I see how to set the total run time for a transient simulation, but what if I didn't want the simulation to start at 0s?
For example, if I have two voltages sources that are stepping at offset times from each other, and one of them doesn't start until time = 1s. How can I shift the simulation to start at 1s instead?
As the others have said, any SPICE solver needs to actually solve the circuit up until the time of your interest, but you can also use the simulation card to only save from a certain time:
.tran 0 {total_simulation_time} {time_to_start_saving_data} {optional_timestep}
For example, if you need 5s of simulation, but you need to discard the forst 3s, then the card would look like this: .tran 0 5 3.
That's quite different. :-) If you are using the builtin PULSE source, then it's as easy as setting the td parameter, for example a unity 1kHz pulse with 0.3 width, 1% rise/fall times, and 666us delay would look like this:
PULSE 0 1 666u 10u 10u 0.299u 1m
If you're using behavioural sources, then you'd want to use the delay(x,y) function. And if you're having some other custom circuitry, depending on the type of signal (digital or analog), you could either use the same behavioural source with delay(), a tline or ltline (these work with both analog and digital), or a dedicated A-device with td=<...>. The manual has more details about them. Or see ltwiki.
I use LTspice all the time and I usually just edit the time axis when I want a specific range, for example. I get your pain, though. I also want the ability to set up a special spice deck card on the schematic itself that will set up the x-axis and y-axis for me, with ranges specified, along with the curves I want traced out. It would be cool to have it. I'm just not aware how to achieve it.
While, I'm not aware of an automatic method where you place a special spice deck card on the schematic that will load up the right plot parameters for you, I can tell you that if you do change the x-axis and y-axis parameters and ranges to get what you want to see, you can save all that in a ".plt" file. Just click on the plot pane that LTspice has generated for you and then a menu option called "Plot Settings" will appear. Near the bottom of the drop-down list will appear something called "Save Plot Settings". If you click on that, you can save the plot settings you have worked out and it will create a file for you with all the needed information.
This plot file can be re-loaded at any time by clicking on the plot pane again (to select it) and then use the "Plot Settings" menu option. Go down the list to near the bottom again and pick "Open Plot Settings File" and select your saved file name. This will immediately adjust your plot pane per the information stored in that file. So you can recover it, manually, this way.
That's the best I can offer, for now. I don't know of a better way to handle it.
You can only change the axis of your diagram, it is not possible to "delay" simulation start. The simulation always has to start at time 0. If you could set the start to a later point the software could not know what voltage levels you have in your circuit.
The way these simulation work is by differentially determining the voltage levels at your differnt points in the circuit, step by step. This automatically means, that the software always has to start from the beginning and has to calculate every single time step, otherwise it would loose track of whats going on. So, as I wrote in the beginning, you can not change the start point of the simulation. You can only change the axis of your plot, so you can only see a specific part of your simulation. It will not change the calculation time.
