基于hyperworks的结构静力学分析实例教程

Linear Static Analysis of a Plate with a Hole - RD-1000
This tutorial demonstrates how to create finite elements on a given CAD geometry of a plate with a hole, apply boundary conditions, and perform a finite element analysis of the problem. Post-processing tools will be used in HyperView to determine deformation and stress characteristics of the loaded plate.
The following exercises are included:
•Setting up the problem in HyperMesh
•Applying Loads and Boundary Conditions
•Submitting the job
•Viewing the results
Exercise
Step 1: Launch HyperMesh and set the RADIOSS (Bulk Data) User Profile
unch HyperMesh.
A User Profiles… Graphic User Interface (GUI) will appear. If it does not appear, go to Preferences>
User Profiles … from the menu on the top.
2.Select RADIOSS in the User Profile dialog.
3.From the extended list, select Bulk Data.
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 plate_hole.hm
1.Click the Open .hm file icon .
An Open file… browser window pops up.
2.Select the plate_hole.hm file, located in the HyperWorks installation directory under
<install_directory>/tutorials/hwsolvers/radioss/.
3.Click Open.
The plate_hole.hm database is loaded into the current HyperMesh session, replacing any existing data. The database only contains geometric data.
Setting Up the Problem in HyperMesh
When building models, we encourage you to create the material and property collectors before creating the component collectors. This is the most efficient way of setting up the file since components need to reference materials and properties.
Step 3: Create the material
1.Click the Material Collector Panel toolbar button .
2.Make sure the create subpanel is selected using the radio buttons on the left-hand side of the panel.
3.Click mat name = and enter steel.
4.Select the desired color for the material steel by clicking on .
5.Click type = and select ISOTROPIC.
6.Click card image = and select MAT1.
7.Click create/edit.
The MAT1 card image pops up.
If a material property in brackets does not have a value below it, it is off. To edit these material
properties, click the property in brackets you wish to edit and an entry field will appear below it. Click the entry field and enter a value.
8.Enter the following values for E, NU and RHO; E as 2e5; NU as 0.3 and RHO as 7.9e-09.
9.Click return twice.
A new material, steel, has been created. The material uses RADIOSS's linear isotropic material model,
MAT1. This material has a Young's Modulus of 2E+05 and a Poisson's Ratio of 0.3. It is not necessary to define a density value since only a static analysis will be performed. Density values are required,
however, for other solution sequences.
At any time, the card image for this collector can be modified using the Card Editor .
Step 4: Create the properties and update the Component Collector
1.Click Properties toolbar icon .
2.Make sure the create subpanel is selected using the radio buttons on the left-hand side of the panel.
3.Click prop name = and enter plate_hole.
4.Select the desired color for the property plate_hole by clicking on .
5.Click type = and select 2D.
6.Click card image = and select PSHELL.
7.Click material = and select steel.
8.Click create/edit.
The PSHELL card image pops up.
9.Click [T] and enter 10.0 as the thickness of the plate.
10.Click return twice and go back to the main menu.
The property of the shell structure has been created as 2D PSHELL. Material information is also linked to this property.
11.Click the Component Collector Panel toolbar button .
12.Make sure the update subpanel is selected using the radio buttons on the left-hand side of the panel.
13.Click comps >> and select plate_hole from the list.
14.Toggle <no property> to property =.
15.Click property = twice and select the plate_hole property from the list.
Property card image and material information are listed below the property entry field.
16.Click update.
17.Click return to go to the main menu.
The component plate_hole has been updated with a property of the same name and is currently the
“Current Component” (see the box in the lower right for plate_hole ). This component uses the
plate_hole property definition with a thickness value of 10.0. The material steel is referenced by this component.
At any time, the card image for this collector can be modified using the Card Editor and the material referenced by this component collector can be changed using the update option in the Collectors panel.
Apply loads and boundary conditions to the model
In the following steps, the model is constrained so that two opposing edges of the four external edges cannot move. The other two edges remain unconstrained. A total load of 1000N is applied at the edge of the hole in the positive z-direction.
Step 5: Create load collectors (spcs and forces )
A new load collector, spcs is created.
A new load collector, forces is created.
Step 6: Create constraints
1.Click the Load Collectors toolbar icon .
2.Make sure the create subpanel is selected using the radio buttons on the left-hand side of the panel.
3.Click loadcol name = and enter spcs .
4.Click color and select a color from the color palette.
5.Click the creation method switch and select no card image from the pop-up menu.
6.Click create .
7.Click loadcol name = and enter forces .
8.Click color and select a different color from the color palette.
9.Click create .
10.Click return to go to the main menu.1.From Model Browser expand LoadCollectors , right-click on spcs and click Make current to set spcs
as the current load collector.
The window is polygonal, and every mouse click creates a window vertex.
Illustration of which nodes to select for applying single point constraints. Dofs with a check will be constrained while dofs without a check will be free.
Dofs 1, 2, and 3 are x, y, and z translation degrees of freedom.
Dofs 4, 5, and 6 are x, y, and z rotational degrees of freedom.
This applies these constraints to the selected nodes.
Step 7: Create forces on the nodes around the hole
The window is polygonal, and every mouse click creates a window vertex.
2.From the Analysis page,enter the constraints panel.
3.Make sure the create subpanel is selected using the radio buttons on the left-hand side of the panel.
4.Make sure nodes are selected from the entity selection switch.
5.Click nodes and select by window from the pop-up extended entity selection menu.
