OS-1315: Modal Transient Dynamic Analysis of a Bracket

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

rd2030_pic1

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 modal 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). Modal damping has been defined as 2% critical damping for all the modes. Modes up to 1000 Hz have been considered. 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

Time history of applied loading

This tutorial uses the following exercises to set up a modal 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 modal damping table

•	Define load collector to extract normal modes up to 1000 Hz using the Lanczos method

•	Define the transient response dynamic excitation

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

•	Specify output requests

•	Run modal transient dynamic analysis

•	Post-process results using Altair HyperGraph

Exercise

Step 1: Launch HyperMesh and set the OptiStruct User Profile

1.	Launch HyperMesh.

2.	Select OptiStruct in the User Profiles dialog.

3.	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.

Step 2: Open the File

1.	Click File > Open. An Open Model browser window opens.

Note:

If HyperMesh Desktop was launched, use: File > Open > Model.

2.	Select the bracket_transient.hm file you saved to your working directory from the optistruct.zip file. Refer to Accessing the Model Files.

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

Step 3: Create a TABLED1 card to define time dependent dynamic load

1.	In the Model browser, right-click and select Create > Load Collector.

2.	For Name, enter tabled1.

3.	Click Color and select a color from the color palette.

4.	For Card Image, select TABLED1 from the drop-down menu.

5.	For TABLED1_NUM, enter a value of 4 and press enter.

6.	Click the Table icon below TABLED1_NUM and enter the values in the pop-out window, as shown in the figure below.

OS_1315_01

7.	Click Close. The load collector TABLED1 that defines the time history of the loading has been created.

Step 4: Create a TSTEP card (the transient time step to define the time step intervals at which solution is generated and output)

1.	In the Model browser, right-click and select Create > Load Collector.

2.	For Name, enter tstep.

3.	Click Color and select a color from the color palette.

4.	For Card Image, select TSTEP on the pop-up menu.

5.	For TSTEP_NUM, enter the number 1 and press ENTER.

6.	In the dialog, under N, enter the number of time steps as 800.

7.	To specify the time increment, enter 0.005 under DT. The total time applied to the load is: 800 x 0.005 = 4 seconds. NO has a default value of 1.0. This is the time step at which output is requested.

8.	Click Close to go back to the Entity Editor.

Step 5: Create DAREA card 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 from the pop-up menu. Two sets are displayed.

7.	Select force and click select. The nodes that belong to the set force are selected.

rd2030_pic3

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

9.	For dof3, enter a value of -1500.

10.	Set load types = to DAREA.

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

12.	Click return.

Step 6: Create a TABDMP1 card (the modal damping table to define damping as a tabular function of frequency)

1.	In the Model browser, right-click and select Create > Load Collector.

2.	For Name, enter tabdmp1.

3.	Click Color and select a color from the color palette.

4.	For Card Image, select TABDMP1 from the drop-down list.

5.	For TABDMP1_NUM, enter a value of 2 and press enter.

6.	Click below TABDMP1_NUM and enter the values in the pop-out window, as shown in the figure below.

7.	Populate the frequency and damping values for frequencies 0 and 1000 Hz and damping to be 0.02, as shown below. This provides a table of damping values for the frequency range of interest.

OS_1315_02

8.	Click Close to return to the Entity Editor.

9.	For TYPE, switch to CRIT to specify critical damping.

Step 7: Create an EIGRL load collector to extract modes up to 1000 Hz

1.	In the Model browser, right-click and select Create > Load Collector.

2.	For Name, enter eigrl.

3.	Click Color and select a color from the color palette.

4.	For Card Image, select EIGRL from the drop-down menu.

5.	For V1, enter 0.0.

6.	For V2, enter 1000.

7.	Leave the ND field blank to extract modes up to 1000 Hz.

Step 8: Create a TLOAD1 card (transient dynamic response excitation)

1.	In the Model browser, right-click and select Create > Load Collector.

2.	For Name, enter tload1.

3.	Click Color and select a color from the color palette.

4.	For Card Image, select TLOAD1 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 (created in the last section to define the forces on the top surface of the bracket).

7.	Click OK to complete the selection.

8.	Similarly select the tabled1 load collector 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 TLOAD1 card image defines the type of load. The type is set to applied load by default.

Step 9: Create the load step to perform the modal transient dynamic analysis

1.	In the Model browser, right-click and select Create > Load Step.

2.	For Name, enter transient.

3.	For Analysis type, select Transient (modal) from the drop-down menu.

4.	For SPC, select spc from the Select Loadcol pop-out window.

5.	For DLOAD, select tload1.

6.	For TSTEP(TIME), select tstep.

7.	For METHOD (STRUCT), select the load collector eigrl created previously.

8.	For SDAMPING (STRUCT, select the load collector tabdmp1 created previously. A subcase is created that specifies the loads, boundary conditions, and damping for modal transient dynamic analysis.

Step 10: Create output requests for transient dynamic analysis

1.	Click Setup > Create > Control Cards panel and select GLOBAL_OUTPUT_REQUEST.

2.	Select DISPLACEMENT and leave the field for FORMAT(1) blank.

3.	For FORM(1), select BOTH.

4.	For OPTION(1), select SID – . A yellow button SID appears.

5.	Double-click SID and select center.

The center set represents the node at the center of the spider attached to the mass element, which is node 395.

6.	Click return > next.

7.	Click OUTPUT.

8.	For number_of_outputs =, enter 2.

9.	For KEYWORD, select H3D and HGTRANS.

10.	For FREQ, select ALL for both.

11.	For the H3D KEYWORD you will have another field, set this to the blank option.

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

Step 11: Run the modal transient dynamic analysis

1.	From the Analysis page, click OptiStruct.

2.	Click save as following the input file: field. A Save Model browser window opens.

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

4.	Click Save.

The name and location of the bracket_transient_modal.fem file displays in the input file: field.

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. 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_modal.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:

bracket_transient_modal.html	HTML report of the analysis, giving a summary of the problem formulation and the results.
bracket_transient_modal.out	OptiStruct output file containing specific information on the file setup, the setup of the problem, estimates for the amount of RAM and disk space required for the run and compute time information. Review this file for warnings and errors that are flagged from processing the bracket_transient_modal.fem file.
bracket_transient_modal.h3d	HyperView binary results file.
bracket_transient_modal_tran.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.
bracket_transient_modal.stat	Summary of analysis process, providing CPU information for each step during analysis process.

Step 12: Post-process displacement results of node 395 using HyperGraph

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

2.	Click File > Open > Session.

3.	Select the HyperView session file bracket_transient_modal_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, you are interested in the z-displacement time history of node 395.

4.	Click Close and the Message Log opens.

5.	Click on the Curves 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 by then clicking the line attributes Off, as shown below.

rd2030_pic6

6.	Click to fit the y-axis (that is Z displacement) of node 395.

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

rd2030_pic7

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.