R212ABAQUS资料IABSW03QNonlinearStaticsWord文档格式.docx

1、IntroductionIn this workshop you will model the plate shown in Figure W31. It is skewed at 30 to the global X-axis, built-in at one end, and constrained to move on rails parallel to the plate axis at the other end. You will determine the midspan deflection when the plate carries a uniform pressure.

2、You will modify the model to include alternate nodal and material directions as well as nonlinear effects. FigureW31. Sketch of skewed platePreliminaries1.Enter the working directory for this workshop./abaqus_solvers/interactive/skew 2.Run the script ws_solver_skew_plate.py using the following comma

3、nd:abaqus cae startup=ws_solver_skew_plate.py.The above command creates an Abaqus/CAE database named SkewPlate.cae in the current directory. A model named linear includes the geometry, mesh and material definitions for the plate. You will first add the necessary data to complete the linear analysis

4、model. You will later perform the simulation considering both geometrically and material nonlinear effects. In a subsequent workshop a restart analysis will be performed to study the unloading of the plate.Defining the local material directionsThe orientation of the structure in the global coordinat

5、e system is shown in Figure W31. The global Cartesian coordinate system defines the default material directions, but the plate is skewed relative to this system. It will not be easy to interpret the results of the simulation if you use the default material directions because the direct stress in the

6、 material 1-direction （i.e., global X-direction）, 11, will contain contributions from both the axial stress, produced by the bending of the plate, and the stress transverse to the axis of the plate. It will be easier to interpret the results if the material directions are aligned with the axis of th

7、e plate and the transverse direction. Therefore, a local rectangular coordinate system is needed in which the local x-direction lies along the axis of the plate （i.e., at 30 to the global X-axis） and the local y-direction is also in the plane of the plate.You will define the datum coordinate system

8、（CSYS） and then assign the material orientation.1.Switch to the Property module and define a rectangular datum coordinate system as shown in Figure W32 using the Create Datum CSYS: 2 Lines tool .a.Note the small black triangles at the base of the toolbox icons. These triangles indicate the presence

9、of hidden icons that can be revealed. Click the Create Datum CSYS: 3 Points tool but do not release the mouse button. When additional icons appear, release the mouse button. b.Select the Create Datum CSYS:. It appears in the toolbox with a white background indicating that you selected it.c.In the Cr

10、eate Datum CSYS dialog box, name the datum CSYS Skew, select the Rectangular coordinate system type, and click Continue. Make the next two selections as indicated in Figure W32.W32. Datum coordinate system used to define local directions2.Assign the material orientations to the plate.a.In the toolbo

11、x, click the Assign Material Orientation tool . b.Select the entire part as the region to be assigned a local material orientation. c.Click mouse button 2 in the viewport or click Done in the prompt area to confirm the selection.d.Click Datum CSYS List in the prompt area.e.In the Datum CSYS List dia

12、log box, select skew and click OK. In the material orientation editor, select Axis 3 for the direction of the approximate shell normal. No additional rotation is needed about this axis.f.Click OK to confirm the input.Tip: To verify that the local material directions have been assigned correctly, sel

13、ect ToolsQuery from the main menu bar and perform a property query on the material orientations.Once the part has been meshed and elements have been created in the model, all element variables will be defined in this local coordinate system.Prescribing boundary conditions and applied loads As shown

14、in Figure W31, the left end of the plate is completely fixed; the right end is constrained to move on rails that are parallel to the axis of the plate. Since the latter boundary condition direction does not coincide with the global axes, you must define a local coordinate system that has an axis ali

15、gned with the plate. You can use the datum coordinate system that you created earlier to define the local directions. 1.In the Model Tree, double-click the BCs container and define a Displacement/Rotation mechanical boundary condition named Rail boundary condition in the Apply Pressure step. In this

16、 example you will assign boundary conditions to sets rather than to regions selected directly in the viewport. Thus, when prompted for the regions to which the boundary condition will be applied, click Sets in the prompt area of the viewport.2.From the Region Selection dialog box that appears, selec