6.
Draw a window in the graphics area encompassing the nodes to be selected (shown in the figure).7.Check the box beside interior and click on select entities .
8.Constrain dof1, dof2, dof3, dof4, dof5, and dof6 and set all of them to a value of 0.0.
9.Ensure the load types is set to SPC .
10.Click create .
11.Click return to go to the main menu.
1.Set your current load collector to forces in Model Browser as shown before in point 1 under Step 6.
2.From the Analysis page, enter the forces panel.
3.Make sure the create subpanel is selected using the radio buttons on the left-hand side of the panel.
4.Make sure nodes are selected from the entity selection switch.
5.Click nodes and select by window from the pop-up extended entity selection menu.
6.Draw a window in the graphics window encompassing the nodes shown in the figure below.
Nodes selected for creating loading around hole.
7.Check the box beside interior and click on select entities.
8.Set the coordinate system toggle to global system.
9.Click the vector definition switch and select constant vector.
10.Click magnitude = and enter 21.277 (i.e. 1000 divided by the number of nodes 47).
11.Click the direction definition switch below magnitude=, and select z-axis from the pop-up menu.
12.Ensure the load types is set to FORCE.
13.Click create.
This creates a number of point forces, with the given magnitude in the z-direction, to be applied to the nodes about the hole.
14.Click return to go to the main menu.
Step 8: Create a RADIOSS subcase (also referred to as a loadstep)
1.From the Analysis page, enter the loadsteps panel.
2.Click name = and enter lateral force.
3.Click the type: switch and select linear static, if it is not already selected by default.
4.Check the box preceding SPC.
An entry field appears to the right of SPC.
5.Click on the entry field and select spcs from the list of load collectors.
6.Check the box preceding LOAD.
An entry field appears to the right of LOAD.
7.Click on the entry field and select forces from the list of load collectors.
8.Click create.
A RADIOSS subcase has been created which references the constraints in the load collector spcs and
the forces in the load collector forces.
9.Click return to go to the main menu.
Step 9: Submitting the job
1.From the Analysis page, enter the RADIOSS 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 RADIOSS model file and enter the name for the
model, plate_hole.fem, in the File name: field.
The .fem filename extension is the recommended extension for RADIOSS Bulk Data Format input decks.
4.Click Save.
Note the name and location of the plate_hole.fem file displays in the input file: field.
5.Set the export options:toggle to all.
6.Click the run options: switch and select analysis.
7.Set the memory options: toggle to memory default.
8.Click Radioss.
This launches the RADIOSS job. If the job is successful, you should see new results files in the directory from which plate_hole.fem was selected. The plate_hole.out file is a good place to look for error messages that could help debug the input deck if any errors are present.
The default files written to the directory are:
plate_hole.html HTML report of the analysis, giving a summary of the problem
formulation and the analysis results.
plate_hole.out RADIOSS 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
optimization iteration, and compute time information. Review this file
for warnings and errors.
plate_hole.h3d HyperView binary results file.
plate_hole.res HyperMesh binary results file.
plate_hole.stat Summary of analysis process, providing CPU information for each
step during analysis process.
Viewing the Results
Displacement and Stress results for linear static analyses are output from RADIOSS by default. The following steps describe how to view those results in HyperView.
HyperView is a complete post-processing and visualization environment for finite element analysis (FEA), multi-body system simulation, video and engineering data.
Step 10: View a contour plot of stresses
1.Once you receive the message 'Process Completed Successfully' in the command window, click
HyperView.
HyperView is launched and the results are loaded. A message window appears to inform of the
successful model and result files loading into HyperView.
2.Click Close to close the message window.
3.Click the Contour toolbar button .
4.Select the first pull-down menu below Result type:and select Element Stresses [2D & 3D] (t).
5.Select the second pull-down menu below Result type:and select vonMises.
6.Select None in the field below Averaging method:.
7.Click Apply.
A contoured image representing von Mises stresses should be visible. Each element in the model is
assigned a legend color, indicating the von Mises stress value for that element, resulting from the applied loads and boundary conditions.
8.Click Top in the view controls from the bottom right corner to view the model, as shown in the following
figure.
von Mises stress assigned plot
What is the maximum von Mises stress value?
At what location does the model have its maximum stress?
Does this make sense based on the boundary conditions applied to the model?
Step 11: View a contour plot of displacements
1.Select the first pull-down menu below Result type:and select Displacement (v).
2.Select the second pull-down menu below Result type:and select Mag.
3.Click Apply.
The resulting contours represent the displacement field resulting from the applied loads and boundary conditions.
What is the maximum Displacement value?
At what location does the model have its maximum displacement?
Does this make sense based on the boundary conditions applied to the model?
Step 12: View the deformed shape
1.Click Iso in the view controls (bottom right corner) to display the isometric view of the model.
2.Click the Deformed toolbar button .
3.Set Result type: to Displacement(v), Scale:to Scale factor; and Type:to Uniform.
4.In the field next to value, enter 500.
This means that the displacement results of the analysis will be multiplied by 500.
5.For Show:, select Wireframe.
6.Click Apply.
A deformed plot of your model with displacement contour should be visible, overlaid on the original
undeformed mesh. Refer to the following figure to see what the plot should look like in isometric view.
Isometric view of deformed plot overlaid on the original undeformed mesh with model units set to 500.
Go To
RADIOSS, MotionSolve, and OptiStruct Tutorials。