Direct Transient Dynamic Analysis of a Bracket - OS-1120

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

Finite element model of the bracket

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 the next figure. The direct transient analysis is run for a total time of 4 seconds with the time being divided into 800 increments (i.e. 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.

Time history of applied loading

This tutorial will use the following steps to set up direct transient dynamic analysis:

·      Define the time dependent dynamic load or the variation of load vs time

·      Define the time step for transient analysis

·      Define the grid point forces on the top flat surface of the bracket

·      Define the transient response dynamic excitation

·      Define the subcase to include all the necessary loads as defined above

·      Specify structural damping and output requests

·      Run direct transient dynamic analysis

·      Post-process results using Altair HyperGraph

To load the OptiStruct user profile and open the model file:

1. Launch HyperMesh and choose the OptiStruct user profile in the User Profiles dialog.

User Profiles… can also be accessed from the Preferences pull-down menu on the toolbar.

2. Click the Files panel toolbar button .

3. Select the hm file subpanel using the radio buttons on the left-hand side of the panel.

4. Click retrieve….

An Open file… browser window pops up.

5. Select the bracket_transient.hm file, located in <install_directory>/tutorials/os/.

6. Click Open.

The bracket_transient.hm database is loaded into the current HyperMesh session, replacing any existing data.

7. Click return to go to the main menu.

To create a TABLED1 (table to define time dependent dynamic load):

1. Click the Collectors toolbar button .

2. Select the create subpanel, using the radio buttons on the left side of the panel.

3. Click the collector type switch and select load collectors from the pop-up menu.

4. Click name = and enter tabled1.

5. Click card image= and choose TABLED1 from the pop-up menu.

6. Click create/edit.

7. Click TABLED1_NUM = and input the number 4.

8. Press ENTER.

This should populate the TABLED1 entry to 4 fields for x and 4 for y.

9. Leave both XAXIS and YAXIS as LINEAR.

10. Type the following values for x1 and y1 as shown below:

11. Click return.

The load collector tabled1 that defines the time history of the loading has been created.

To create a TSTEP (the transient time step to define the time step intervals at which solution will be generated and output):

1. In the Collectors panel , select the create subpanel.

2. Make sure that the collector type switch is set to load collectors.

3. Click name = and enter tstep.

4. Click card image= and choose TSTEP from the pop-up menu.

5. Click create/edit.

6. Click TSTEP_NUM = and enter 1.

7. Press ENTER.

8. To specify the number of timesteps, enter 800 under N.

9. To specify the time increment, enter 0.005 under DT.

The total time for which the load is applied is 800 x 0.005 = 4 seconds.

10. Leave N0 as the default value 1 (this is the time step at which output is requested).

11. Click return.

To create a DAREA to define forces on the top surface of the bracket:

1. In the Collectors panel , select the create subpanel using the radio buttons.

2. Make sure that the collector type switch is set to load collectors.

3. Click name = and enter darea.

4. Click the switch next to card image and choose no card image.

5. Click create.

6. Click return.

7. From the Analysis page, click the load types panel.

8. Click constraint = and select DAREA.

9. Click return.

10. Click the constraints panel and make sure that the create subpanel is active.

11. Click nodes, and select by sets from the pop-up menu.

12. Two sets are displayed, choose force and click select.

The nodes that belong to the set force get selected as shown below.

13. Unselect (right click) all degrees of freedom (dof) except dof3, indicating that dof3 is the only active degree of freedom.

14. Enter a value of -1500 for dof3.

15. Click create.

This creates a force of 1500 units applied to the selected nodes in the negative z direction.

16. Click return.

Grid point forces have been created on the top of the bracket.

To create a TLOAD1 (the transient dynamic response excitation):

1. In the Collectors panel , make sure that the create subpanel is active.

2. Verify that the collector type switch is set to load collectors.

3. Click name = and enter tload1.

4. Click card image= and choose TLOAD1 from the pop-up menu.

5. Click create/edit.

6. Click on EXCITEID and choose the darea load collector (created in the last section to define the forces on the top surface of the bracket).