17、t the set Plate-1.EndB. Toggle on Highlight selections in viewport to make sure the correct set is selected. The right edge of the plate should be highlighted. Click Continue.3.In the Edit Boundary Condition dialog box, click to specify the local coordinate system in which the boundary condition wil

18、l be applied. In the viewport, select the datum CSYS Plate-1.Skew. The local x-direction is aligned with the plate axis. Note that Plate-1.Skew is the assembly-level datum CSYS generated by the part-level datum CSYS Skew.4.In the Edit Boundary Condition dialog box, fix all degrees of freedom except

19、for U1 by toggling them on and entering a value of 0 for each.The right edge of the plate is now constrained to move only in the direction of the plate axis. Once the plate has been meshed and nodes have been generated in the model, all printed nodal output quantities associated with this region （di

20、splacements, velocities, reaction forces, etc.） will be written in this local coordinate system.5.Create another boundary condition named Fix left end to fix all degrees of freedom at the left edge of the plate （set Plate-1.EndA）. Use the default global directions for this boundary condition.6.Defin

21、e a uniform pressure load named Pressure across the top of the shell in the Apply Pressure step. Select both regions of the part using Shift+Click, and choose the top side of the shell （Brown） as the surface to which the pressure load will be applied. You may need to rotate the view to more clearly

22、distinguish the top side of the plate. Specify a load magnitude of 2.0E4 Pa.Running the job and postprocessing the results 1.Create a job named SkewPlate with the following description: Linear Elastic Skew Plate, 20 kPa Load.2.Save your model database file.3.Submit the job for analysis and monitor t

23、he solution progress. When the analysis is complete, use the following procedure to postprocess the analysis results.4.In the Model Tree, click mouse button 3 on the job SkewPlate and select Results from the menu that appears to open the file SkewPlate.odb in the Visualization module.5.Click the Plo

24、t Deformed Shape tool to plot the deformed shape.6.Use the the Query information tool to probe the value of the midspan deformation. a.In the Query dialog box, select Probe values in the Visualization Module Queries field. b.Change the displayed field variable to the displacement along the 3-directi

25、on. In the Probe Values dialog box, click to change the default field output variable to U3. In the Field Output dialog box that appears, select U as the output variable and U3 as the component and click OK. c.In the Probe Values dialog box, select Nodes as the item to probe. d.Click on a node （as i

26、ndicated in Figure W33） along the midespan to probe its displacement along the 3-direction. Enter this value in the “Linear” column of Table W31. Figure W33. Midspan nodeAdding geometric nonlinearityNow perform the simulation considering geometrically nonlinear effects. Copy the model named linear t

27、o a new model named nonlinear. You will add geometric nonlinearity into the model nonlinear; the changes required for this model are described next.7.In the Model Tree, expand the Steps container and double-click Apply Pressure to edit the step definition. a.In the Basic tabbed page of the Edit Step

28、 dialog box, toggle on Nlgeom to include geometric nonlinearity effects and set the time period for the step to 1.0.b.In the Incrementation tabbed page, set the initial increment size to 0.1. Note that the default maximum number of increments is 100; Abaqus may use fewer increments than this upper l

29、imit, but it will stop the analysis if it needs more.You may wish to change the description of the step to reflect that it is now a nonlinear analysis step.8.Create a job named NlSkewPlate for the model nonlinear and give it the description Nonlinear Elastic Skew Plate. Save your model database file

30、.9.Submit the job for analysis and monitor the solution progress.The Job Monitor is particularly useful in nonlinear analyses. It gives a brief summary of the automatic time incrementation used in the analysis for each increment. The information is written as soon as the increment is completed, so you can monitor the analysis as it is running. This facility is useful in large, complex problems. The information given in the Job Monitor is the same as that given in the status file （NlSkewPlate.sta）.10.When the job is c