I drew it up as a straight power-on delay. The rail at the top is Acc (14V accessory power) from the ignition switch.
The switch symbol is actually redefined as a behavioural resistor
* (Ctrl-RightClick on a component to get to the dialog that lets you override what SPICE sees it as and modify hidden parmeters if permitted for that component type). I changed the prefix to
R and the value to
R=sw(I(L1)>30mA) and that (with the .func sw on the schematic) makes the switch act as relay contacts, ON if the current through L1 is over 30 mA.
However if you don't have the swSPST.asy symbol, LTspice looses all that when it opens the schematic, and one of the *MAJOR* problems with LTspice is keeping track of what symbols and models are standard and what are custom or 3rd party. Probably the easiest fix would be to paste this:
Version 4
SymbolType CELL
LINE Normal -15 0 -33 0
LINE Normal 1 -15 -15 0
LINE Normal 15 0 0 0
LINE Normal 31 0 15 0
CIRCLE Normal 3 -13 -1 -17
CIRCLE Normal 2 2 -2 -2
PIN -32 0 NONE 8
PINATTR PinName 1
PINATTR SpiceOrder 1
PIN 32 0 NONE 8
PINATTR PinName 2
PINATTR SpiceOrder 2
into a text editor and save it as swSPST.asy in the same folder as you downloaded the .asc file to then reopen the unmodified .asc file.
Alternatively simply delete the switch and load as its sufficient to plot the current through the relay coil.
When you run the sim the plot window comes up empty unless you have a saved .plt file. With the plot window open, and no specific schematic drawing tools active, click a node (connection) to plot a voltage and click a component to plot the current through it. For components with more than two leads, you must click the lead to plot individual lead currents (where you see a 'clamp ammeter' cursor if you hover). Finally, to plot a voltage difference drag from the node you want to plot to the node you want as reference.
I would suggest plotting the nodes vc and drv (or instead of drv, plot I(L1) ). The sim runs five times with increasing {rt} so you will see five curves for the capacitor and five increasing delays for drv or I(L1), all on the same plot. If you find that confusing comment out the .step param rt command.
To use it for real, connect it in parallel to the existing horn so it gets power when you press the horn button. As the horn is a nasty inductive load, it will need a beefy diode in parallel, cathode positive to prevent the back-EMF spike killing the delay circuit when you let go of the horn button. You'll probably want to power the new horn off a spare fuse in the fusebox, off the switched accessory supply, via the delay circuit's relay contacts, so you don't overload the horn button.
* see: http://ltwiki.org/?title=Undocumented_LTspice