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
-
Launch HyperMesh.
The User Profile dialog opens.
-
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
-
Click
.An Import tab is added to your tab menu.
- For the File type, select OptiStruct.
-
Select the Files icon .
A Select OptiStruct file browser opens.
- Select the bracket_transient.hm file you saved to your working directory.
- Click Open.
- Click Import, then click Close to close the Import tab.
Set Up the Model
Create TABLED1 Curve
- In the Model Browser, right-click and select .
- For Name, enter tabled1.
-
In the Curve Editor window, enter the values shown in Figure 3.
- Close the Curve Editor.
- In Curves, select tabled1.
- Click Color and select a color from the color palette.
- For Card Image, select TABLED1 from the drop-down menu.
-
Click Close.
The TABLED1 that defines the time history of the loading has been created.
Create TSTEP Load Collector
- In the Model Browser, right-click and select .
-
For Name, enter tstep.
Transient time step to define the time step intervals at which solution is generated and output.
- Click Color and select a color from the color palette.
- For Card Image, select TSTEP from the drop-down menu.
- For TSTEP_NUM, enter 1 and press Enter.
- For N, enter the number of time steps as 800.
-
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.
- Click Close.
Create a DAREA Load Collector
To define forces on the top surface of the bracket.
- In the Model Browser, right-click and select .
- For Name, enter darea.
- Click Color and select a color from the color palette.
- For Card Image, select NONE.
- Click to open the Constraints panel.
-
Click
.Two sets are displayed.
-
Select force and click select.
The nodes that belong to the set force get selected.
- 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.
- For dof3, enter a value of -1500.
- For load types=, select DAREA.
-
Click create.
This creates a force of 1500 units applied to the selected nodes in the negative z direction.
- Click return to go back to the main menu.
Create a TLOAD Load Step Input
- In the Model Browser, right-click and select .
- For Name, enter tload1.
- For Config type, select Dynamic Load – Time Dependent from the drop-down list
- For Type, select TLOAD1 from the drop-down menu.
- For Exciteid , click .
- In the Select Loadcol dialog, select darea from the list of load collectors.
- Click OK to complete the selection.
-
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.
Create a Load Step
Load Step to perform Direct Transient Analysis.
-
In the Model Browser, right-click and
select .
A default load step template is now displayed in the Entity Editor below the Model Browser.
- For Name, enter transient.
- For Analysis type, select Transient(direct) from the drop-down menu.
- From the Select Loadcol dialog, select spcs.
- For DLOAD, select tload1 from the Select Load Step Inputs pop-out window.
-
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
- Click to enter the Control Cards panel.
- Click next to view more cards.
- Click PARAM to define parameter cards.
-
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.
-
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.
- Click return.
Create Output Requests
- Click GLOBAL_OUTPUT_REQUESTS and select DISPLACEMENT and leave the space beneath FORMAT blank.
- For FORM(1), select BOTH.
-
For OPTION(1), select SID.
A yellow button labeled SID appears.
- Double-click on SID and select center.
-
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.
- Click .
- Click OUTPUT.
- Under number_of_outputs =, enter 2.
- For KEYWORD, select H3D and HGTRANS.
- For FREQ, select ALL for both.
- Click return twice to exit from the Control Cards panel.
Save the Database
Set the directory in which to save the file.
- Click .
- For File name, enter bracket_transient_direct.hm.
- Click Save.
Submit the Job
-
From the Analysis page, click the OptiStruct
panel.
- Click save as.
-
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.
-
Click Save.
The input file field displays the filename and location specified in the Save As dialog.
- Set the export options toggle to all.
- Set the run options toggle to analysis.
- Set the memory options toggle to memory default.
- Click OptiStruct to launch the OptiStruct job.
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.
Post-process Displacement Results
- From the OptiStruct panel, click HyperView to launch HyperView.
- Click .
-
Select the HyperView session file
bracket_transient_direct.mvw from the
directory in which the input file was run.
The following prompt appears:
-
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.
-
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:
- Click to fit the y-axis (that is Z displacement) of node 395 in the GUI.
-
You can change the color and/or line attributes of the curve if you want
to.