DDTR - Differentiator (Differential IO)

Old Content - visit altium.com/documentation

Model Kind

General

Model Sub-Kind

Generic Editor

SPICE Prefix

A

Model Name

DDTR

SPICE Netlist Template Format

@DESIGNATOR %%vd(%1,%2) %%vd(%3,%4) @"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 differential current or differential voltage signal.

Examples

Consider the differentiator function in the above image, with the following characteristics:

  • Pin1 (positive input) is connected to net IN
  • Pin2 (negative input) is connected to net GND
  • Pin3 (positive output) is connected to net OUT
  • Pin4 (negative output) is connected to net GND
  • 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 %vd(IN,0) %vd(OUT,0) 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
You are reporting an issue with the following selected text and/or image within the active document: