DDT - Differentiator (Single-Ended IO)
Model Kind
General
Model Sub-Kind
Generic Editor
SPICE Prefix
A
Model Name
DDT
SPICE Netlist Template Format
@DESIGNATOR %1 %2 @"DESIGNATOR"DDT
.MODEL @"DESIGNATOR"DDT d_dt (?out_offset|out_offset=@out_offset| ?gain|gain=@gain| out_lower_limit=@out_lower_limit out_upper_limit=@out_upper_limit ?limit_range|limit_range=@limit_range|)
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.
| Out_Offset | output 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). |
Notes
This model is a simple derivative stage that approximates the time derivative of an input signal by calculating the incremental slope of that signal since the previous time point.
The output upper and lower limits are used to prevent convergence errors due to excessively high output values.
The Limit_Range specifies the value below Out_Upper_Limit and above Out_Lower_Limit at which smoothing of the output begins.
The Differentiator function does not include truncation error-checking. It is therefore not recommended that this function be used to provide integration through the use of a feedback loop. Undesirable results may be obtained. It is better in this case, to use the Integrator function, which provides for truncation error-checking.
The input signal can be either a single-ended current or single-ended voltage signal.
Examples
Consider the differentiator 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 =
-20 - Out_Upper_Limit =
20 - All other parameters are left at their default values.
The entry in the SPICE netlist would be:
*Schematic Netlist:
AU1 IN OUT AU1DDT
.MODEL AU1DDT d_dt ( out_lower_limit=-20 out_upper_limit=20 )
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
225.0u - Transient Step Time - set to
900.0n - Transient Max Step Time - set to
900.0n