RD-1070: Analysis of an Axi-symmetric Structure using RADIOSS

Transcription

1 RADIOSS, MotionSolve, and OptiStruct RD-1070: Analysis of an Axi-symmetric Structure using RADIOSS In this tutorial, you will learn the method of modeling an axi- symmetry problem in RADIOSS. The figure below shows the model that will be used for this exercise. Full model; Elements, material, props and BC s The following exercises are included: 1. Analysis with the full model Retrieving the HyperMesh database file Submitting the job Viewing the results in HyperView 2. Analysis with a small portion of the full model with axi- symmetry boundary conditions Setting up the axi- symmetric structure in HyperMesh Submitting the job Viewing the results in HyperView Exercise 1: Analysis with the Full Model Step 1: Launch HyperMesh and set the RADIOSS User Profile 1. Launch HyperMesh.

2 A User Profiles Graphic User Interface (GUI) will appear. 2. Select RADIOSS in the User Profile dialog. 3. From the extended list, select BulkData. 4. 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 in Bulk Data Format for RADIOSS and OptiStruct. Step 2: Open the File axi-symmetry_full_geometry.hm 1. Click File > Open. An Open Model browser window opens. Note: If HyperMesh Desktop was launched, please use: File > Open > Model. 2. Select the axi-symmetry_full_geometry.hmfile, located in the HyperWorks installation directory under <install_directory>/tutorials/hwsolvers/radioss/. 3. Click Open. The axi-symmetry_full_geometry.hmdatabase is loaded into the current HyperMesh session, replacing any existing data. The database only contains geometric data. You will find that the structural model has already been set up with the necessary elements, boundary conditions, property, and material data so that it is ready to solve. Pressure load is applied on the top face of the geometry and constraints are defined at the bottom face. Note that the model is symmetrical about the z- axis and that loads and boundary conditions are symmetrical about the same axis as well. These represent the conditions necessary for modeling axi- symmetry problems. First, we will obtain the result for the full model and then we will model a small part of the model with boundary conditions suitable to enforce the axi- symmetric behavior. Finally, we will compare the results of the axi- symmetric model with the full model results. In the next section, we will solve the job and post process the results. Submitting the Job 1. From the Analysis page, enter the Radioss panel. 2. Click save as following the input file: field. A Save As browser window appears. 3. Select the directory where you would like to write the RADIOSS model file and enter the name for the model, axi-symmetry_full_geometry.fem, in the File name: field. The.femfile name extension is the suggested extension for RADIOSS input decks. 4. Click Save. Note the name and location of the axi-symmetry_full_geometry.femfile 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 Radioss. This launches the RADIOSS job. A command window opens up and indicates the start of the RADIOSS run. If the job is successful, new results files can be seen in the directory where the RADIOSS model file was written. The axi-symmetry_full_geometry.outfile is a good place to look for error messages that will help to debug the input deck if any errors are present.

3 Viewing the Results Once you see the message Process completed successfully in the command window, click on the HyperView button in the Radioss panel of HyperMesh. The HyperView Graphic User Interface (GUI) window opens and the results automatically get loaded into HyperView. A message window appears to inform about the successful loading of the model and result files in to HyperView. Close the message window. Displacement and stress results are output for each subcase to the axisymmetry_full_geometry.h3dfile from RADIOSS. This section describes how to view those results in HyperView. Step 3: View the displacements of the structure It is helpful to view the deformations of the model first, to determine if the boundary conditions have been defined correctly and also to see if the model is deforming as expected. 1. Set the Animation mode to Linear. 2. Click the Contour icon on the toolbar. 3. Select the first pull- down menu below Result Type and select Displacement [v]. 4. Select the second pull- down menu below Result Type and select Mag. 5. Click Apply to display the displacement contour. To view the displacement variation across the thickness, we will mask one half of the structure. 6. Expand the Components folder in the Results Browser. 7. Click the elements icon in front of the component bottom_half to mask the component from display. 8. Click XZ Left Plane View to display the Left view. 9. The following figure shows the displacements through the thickness.

