# OS-HM-T: 2000 Direct Transient Analysis of Airframe Model

This tutorial demonstrates how to perform direct transient dynamic analysis using OptiStruct using an existing finite element model of a wing structure. HyperView is used to post-process the deformation characteristics of the Wing Structure under the transient dynamic loads.

Before you begin, copy the file(s) used in this tutorial to your working directory.

The wing structure is constrained in all the DoFs at the bolt joints by using rigid elements represented by the rigid2 component. Transient dynamic pressure load is applied at the grid points in 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 3 seconds with the time divided into 30 increments (meaning the time step is 0.1).

The following exercises are included:
• Create the time-dependent dynamic pressure load or the variation of load versus time
• Create the time step for transient analysis
• Create the direct transient subcase to include the load collectors
• Run a direct transient dynamic analysis
• Post-process the results using HyperView

## Launch HyperWorks

1. Launch Altair HyperWorks.
2. In the New Session window, select HyperMesh from the list of tools.
3. For Profile, select OptiStruct.
4. Click Create Session.
This loads the user profile, including the appropriate template, menus, and functionalities of HyperMesh relevant for generating models for OptiStruct.

## Import the Model

1. On the menu bar, select File > Import > HyperMesh Model.
2. Navigate to and select wing_structure.fem.
3. Click Import.

## Set Up the Model

### Create a TABLED1 Curve

This table defines the time-dependent dynamic load.

1. On the Model ribbon, select Curves.
A new window of the curve editor opens.
2. Click to add a curve.
4. In the Table, right-click and select Add rows.
5. Enter the following values in the table.
Table 1. Curve Table Values
X Y
1 0.0 0.0
2 1.0 0.015
3 3.0 0.015
6. Close the curve editor.
7. In the Model Browser, double-click on Curves to open the Curves Browser tab.
8. In the browser tab, click LOAD_HISTORY.
9. Click Color and select a color from the color palette.
10. For Card Image, select TABLED1 from the drop-down menu.
The TABLED1 curve that defines the time history of the loading is created.

### Create a TSTEP

The transient time step defines the time step intervals at which the solution is generated and output.

1. In the Model Browser, select Create > Load Collector.
The Create Load Collector window opens.
2. For Name, enter TIMESTEP.
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 timesteps as 30.
7. For DT, enter the time increment of 0.1.
The total time applied to the load is 30 x 0.1 = 3.
8. Click Close.

### Create a Pressure Load Collector

1. In the Model Browser, select Create > Load Collector.
The Create Load Collector window opens.
2. For Name, enter Pressure.
3. Click Color and select a color from the color palette.
4. For Card Image, select None.
5. From the menu bar, select the Analyze ribbon.
6. On the ribbon, select the Loads tool.
7. On the panel, select the Create radio button.
8. From the first drop-down menu, select elems.
9. From the second drop-down menu, select faces.
10. Select faces on the model as shown below.
11. For magnitude, enter 1.0.
A pressure load of magnitude 1 MPA is applied.
12. From the first drop-down menu, change the button from normal to direction.
13. In the second drop-down menu, select z-axis as the axis of application of the pressure load.
15. Click Create.
A force of 1 MPA pressure load is applied to the selected nodes in the z-direction.

### Create an SPC Load Collector

In this step, an SPC load collector for constraints is created.

1. In the Model Browser, select Create > Load Collector.
The Create Load Collector window opens.
2. For Name, enter spc.
3. Click Color and select a color from the color palette.
4. For Card Image, select None.
5. From the menu bar, select the Analyze ribbon.
6. From the ribbon, select BCs > Constraints.
7. In the panel, select the Create radio button.
8. Select the nodes on the model as shown below.
9. Constrain the nodes in all the degrees of freedom.
10. Click Create.

This step creates the transient dynamic response excitation.

1. In the Model Browser, select Create > Load Step Inputs.
The Create Load Step Inputs window opens.
3. Click Color and select a color from the color palette.
4. For Config type, select Dynamic Load - Time Dependent from the drop-down list.
5. For Type, select TLOAD1 from the drop-down list.
6. For Exciteid, click Unspecified and select to open the Advanced Selection dialog.
Tip: You can also press the Spacebar to open Advanced Selection.
7. In the dialog, select Pressure from the list of load collectors.
8. Click Apply, then OK
9. Similarly, for the TID field select the LOAD_HISTORY curve 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.
10. Click Close.

In this step, a load step for Direct Transient Analysis is created.

1. In the Model Browser, select Create > Load Step.
2. For Name, enter transient.
3. For Analysis type, select Transient (direct) from the drop-down menu.
4. For SPC, click Unspecified and select to open the Advanced Selection dialog.
Tip: You can also press the Spacebar to open Advanced Selection.
5. In the dialog, select spc from the list of load collectors.
6. Click OK
8. For TSTEP (TIME) select the TIMESTEP load collector.
9. Click Close.
A subcase is created that specifies the loads and boundary conditions for direct transient dynamic analysis.

### Create Output Request

In this step, the output request for Transient Dynamic Analysis is created.

1. On the Analyze ribbon, under the Analyze tool group, select Run > Control Cards.
The Control Cards panel opens.
2. In the panel, select PARAM.
3. Select PRGPST from the drop-down menu.
4. Click No.
5. Click return.
With this setting, autospc is not printed in the output file.
6. On the panel, select GLOBAL_OUTPUT_REQUEST.
7. Select STRESS.
8. For FORMAT, select H3D.
9. For OPTIONS, select ALL.
10. Click return.
11. Similarly, select DISPLACEMENT and SPF and specify the same FORMAT and OPTIONS settings.

## Save the Database

Set the directory in which to save the file.

1. Click File > Save.
2. For File name, enter wing_structure.hm.
3. Click Save.

## Run Direct Transient Analysis

1. From the menu bar, select Analyze.
2. On the Analyze ribbon, under the Analyze tool group, select Run OptiStruct Solver .
The panel area opens.
3. Click Save as.
4. For File name, enter wing_structure.fem.
The name and location of the file are displayed in the input file: field.
5. Set export options: to all.
6. Set run options: to analysis.
7. Set memory options: to memory default.
8. Click OptiStruct to launch the job.
If the job was successful, new results files appear in the directory where the OptiStruct model file was written. The wing_structure.out file is a good place to look for error messages to help debug the input deck if any errors are present.
The default files written to the directory are:
Table 2. Default Output Files
File Name Description
wing_structure.html HTML report of the analysis giving a summary of the problem formulation and the results.
wing_structure.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 wing_structure.fem file.
wing_structure.h3d HyperView binary results file.
wing_structure.mvw HyperView session file. This file is only created when the transient analysis is performed. This file automatically creates plots for the displacement, velocity, and acceleration results contained in the file.
wing_structure.stat Summary of the analysis process, providing CPU information for each step during the analysis process.

## Post-Process the Results

In this step, the wing structure results are reviewed in HyperMesh.

1. In HyperMesh menu bar, select Post.
2. On the Post ribbon, select Results.
3. From the Results Browser, right-click the last timestep in the results and select Make Current from the context menu.
4. On the Post ribbon, select Contour.
5. In the Contour window, for Data type select Displacement.
6. For Component, select Z-direction.
7. In the modeling window, select all components.
8. Close the Contour window and select to plot the result.
9. Similarly, plot the results for Von Mises element stresses (2D & 3D).