7. Click on TID and choose the tabled1 load collector created previously (to define the time history of the loading).

8. Click return twice to exit from the Collectors panel.

To create the load step to perform the direct transient dynamic analysis:

1. From the Analysis page, choose the subcase panel.

2. Click name = and enter transient.

3. Toggle the type: and select transient (direct).

4. Activate SPC and for SPC =, select the already existing load collector spc.

5. Activate DLOAD and for DLOAD =, select the load collector tload1 created previously.

6. Activate TSTEP and for TSTEP =, select the load collector tstep created previously.

7. Make sure that the TIME/FOURIER toggle is set to TIME.

8. Click create.

9. Click return.

A subcase is created that specifies the loads and boundary conditions for direct transient dynamic analysis.

To create Damping parameters for transient dynamic analysis:

1. From the Analysis page, select the control cards panel.

2. Click next to see more cards.

3. Click PARAM to define parameter cards.

4. Activate G, click on G_V1, and enter 0.2.

This parameter is used to specify the uniform structural damping coefficient for the direct transient dynamic analysis.

5. Activate W3 and, under W3_V1, input 300.

This parameter is used in transient analysis to convert structural damping to equivalent viscous damping.

6. Click return twice.

To create output requests for transient dynamic analysis:

1. From the Analysis page, select the control cards panel.

2. Select DISPLACEMENTS and leave the space beneath FORMAT blank.

3. For DISP_FORM, select BOTH.

4. For DISP_OPT, select SID.

A yellow button labeled SID pops up.

5. Click on SID and select center

6. Choose the option for center as shown below.

This set represents the node at the center of the spider attached to the mass element, i.e. node 395.

7. Click return.

8. Click next.

9. Click OUTPUT.

10. Under number_of_outputs =, enter 2.

11. For KEYWORD, select H3D and HGTRANS.

12. For FREQ, select ALL for both.

13. Click return twice to exit from the Control Cards panel.

To run the direct transient dynamic analysis:

1. From the Analysis page, select the OptiStruct panel.

2. Click save as… following the input file: field

A Save file… browser window pops up.

3. Select the directory where you would like to write the file and enter the name bracket_transient_direct.fem in the File name: field.

4. Click Save.

Note that the name and location of the bracket_transient_direct.fem file shows in the input file: field.

5. Set the memory options: toggle to memory default.

6. Click the run options: switch and select analysis.

7. Set the export options: toggle to all.

8. Click OptiStruct.

This launches the OptiStruct job.

If the job was successful, new results files can be seen in the directory where the OptiStruct model file was written. The bracket_transient_direct.out file is a good place to look for error messages that will help to debug the input deck if any errors are present.

The default files written to the directory are:

Post-process displacement results of node 395 using HyperGraph:

1. From the OptiStruct panel, click the HyperView button to launch HyperView.

2. Change the application from HyperView to HyperGraph using the switch to the left of the toolbar buttons.

The following prompt appears: This operation will erase data in the current window. Do you wish to continue?

3. Click Yes.

4. Select File from the pull-down menu and select Open.

5. Select the HyperView session file bracket_transient_direct_tran.mvw from the directory in which the input file was run. This file automatically creates plots for the displacement results contained in the file.

Since the loading is applied only in the z-direction, we are interested in the z-displacement time history of node 395.

6. Click on the Entity Attributes toolbar button 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 by then clicking the line attributes Off as shown below.

7. Select Fit Y in the view controls section to fit the y-axis (i.e. Z displacement) of node 395 in the GUI.

8. You can change the color and/or line attributes of the curve if you wish.

z-displacement time history of the concentrated mass at center of spider for direct transient dynamic analysis

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.

Go To

OptiStruct Tutorials