4 Exercise 2: Analysis with a Small Portion of the Full Model with Axi-symmetry Boundary Conditions Setting up the New Analysis Return to HyperMesh to delete the all the elements, except for a small portion and to set up the axi- symmetry boundary conditions. Before proceeding to the next section, let s look at the criteria for modeling an axi- symmetry problem. Note that even if the geometry is symmetrical about an axis, if any of the loads or boundary conditions are not symmetrical about the same axis, then it cannot be modeled as an axisymmetry model. Therefore, the models shown below are examples that cannot be modeled as axisymmetry models. Non axi-symmetric loads Non axi-symmetric boundary conditions Step 1: Setup the axi-symmetry model

5 1. Click to enter the Delete panel, or click F2. 2. Make sure the entity selection switch is set to elems. 3. Click on the yellow button elems to open the extended entity selection window and select by sets. 4. Click in the check box in front of SetA. A check mark appears before SetA to indicate that it is selected. 5. Click select. The selected elements are highlighted. 6. Click delete entity to delete the selected elements. 7. Click return to exit the Delete panel. We will use the retained portion to model the axi- symmetric model with suitable boundary conditions. Step 2: Apply the additional boundary conditions to model axi-symmetry conditions The axi- symmetry conditions are applied by constraining all of the nodes from moving in the tangential direction. This is done by first assigning all of the nodes to a cylindrical coordinate system and then constraining all of them in tangential 1. From the Analysis page, enter the systems panel. 2. Select the assign radio button. degrees of freedom. 3. Make sure the entity selection switch in front of set: is set to nodes. 4. Click on the yellow button nodes to open the extended entity selection window and select all. 5. Click on the yellow button system to activate it and select the red colored system from the graphic window. 6. Click set displacement. You will see the message on the footer bar The analysis system has been assigned. 7. Click return. All of the nodes in the model are assigned to a cylindrical coordinate system. Note that the z-axis of the cylindrical coordinate system coincides with the axis about which the model is symmetrical. Now, constraining the nodes that are assigned to the cylindrical coordinate system in tangential degrees of freedom will enforce the axi- symmetry boundary condition. Step 3: Create constraints 1. Expand the Load Collectors folder in the Model Browser. 2. Right-click on SPCs and click Make Current to make SPCs the current component, if not already done. 3. Click BCs > Create > Constraints to open the Constraints panel. 4. Make sure the entity selection switch is set to nodes. 5. Click on the yellow button nodes to open the extended entity selection window and select all. 6. Constrain dof2. Dofs with a check will be constrained, while dofs without a check will be free. Dofs 1, 2, and 3 are radial, tangential and translation degrees of freedom. Dofs 4, 5, and 6 are radial, tangential and translation rotational degrees of freedom. 7. Click create.

6 This applies these constraints to the selected nodes. 8. Click return to return to the main menu. Submitting the Job 1. From the Analysis page, enter the Radioss panel. 2. Solve the job with file name as axi-symmetry_model.femby following the same steps as explained in the earlier section. If the job is successful, new results files can be seen in the directory where the RADIOSS model file was written. The axi-symmetry_model.outfile is a good place to look for error messages that will help to debug the input deck if any errors are present. Viewing the Results Displacement and Stress results are output for each subcase to axi-symmetry_model.h3dfile from RADIOSS. Results from the axi- symmetry model should match with the results of the full model. We will use load the result file in the previously opened HyperView session to compare the results. 1. Click on HyperView to view the results. 2. Click the Page Layout button. 3. Select the two window layout. 4. Activate the new window by clicking in the graphic area of the new window. 5. Click to open the Load model and results panel. 6. Click the Load model button on the toolbar and load the axi-symmetry_model.h3d. This loads the complete path of the selected.h3dfile in the field. Also note that the same file path is loaded next to the field Load results. 7. Click Apply. 8. Click XZ Left Plane View to display the Left view. 9. Click the Contour icon on the toolbar and contour the displacements. 10. Compare the displacement results of the axi- symmetry model with the result from the full model. The results should match, as shown in the below picture. Similarly, stress and other results will also match. C omparison of displacement results

7 Go To RADIOSS Tutorials