OS-T: 1310 Direct Transient Dynamic Analysis of a Bracket

In this tutorial, an existing finite element model of a bracket is used to demonstrate how to perform direct transient dynamic analysis using OptiStruct. HyperGraph is used to post-process the deformation characteristics of the bracket under the transient dynamic loads.

Before you begin, copy the file(s) used in this tutorial to your working directory.
The bracket is constrained at the bottom of the two legs. Transient dynamic loads are to be applied at the grid points of the top, flat surface of the bracket around the hole in the negative z direction. The time history of the loading is shown in Figure 2. The direct transient analysis is run for a total time of 4 seconds with the time being divided into 800 increments (that is time step is 0.005). Structural damping has been considered for the model. A concentrated mass element is defined at the center of the spider and z displacements are monitored at the concentrated mass at the center of this hole.

Launch HyperMesh and Set the OptiStruct User Profile

1. Launch HyperMesh.
The User Profile dialog opens.
2. Select OptiStruct and click OK.
This loads the user profile. It includes the appropriate template, macro menu, and import reader, paring down the functionality of HyperMesh to what is relevant for generating models for OptiStruct.

Import the Model

1. Click File > Import > Solver Deck.
2. For the File type, select OptiStruct.
3. Select the Files icon .
A Select OptiStruct file browser opens.
4. Select the bracket_transient.hm file you saved to your working directory.
5. Click Open.
6. Click Import, then click Close to close the Import tab.

Set Up the Model

Create TABLED1 Curve

1. In the Model Browser, right-click and select Create > Curve.
2. For Name, enter tabled1.
3. In the Curve Editor window, enter the values shown in Figure 3.
4. Close the Curve Editor.
5. In Curves, select tabled1.
6. Click Color and select a color from the color palette.
7. For Card Image, select TABLED1 from the drop-down menu.
8. Click Close.
The TABLED1 that defines the time history of the loading has been created.

1. In the Model Browser, right-click and select Create > Load Collector.
2. For Name, enter tstep.

Transient time step to define the time step intervals at which solution is generated and output.

3. Click Color and select a color from the color palette.
4. For Card Image, select TSTEP from the drop-down menu.
5. For TSTEP_NUM, enter 1 and press Enter.
6. For N, enter the number of time steps as 800.
7. For DT, enter the time increment of 0.005.
The total time applied to the load is: 800 x 0.005 = 4 seconds. This is the time step at which output is requested. NO has a default value of 1.0.
8. Click Close.

To define forces on the top surface of the bracket.

1. In the Model Browser, right-click and select Create > Load Collector.
2. For Name, enter darea.
3. Click Color and select a color from the color palette.
4. For Card Image, select NONE.
5. Click BCs > Create > Constraints to open the Constraints panel.
6. Click nodes > by sets.
Two sets are displayed.
7. Select force and click select.
The nodes that belong to the set force get selected.
8. Uncheck all degrees of freedom (dof), except dof3 by clicking the box next to each, indicating that dof3 is the only active degree of freedom.
9. For dof3, enter a value of -1500.
10. For load types=, select DAREA.
11. Click create.
This creates a force of 1500 units applied to the selected nodes in the negative z direction.

1. In the Model Browser, right-click and select Create > Load Step Inputs.
3. For Config type, select Dynamic Load – Time Dependent from the drop-down list
5. For Exciteid , click Unspecified > Loadcol.
6. In the Select Loadcol dialog, select darea from the list of load collectors.
7. Click OK to complete the selection.
8. Similarly select the tabled1 curves for the TID field (to define the time history of the loading).
The type of excitation can be an applied load (force or moment), an enforced displacement, velocity, or acceleration. The field [TYPE] in the TLOAD load step input defines the type of load. The type is set to applied load by default.

Load Step to perform Direct Transient Analysis.

