Aborting transient analysis after desired value is found

I feel more clarification is needed.  Here is the output for a 1 second long simulation that I aborted after it reached 30 microseconds (which took more than 10 minutes to run the simulation):

    tran: time = 17.72 ps   (1.77 n%), step = 298.4 as    (29.8 f%)
    tran: time = 109 ps     (10.9 n%), step = 106.6 fs    (10.7 p%)
    tran: time = 1.145 ns    (114 n%), step = 891.6 fs    (89.2 p%)
    tran: time = 10.4 ns    (1.04 u%), step = 5.085 ps     (509 p%)
    tran: time = 2.667 us    (267 u%), step = 11.28 ns    (1.13 u%)
    tran: time = 3.373 us    (337 u%), step = 26.15 ps    (2.62 n%)
    tran: time = 4.683 us    (468 u%), step = 21.92 ps    (2.19 n%)
    tran: time = 6.609 us    (661 u%), step = 183.6 ps    (18.4 n%)
    tran: time = 8.076 us    (808 u%), step = 546.5 ps    (54.7 n%)
    tran: time = 10.56 us   (1.06 m%), step = 3.132 ns     (313 n%)
    tran: time = 11.91 us   (1.19 m%), step = 1.13 ns      (113 n%)
    tran: time = 14.02 us    (1.4 m%), step = 89.52 ps    (8.95 n%)
    tran: time = 17.12 us   (1.71 m%), step = 339.6 ps      (34 n%)
    tran: time = 18 us       (1.8 m%), step = 8.234 ps     (823 p%)
    tran: time = 20.87 us   (2.09 m%), step = 9.58 ns      (958 n%)
    tran: time = 22.94 us   (2.29 m%), step = 743.4 ps    (74.3 n%)
    tran: time = 24.04 us    (2.4 m%), step = 89.32 ps    (8.93 n%)
    tran: time = 24.83 us   (2.48 m%), step = 49 ps        (4.9 n%)
    tran: time = 26.18 us   (2.62 m%), step = 401.1 ps    (40.1 n%)
    tran: time = 27.26 us   (2.73 m%), step = 5.733 ns     (573 n%)
    tran: time = 28.01 us    (2.8 m%), step = 2.069 ns     (207 n%)
    tran: time = 29.13 us   (2.91 m%), step = 117.2 ps    (11.7 n%)

The maximum charge was reached at 71 nanoseconds.  I would like the simulation to automatically stop around this time.  The rest of the simulation is updating the waveform when the charge changes from one below the maximum charge back to the maximum charge.  Is there some way to set the minmum step to 10 nanoseconds?  Are there other methods that I could use to abort the simulation?

Or perhaps is there a way to run a transient simulation manually one step at a time?  For example, step 1 nanosecond, check value, step 5 nanoseconds, check value, etc. 

Thank you for your help. 

Several ways you could do this. One is to use SpectreMDL to run the analyses and make the measurements, and then use the "autostop" facility to stop the simulation. Look in the simulator documentation for the Measurement Description Language info.

The other approach (which will probably work better if you are using OCEAN or ADE for simulation) is to have a VerilogA block in your schematic which checks for the condition having been met, and then calls $finish_current_analysis when met. See Solution 11488490 .

An example:

 `include "disciplines.vams"
module stopearly (a);

input a;
electrical a;

analog

   @(cross(V(a)-0.9)) $finish_current_analysis;

endmodule

Regards,

Andrew

 Thank you for your quick reply Andrew.  I saw the autostop function, but I do not have much information on how to use it. All it says is 

"If yes, the analysis is terminated when all event-type
meaurement expressions have been evaluated. Event-type
expressions use thresholding, event or delay type functions.
Possible values are no or yes."

 How do I use this function?  As for putting the code in Verilog directly, the only problem is that I do not know what the maximum charge value is.  The only way to tell is to let the experiment run a little longer and see if the charge decreases or never reaches a higher value.  This maximum charge and time changes for each set of parameters. 

 Is there a way to manually run a transient analysis?  I think this would be easiest and quickest for a large number of experiments because I could just test points around the typical values to get the charging time.  It does not have to be exact, just in the range.

 Thanks again.

For MDL-based autostop, there are examples in the installation. Look in <MMSIMinstDir>/tools/spectre/examples/MDL_workshop and you'll find a PDF and gzipped tar file showing you the data. Within the workshop, at least dflip/autostop.mdl is one (you may have others depending on the version you're using - do a grep for autostop). As with the VerilogA based solution, you need to have some criteria by which to decide to stop.

With VerilogA, there's no reason why you couldn't detect when (say) the derivative of the charge crosses 0 (i.e. the slope flattens and then goes negative). Or you could check it's been negative for a while. Really depends on how you want to decide whether to stop.

I don't know what you mean by "manually run a transient analysis". You can run spectre from the command line, if that's what you mean?

Andrew.

The slope is always zero.  I was not clear earlier.  When I say charge, I mean number of electrons.  So the final graph looks like a staircase with each step being an additional electron.  So, I can't check when the slope goes negative or if the slope stays 0 for a certain amount of time.  Imagine the maximum charge being reached at 70 ns, drops to max - 1 at 82 ns, back to max at 100ns, then drops down to max - 1 at 110 ns.  If I wait for 15 ns I would get the max - 1 value and the incorrect time.  Similar situations can be imagined for any "wait" time. 

  By manually run the transient analysis, I mean check the waveform result at an input time without having to simulate the entire wave.  For the result I posted above:

    tran: time = 17.72 ps   (1.77 n%), step = 298.4 as    (29.8 f%)
    tran: time = 109 ps     (10.9 n%), step = 106.6 fs    (10.7 p%)
    tran: time = 1.145 ns    (114 n%), step = 891.6 fs    (89.2 p%)

Lets say I wanted to check the values at 1 ns, then the value at 5 ns, so a 5 ns step, so only have two data points for the waveform.  As opposed to the 106.6 fs and 891.6 fs steps.  Or just ask the simulator to simulate a specific time, such as 1.145 ns without having to do the previous steps.

Or another way to put it, run a transient analysis for 1 ns with 10 ps steps, have the simulation stop so I could check the value, then continue again for another 10 ns with 1 ns steps, stop and check value, with both simulations adding to the same waveform.

I got it to work using $finish_current_analysis and a couple if statements in Verilog.  Thank you for your help.