Transient Stress -Direct Integration

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.

Apply Global Damping

Damping can be applied to the entire model using the Damping section of the Analysis Parameters dialog box. The values in the Alpha and Beta fields is used to create the damping matrix, [C], using the equation, [C] = ALPHA * [M] + BETA * [K] where [M] is the mass matrix, and [K] is the stiffness matrix.

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

In addition to applying forces and moments to nodes in the display area, use the transient stress analysis to apply these loads through the Dynamic Load Data table in the Loads tab of the Analysis Parameters dialog box. First, you must specify the number of the node to which the load is applied in the Node Number column. 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 scale factor that is applied to the load in each of the three global directions in the X Scale, Y Scale, and Z Scale columns. 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.

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.

Solution Options Section

The type of solver for a transient stress analysis can be selected in the Type of solver drop-down menu on the Options tab of the Analysis Parameters dialog box. See also Solvers in Finite Element Analysis for background information. The options available are as follows:

Automatic:. If this option is selected, the processor chooses between the available solvers based on the model size. The sparse solver (BCSLIB-EXT) is the optimum solver for mid-sized and large models.
BCSLIB-EXT: Uses the BCSLIB-EXT sparse solver. The sparse solver uses multiple threads/cores when available. If a 64 bit processor is available on the system, the BCSLIB-EXT solver takes advantage of it.

The sparse solver takes advantage of multiple threads/cores installed in the computer. The drop-down Number of threads/cores control is enabled when the type of solver is automatic or BCSLIB-EXT. You want to use all the threads/cores available for the fastest solution, but might choose to use fewer threads/cores if you need some computer power to run other applications at the same time as the analysis.

If for some reason you want to create the stiffness matrix but not perform the analysis, activate the check box for Stop after stiffness calculations. The only time this is useful is if you are using the stiffness matrix for other purposes, such as accessing it from another program. The stiffness matrix is always calculated when running an analysis, so there is no advantage to use this option in normal circumstances.

The Solver memory allocation field sets the amount of memory to use during the sparse matrix solution for the BCSLIB-EXT solver. In general, allocating more memory should result in a faster analysis.

For the sparse solver, the Percent memory allocation field controls how much of the available RAM is used to read the element data and to assemble the matrices. A small value is recommended. (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.)

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 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 Equation numbers data option writes a table that correlates the node numbers to the degrees of freedom (DOF) and equations in the solution matrix. This option is useful mainly when a warning or error message is given that references a DOF or equation. By searching this table for the DOF or equation number, the corresponding node number can be determined, and the node number can be located in the Results Environment (using the Result Inquire Inquire Current Results Specify command).
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.)
Activating the Element data or Nodal data outputs the element connectivity and nodal coordinates, respectively, for the entire model to the summary file.

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 filename.l4 file. The Histories and Maxima option outputs the magnitude of the translation or rotation of a particular node at every time step to the filename.l4 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.

Contact Settings

There are two methods of handling bonded connections. Which method is used depends in part on whether the nodes are matched between the two parts or not matched.

Activating the option Enable smart bonded/welded contact on the Contact tab uses multi-point constraint equations (MPCs) when necessary to bond the nodes on part A, surface B with the nearest nodes on part C, surface D. Shape functions interpolate the displacements at the nodes on surface B to the nodes on surface D. Therefore, the meshes do not need to match between the parts. The MPCs are used for all the nodes on the surface contact pair whenever any node does not match. If the meshes do match at all nodes, then node matching is used to bond the contact surface; the two vertices on the adjoining parts are collapsed to one node, and MPC equations are not used for the contacting surfaces. The options for the smart bonding drop-down are as follows:

None: Smart bonding is not used. Therefore, the nodes must match for parts to be bonded.
Coarse bonded to fine mesh: Smart bonding creates MPC equations that connect the nodes on the surface with the coarser mesh to the nodes on the surface with the finer mesh.
Fine bonded to coarse mesh: Smart bonding creates MPC equations that connect the nodes on the surface with the finer mesh to the nodes on the surface with the coarser mesh.

The smart bonding option applies to bonded contact and welded contact. See the page Meshing Overview: Creating Contact Pairs: Types of Contact for a discussion of defining contact and additional information about using smart bonding.

By default, smart bonding uses the condensation method to solve your analysis. If you find your analysis doesn't converge or is not performing as you expect, you can try a different Solution method to use with MPC equations (see Multi-Point Constraints). Click SetupLoadsMulti-Point Constraint and choose from the Solution method options. If you use the Penalty Method, the accuracy of the solution is controlled by the Penalty multiplier field. The Penalty multiplier, times the maximum diagonal stiffness in the model, is used during the penalty solution. A value in the range of 10⁴ to 10⁶ is recommended.

Note:

The solution method you select in the Define Multi-Point Constraints dialog box becomes the method used for all features that include MPCs. These features include, but are not limited to, cyclic symmetry, frictionless constraints, smart bonding, and user-defined MPCs. For example, if you want to use the Penalty Method to solve all your analyses involving smart bonding, you can override the default condensation method by selecting Penalty Method in the Define Multi-Point Constraints dialog box.
Smart bonding applied to contact between brick, 2D, membrane, and plate elements. Bonded contact involving other element types requires the nodes to match and are not affected by the smart bonding setting.

When the option Enable smart bonded/welded contact is not activated, the parts are bonded only if the nodes match between the parts.