[help]How to see the transient operating points at different timing

[werank]

Hi friends:
I run a transient simulation and want to see the change of operating points through timing.
The Results--Print--transient operating points can show me the beginning statement of OP.
But can not show me all the simulation time operating (ex. transistor region,Cgs )
Thanks

 

[jeffrey samuel]

what are you using where did you use this command

the schematic or something that can educate us

 

[erikl]

I run a transient simulation and want to see the change of operating points through timing.

You can probe node voltages and device currents and represent them on the waveform tool vs. time.

But can not show me all the simulation time operating (ex. transistor region,Cgs )

These aren't operating points (OPs) but calculated parameters which can't be represented directly vs. time.

With the help of the calculator you can represent the function Veff=Vds-Vgs which gives you an approximate perception of the region -- at least a differentiation between triode & saturation region.

You could also save the OPs at discrete time points and calculate those dependent parameters afterwards.

 

[werank]

You could also save the OPs at discrete time points and calculate those dependent parameters afterwards.

How to setup the ADE to save the OPs, is it can save the operate region ?
THX

 

[erikl]

How to setup the ADE to save the OPs, is it can save the operate region ?

You'd have to put the save commands either into the netlist file, or into an included model file.
Another possibility is to use the OCEAN script tool. Check the ADE and SPECTRE documents!

 

[werank]

Hi erikld:
I wonder if you can show me how to save the OP data through the time.

 

[erikl]

I wonder if you can show me how to save the OP data through the time.

You can't save the OP data through the time, just node voltages and device currents, as I already tried to tell you above.

You can save OP data only at discrete time points: at the beginning or at the end of a simulation, and may be at discrete time points in between (but for the latter I can't tell you exactly, how. Probably you need to run a simulation for every end point -- perhaps there's a chance of continuation).

To do this, use the save command. RTFM!

save=[I]selected[/I]        Signals to output. Possible values are [I]all, lvl, allpub, lvlpub, selected[/I], or [I]none[/I].

 

[dick_freebird]

You might consider using stop / continue to let you pick off
transient operating point numbers, but you could also just
use the calculator to get at anything that is voltage, current,
or maths on these.

I really doubt that capacitances in-the-moment are all that
exciting or dependent on the full circuit sim over a long time.
You could just do a quick simple sim to map Cxx to Vxx on
a single device, and then take the larger-circuit voltages
as simply the index-set. Of course this is more work for you
and less of a simple simulator "gimme".

 

[FvM]

Apart form the question if the values of individual transistor capacitances versus time are holding much information, all transistor parameters are functions of circuit voltages and currents and be calculated applying the device equations.

 

[sutapanaki]

You can go to tran analysis menu, then click on Options and go to Outputs tab. Scroll down to find infotimes on ANALYSIS DURING TRAN. In that field list the discrete times at which you want to see the op. After the simulation is done, you can backannotate the schematic with those op. For that you can in analog artist go to Results > Annotate and choose Transient Operating Points - there will be a drop-down menu where you choose the time point. Also there is Transient Node Voltages - for that one you don't have the drop-down menu, you'll have to enter the time manually.