2-材料属性.doc

W5.4IntroductionIn this workshop you will use the ABAQUS/CAE Property module to define the material and section properties of the components in the pump assembly. The gasket will be defined using gasket material properties. All other components (pump housing, cover, and bolts) are assumed to possess the properties of steel.ABAQUS Defining a linear elastic material and solid section propertiesFollow the steps outlined below to complete the steel property and section assignments for the pump components. Note that the units used in this model are in, lb, and psi.1. Start a new session of ABAQUS/CAE from the directory containing the pump assembly model.2. From the main menu bar, select FileOpen to open the model database file PumpAssy.cae.3. Switch to the Property module.4. From the Model list located under the toolbar, select pump_ribs to access the pump_ribs model.5. From the main menu bar, select MaterialCreate to create a linear elastic material named Steel. Specify a Youngs modulus of 30.E6 psi and a Poissons ratio of 0.3.6. From the main menu bar, select SectionCreate to create a homogeneous solid section named steelSection that refers to the material named Steel.7. From the main menu bar, select AssignSection to assign the section named steelSection to the parts named cover, n_bolts, and PUMP-1.Tip: You will need to make the section assignments individually; select the different parts by choosing them from the Part pull-down list.Defining the gasket material and section propertiesThe typical specification of gasket material properties in ABAQUS involves a tabular representation of the pressure versus closure relationship in the thickness direction of the gasket. The pressure versus closure models available in ABAQUS allow the modeling of very complex gasket behaviors, including nonlinear elasticity, permanent plastic deformation, and loading/unloading along different paths. These behaviors are usually calibrated from test data. A detailed discussion of gasket material behavior, however, is beyond the scope of this course. For your convenience (and to make the analysis realistic) the gasket properties are defined in a script that you will read directly into ABAQUS/CAE.1. From the main menu bar, select FileRun Script. The Run Script dialog box appears. 2. Select the file named gasket_material.py. Click OK in the dialog box.3. From the main menu bar, select MaterialManager to open the Material Manager.Notice that the material named Gasket has been added to the model database. 4. Select Gasket, and click Edit.5. Review the gasket material properties. Note the gasket has membrane elasticity of 12155 psi, shear stiffness of 6435 psi, and a coefficient of thermal expansion of 1.67 E-5 /F. 6. Select Gasket Thickness Behavior from the list of available Material Options in the dialog box, and notice the tabular specification of the loading and unloading curves for the gasket (see Figure W51). Figure W51. Edit Material dialog boxYou can use the plotting capabilities within ABAQUS/CAE to plot the loading and unloading curves. This may help you obtain a better understanding of the material behavior. 7. Open the Loading tabbed page. Right-click your mouse over the column headings of the table, and select Create XY Data from the list of options that appears. Name the curve loading when prompted for a name in the Create XY Data dialog box. Repeat the same operation for the unloading curve to create a curve named unloading.8. Switch to the Visualization module.9. From the main menu bar, select ToolsXY DataManager. The XY Data Manager appears. 10. Select both the curves (using the shift key), and click Plot. You should see a similar plot in the viewport as that shown in Figure W52.Figure W52. Loading and unloading gasket behavior11. Click Dismiss in the XY Data Manager, and switch back to the Property module to continue with the gasket section property specification.12. From the main menu bar, select SectionCreate to create a gasket section.13. In the Create Section dialog box, select Other as the category and Gasket as the type. Name the section gasketSection (see Figure W53) and click Continue. Figure W53. Create Section and Edit Section dialog boxes14. In the Edit Section dialo