hyperworks模态分析实例教程

Normal Modes Analysis of a Splash Shield - RD-1020

In this tutorial, an existing finite element model of an automotive splash shield will be used to demonstrate how to set up and perform a normal modes analysis. HyperMesh post-processing tools are used to determine mode shapes of the model.

The following exercises are included:

•Retrieving the RADIOSS input file

•Setting up the model in HyperMesh

•Applying Loads and Boundary Conditions to the Model

•Submitting the job

•Viewing the results

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: Import a Finite Element Model File in HyperMesh

1.From the File pull-down menu on the toolbar, select Import….

An Import… tab is added to your tab menu.

2.Click to import an FE model.

3.For the File type:, select RADIOSS (Bulk Data).

4.Select the Files icon button.

A Select RADIOSS (Bulk Data) file browser will pop up.

5.Browse for sshield.fem file located in the HyperWorks installation directory under

/tutorials/hwsolvers/radioss/ and select the file.

6.Click Open►Import.

7.Click Close to close the Import tab menu.

Step 3: Review Rigid Elements

Notice there are two rigid "spiders" in the model. They are placed at locations where the shield is bolted down. This is a simplified representation of the interaction between the bolts and the shield. It is assumed that the bolts are significantly more rigid in comparison to the shield.

The dependent nodes of the rigid elements have all six degrees of freedom constrained. Therefore, each "spider" connects nodes of the shell mesh together in such a way that they do not move with respect to one another.

The following steps show how to review the properties of the rigid elements.

1.From the 1D page, select the rigids.

2.Click review.

3.Select one of the rigid elements in the graphics region.

In the graphics window, HyperMesh displays the IDs of the rigid element and the two end nodes and indicates the independent node with an 'I' and the dependent node with a 'D'. HyperMesh also indicates the constrained degrees of freedom for the selected element, through the dof checkboxes in the rigids panel. All rigid elements in this model should have all dofs constrained.

4.Click return to go to the main menu.

Step 4: Setting up the Material and Geometric Properties

The imported model has three component collectors with no materials. A material collector needs to be created and assigned to the shell component collectors. The rigid elements do not need to be assigned a material. Shell thickness values also need to be corrected.

1.Select the Material Collectors toolbar button .

2.Select the create subpanel 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 card image = and select MAT1 from the pop-up menu.

6.Click create/edit.

The MAT1 card image pops up.

7.For E, enter the value 2.0E5.

8.For NU, enter the value 0.3.

9.For RHO, enter the value 7.85E-9.

If a quantity in brackets does not have a value below it, it is off. To change this, click the quantity in brackets and an entry field will appear below it. Click in the entry field, and a value can be entered.

10.Click return.

A new material, steel, has now been created. The material uses RADIOSS linear isotropic material

model, MAT1. This material has a Young's Modulus of 2E+05, a Poisson's Ratio of 0.3 and a material density of 7.85E-09. A material density is required for the normal modes solution sequence.

At any time the card image for this collector can be modified using Card Editor.

11.Click return to exit the Material Create panel.

12.Select the Card Editor toolbar button .

13.Click the down arrow on the right of the entity shown in the yellow box, select props from the extended

entity list.

14.Click the yellow props button and then check the box next to design and nondesign.

15.Click select.

16.Make sure card image=is set to PSHELL.

17.Click edit.

The PSHELL card image for the design component collector pops up.

18.Replace 0.300 in the T field with 0.25.

19.Click return to save the changes to the card image.

20.Click return to go to the main menu.