5 V, 10 kΩ/10 kΩ divider with an additional 10 kΩ load from out to ground. The lower two resistors are parallel, giving 5 kΩ. Total source resistance is 15 kΩ, source current is 0.333333 mA, output is 1.666667 V, and each lower branch carries 0.166667 mA. Keep these four predictions in a small result table.

Reproducible input

Save the following as loaded-divider.cir and run it with an available standalone ngspice executable: ngspice -b loaded-divider.cir. These are standard SPICE elements with no external device model. The course supplies the input; the command's availability depends on your environment.

Loaded divider: nominal resistors
V1 supply 0 DC 5
Rtop supply out 10k
Rbottom out 0 10k
Rload out 0 10k
.op
.end

Node 0 is the reference. The first line is a title, and the final .end closes the deck. In this source orientation, i(V1) is negative when the source delivers current; approximately −0.333333 mA is expected. The current through Rload is positive from out to ground. A sign mismatch is not automatically a magnitude mismatch.

Change one condition

Remove Rload and rerun: out should become 2.5 V and source current magnitude 0.25 mA. Restore Rload, change only its value to 100k, and predict 2.380952 V. Use a 1 mV voltage comparison tolerance for the nominal ideal-resistor exercise; this tolerance measures calculation versus simulation, not physical component accuracy.

Record simulator version, exact deck, results, and whether each expected value passed. Check errors and exit status before accepting a printed number. The source network has no disconnected nodes or nonlinear convergence problem, so an unexpected result usually calls for inspecting node names, units, or copied values.

If you also draw the circuit in a schematic editor, compare its exported connections to this deck rather than assuming that a similar-looking picture is electrically identical. No ALcad execution or backend compatibility is established by the standalone command. Syntax and analysis behavior are described in the ngspice documentation.