INT - Integrator (Single-Ended IO)
Model Kind
General
Model Sub-Kind
Generic Editor
SPICE Prefix
A
Model Name
INT
SPICE Netlist Template Format
@DESIGNATOR %1 %2 @"DESIGNATOR"INT
.MODEL @"DESIGNATOR"INT int (?in_offset|in_offset=@in_offset| ?gain|gain=@gain| out_lower_limit=@out_lower_limit out_upper_limit=@out_upper_limit ?limit_range|limit_range=@limit_range| ?out_ic|out_ic=@out_ic|)
Parameters (definable at component level)
The following component-level parameters are definable for this model type and are listed on the Parameters tab of the Sim Model dialog. To access this dialog, simply double-click on the entry for the simulation model link in the Models region of the Component Properties dialog.
| In_Offset | input offset (Default = 0). |
| Gain | gain (Default = 1). |
| Out_Lower_Limit | output lower limit. |
| Out_Upper_Limit | output upper limit. |
| Limit_Range | upper and lower limit smoothing range (Default = 1.0e-6). |
| Out_IC | output initial condition (Default = 0). |
Notes
This model is a simple integration stage that approximates the integral of the input with respect to time.
The output upper and lower limits are used to prevent convergence errors due to excessively high output values. These limits provide for integrator behavior similar to that found in the integration stage of an operational amplifier. Once a limit has been reached, no further storage of values occurs.
The Limit_Range specifies the value below Out_Upper_Limit and above Out_Lower_Limit at which smoothing of the output begins.
Truncation error checking is an inherent part of the model. If truncation errors become excessive, the model uses smaller time increments between simulation data points, therefore providing for a more accurate simulation of the integration function.
The input signal can be either a single-ended current or single-ended voltage signal.
Examples
Consider the integrator in the above image, with the following characteristics:
- Pin1 (in) is connected to net
IN - Pin2 (out) is connected to net
OUT - Designator is
U1 - Out_Lower_Limit =
0 - Out_Upper_Limit =
40e-6 - All other parameters are left at their default values.
The entry in the SPICE netlist would be:
*Schematic Netlist:
AU1 IN OUT AU1INT
.MODEL AU1INT int ( out_lower_limit=0 out_upper_limit=40e-6 )
The effect of the function can be seen in the resultant waveforms obtained by running a transient analysis of the circuit.
In this example, the following analysis parameters on the Transient/Fourier Analysis page of the Analyses Setup dialog have been used:
- Transient Start Time - set to
0.000 - Transient Stop Time - set to
5.000u - Transient Step Time - set to
20.00n - Transient Max Step Time - set to
20.00n