Transient Stress - Modal Superposition

Set up Events

There are three parameters that define the event in a transient stress analysis. These are specified in the Event section of the Analysis Parameters dialog box. The Number of time steps and Time-step size fields must be defined to perform the analysis. The results are calculated for each time step and are written to output files. The results in these output files can be viewed in the Results environment. If you do not want the results at each time step to be written to the output files, specify a value larger than 1 in the Output interval field.

The Percent memory allocation on the Analysis Parameters dialog box controls how much of the available RAM is used to read the element data and to assemble the matrices. (When the value is less than or equal to 100%, the available physical memory is used. When the value of this input is greater than 100%, the memory allocation uses available physical and virtual memory.)

Since the Transient Stress (Modal Superposition) analysis uses the results from a modal analysis, specify which design scenario in the current model has the modal results with the Use modal results from design scenario field.

Note: The Model Units of the transient stress analysis must be identical to the Model Units of the modal results.

Apply Global Damping

Damping can be applied to the entire model using the Damping section of the Analysis Parameters dialog box. Specify the fraction of the model's critical damping to be applied in the Damping Factor (Fraction of Critical) field. This value must be between 0 and 1.

Define Load Curves

In a transient stress analysis, all the loads follow load curves. The load curves are defined in the Analysis Parameters dialog box by pressing the Load Curves button. There are two methods that can be used to create the load curves. If you select the Piecewise Linear radio button in the Load Curve Form section, you can define the load curve by defining several times and the corresponding factors. The factor values is linearly interpolated between the defined times. If you select the Sinusoidal radio button in the Load Curve Form section, you can define the parameters of the sinusoidal curve in the fields below. The value in the Factor column multiplies the magnitude of the load at the given time.

Apply Forces and Moments

Use the transient stress analysis to apply nodal force and moment loads through the Dynamic Load Data table in the Loads tab of the Analysis Parameters dialog box. nodal forces added to the vertices of the model are ignored.

First, you must specify the number of the node to which the load is applied in the Node Number column. This can be obtained from the Results environment. (Using the modal analysis model is the easiest method to obtain the node numbers.)
Next you must specify which load curve the load follows in the Load Curve column.
To apply a force, enter a 0 in the Type column. To apply a moment, enter a 1 in the Type column.
Next, specify the component of the load that is applied in each of the three directions in the X Scale, Y Scale, and Z Scale columns. The directions follow the local coordinate system to which the node is assigned. For example, X Scale follows the radial direction in a cylindrical coordinate system. (See the page Setting Up and Performing the Analysis: Using Local Coordinate Systems for additional details.) For force loads, the input in these columns is in units of force. For moment loads, the input in these columns is in units of length*force. The total load at any time during the analysis is the entered scale factors multiplied by the load curve factor.
Finally, specify the time at which the load is applied in the Activation Time column. The load starts to follow the load curve from time 0 at this time.

Note: The nodal loads applied to the model are not shown in the Results environment.

Apply Ground Motion

Ground motion can be applied to all the nodes in the model to which a boundary condition is applied. This can be set up in the Options tab of the Analysis Parameters dialog box. Select the Translation option in the Ground Motion Type drop-down menu and then press the Setup button.

In the Ground Motion Setup dialog box, specify the Acceleration Magnitude, Load Curve, and Activation Time for the ground motion to be applied in each global direction. The acceleration at any given time equals the entered acceleration magnitude value multiplied by the interpolated load curve factor.

Control Data in Output Files

By default, the calculated strain is output to the binary results file so that the strain can be viewed in the Results Environment. If for some reason you did not want the strain results, some computational time and disk space could be saved by activating the Disable calculation and output of strains option on the Options tab of the Analysis Parameters dialog box.

As the analysis is performed, the input and additional results can be output to various files. The Output tab of the Analysis Parameters dialog box can be used to control the data that is output. Except as noted, this additional output is text based, so these options do not affect the results that can be viewed in the Results Environment.

Activating the Displacement Data option writes the displacement results to the text summary file. Depending on the model size and the number of output time steps, this could make the file very large.
Activating the Stress data option writes the stress results to a text file. Depending on the model size and number of output time steps, this file could be very large.
Activating the Stress/strain at midside nodes (binary) check box outputs the stress and strain at midside nodes to the binary result files. These results can then be displayed in the Results environment. (Midside nodes are an option that can be activated for certain element types using the Element Definition dialog box.)

Using the Output Type Indicator drop-down menu, you can choose to output either the Maxima only or the Histories and Maxima for the nodes specified in the Supplemental Displacement Reporting Locations dialog box which is accessed by pressing the Print Setup.. button. The Maxima only option outputs the time and magnitude of the maximum translation or rotation of a particular node to the summary file. The Histories and Maxima option outputs the magnitude of the translation or rotation of a particular node at every time step to the summary file. This option also tells you when the maximum translation or rotation occurred and the value. In the Supplemental Displacement Reporting Locations dialog box, Specify the node number for which you want the output in the Node column. Then click the degree of freedom that you want the output for at that node. The value in that column changes to Yes.