1. In the Model Browser, right-click and select Create > Load Step.
A default load step template is now displayed in the Entity Editor below the Model Browser.
2. For Name, enter transient.
3. For Analysis type, select Transient(direct) from the drop-down menu.
4. From the Select Loadcol dialog, select spcs.
6. Activate TSTEP(TIME) and select the load collector tstep created previously.
A subcase is created that specifies the loads and boundary conditions for direct transient dynamic analysis.

Create Damping Parameters

1. Click Setup > Create > Control Cards to enter the Control Cards panel.
2. Click next to view more cards.
3. Click PARAM to define parameter cards.
4. Scroll down to activate G, click on G_V1, and enter 0.2.
This parameter specifies the uniform structural damping coefficient for the direct transient dynamic analysis.
5. Scroll down to activate W3, click on W3_V1, enter 300.
This parameter is used in transient analysis to convert structural damping to equivalent viscous damping.
6. Click return.

Create Output Requests

1. Click GLOBAL_OUTPUT_REQUESTS and select DISPLACEMENT and leave the space beneath FORMAT blank.
2. For FORM(1), select BOTH.
3. For OPTION(1), select SID.
A yellow button labeled SID appears.
4. Double-click on SID and select center.
5. Select the option for center.
This set represents the node at the center of the spider attached to the mass element that is node 395.
6. Click return > next.
7. Click OUTPUT.
8. Under number_of_outputs =, enter 2.
9. For KEYWORD, select H3D and HGTRANS.
10. For FREQ, select ALL for both.
11. Click return twice to exit from the Control Cards panel.

Save the Database

Set the directory in which to save the file.

1. Click File > Save as > Model.
2. For File name, enter bracket_transient_direct.hm.
3. Click Save.

Submit the Job

1. From the Analysis page, click the OptiStruct panel.
2. Click save as.
3. In the Save As dialog, specify location to write the OptiStruct model file and enter bracket_transient_direct for filename.
For OptiStruct input decks, .fem is the recommended extension.
4. Click Save.
The input file field displays the filename and location specified in the Save As dialog.
5. Set the export options toggle to all.
6. Set the run options toggle to analysis.
7. Set the memory options toggle to memory default.
8. Click OptiStruct to launch the OptiStruct job.
If the job is successful, new results files should be in the directory where the bracket_transient_direct.fem was written. The bracket_transient_direct.out file is a good place to look for error messages that could help debug the input deck if any errors are present.
The default files written to the directory are:
bracket_transient_direct.html
HTML report of the analysis, providing a summary of the problem formulation and the analysis results.
bracket_transient_direct.out
OptiStruct output file containing specific information on the file setup, the setup of your optimization problem, estimates for the amount of RAM and disk space required for the run, information for each of the optimization iterations, and compute time information. Review this file for warnings and errors.
bracket_transient_direct.h3d
HyperView binary results file.
bracket_transient_direct.res
HyperMesh binary results file.
bracket_transient_direct.stat
Summary, providing CPU information for each step during analysis process.
bracket_transient_direct.mvw
HyperView session file.
This file is only created when transient analysis is performed. This file automatically creates plots for the displacement, velocity and acceleration results contained in the file.

Post-process Displacement Results

1. From the OptiStruct panel, click HyperView to launch HyperView.
2. Click File > Open > Session.
3. Select the HyperView session file bracket_transient_direct.mvw from the directory in which the input file was run.
The following prompt appears:
4. Click Yes to close the message window.
Since the loading is applied only in the z-direction, you are interested in the z-displacement time history of node 395.
This file automatically creates plots for the displacement results contained in the file.
5. Click on the Curve Attributes toolbar icon and turn off the curves X Trans and Y Trans. This can be done by selecting the individual curves (X Trans and Y Trans) and then by clicking the line attributes Off, as shown below:
6. Click to fit the y-axis (that is Z displacement) of node 395 in the GUI.
7. You can change the color and/or line attributes of the curve if you wish to.
As can be observed from the above image, the displacements of node 395 are in the negative z-direction as the loading is in the -z direction too. The displacements eventually damp out due to the structural damping present in the model.