abaqus 典型实例w-6a-hinge-mesh.doc

W6a.9Goals Use the model manager to create a copy of the model Partition the hinge to obtain hex-meshable domains Assign an element type Create mesh seeds Create a mesh using hexahedral elements Create a tetrahedral element mesh using the free meshing techniqueIntroductionThe Mesh module allows you to generate finite element meshes on assemblies. The process of meshing the model, like creating parts and assemblies, is feature based; therefore, you can modify the parameters that define a part or an assembly, and the mesh attributes that you specified within the Mesh module are regenerated automatically.In this workshop you will mesh the part instances that you defined earlier. Creating a finite element mesh usually involves: Partitioning the assembly to ensure that the assembly can be meshed Assigning mesh attributes to the part instances Seeding the part instances Meshing the assemblyNote: The replay file, CAE/Workshops/Hinge-StepIntBc.py, can be used to generate the prerequisite model definitions for this workshop. In the event that you were unable to complete the previous workshop successfully, you accidentally deleted your model database file, etc., do the following: copy the file into a local directory, start ABAQUS/CAE, and run the script by selecting FileRun Script. Then proceed with the rest of the workshop.Creating a copy of the modelTwo different types of meshes will be created in this workshop, each using a different copy of the model. To create a copy of the model:1. Start ABAQUS/CAE, and open the database created in Workshop 5a.2. In the Module list located under the tool bar, select Mesh to enter the Mesh module.3. Select ModelManager. Select Copy Model, and name the model Model-2. Notice that after the copy is created, the name of the model in the pull down menu under the toolbar changes to Model-2.4. Click Dismiss on the Model manager.5. Using the model list under the toolbar, change the model to Model-1.Model-1 will be meshed with hexahedral elements, while Model-2 will be meshed with tetrahedral elements.Creating a hexahedral element meshPartitioningMost three-dimensional domains can be readily meshed with tetrahedral elements using a technique called “free meshing.” Unfortunately, tetrahedral elements are usually less desirable than hexahedral elements in a finite element analysis. Hexahedral elements are generally preferred because they provide a higher accuracy to cost ratio. To create a mesh using hexahedral elements, simple domains are generally required. Thus, to reduce a complex three-dimensional region to simple subdomains, we need to partition. Partitions created in the Mesh module are features used only by the meshing program; these partitions do not alter the geometry or play any role in the physical problem being modeled.Ensure that the current model is Model-1 and that the view rendering is set to Shaded. ABAQUS/CAE color codes regions of the model as follows: Green indicates that a region can be meshed using the structured meshing technique. Yellow indicates that a region can be meshed using the swept meshing technique. Orange indicates that a region cannot be meshed using the default element shape assignment (hexahedral) and must be partitioned further. Figure W6a1. The model before being partitionedThe hinge components are colored orange (Figure W6a1) and need to be partitioned before being meshed with hexahedral elements. ABAQUS/CAE also displays the pin in orange because it is an analytical rigid surface and cannot be meshed. In addition, the areas surrounding the hole in the flange and the lubrication hole must be partitioned. Use the following techniques to help you select faces and vertices during the partitioning process: Use a combination of the view manipulation tools, the display option tools in the toolbar, and the tools in the Views toolbox to resize and reposition the model as necessary. Use the magnification tool and the rotation tool to position the model as required. When necessary, click the Iso tool in the Views toolbox to return the model to its original size and position in the viewport. Select ViewAssembly Display Options to suppress the visibility of part instances and boundary condition or load symbols as necessary.Create partitions as follows:1. From the main menu bar, select ToolsPartition. ABAQUS/CAE displays the Create Partition dialog box.2. From the Create Partition dialog box, choose the Cell partition type. Select the Extend face method, and click Apply.3. Select the solid hinge piece as the cell to partition.4. Select the face to extend, as shown by the gridded face in Figure W6a2.Figure W6a2. Selection of the first partitioning plane5. From the prompt area, click Create Partition. ABAQUS/CAE creates the partition, as shown in Figure W6a3. If the partition is not located correctly, select FeatureDelete from the main menu bar and select the partition to delete.Figure 6a3. Partitioning of the solid hinge pieceNotice that ABAQUS/CAE colors the cube portion of the solid hinge piece green to indicate that it can be meshed using the structured meshing technique; it colors the flange of the solid hinge piece yellow to indicate that it can be meshed using a swept mesh.6. Using a similar method, create a partition between the cube and the flange of the other hinge piece.Here the cube turns green to indicate that it can be meshed using structured meshing, but the flange remains orange, indicating that additional partitioning is required to mesh the flange. The flange will be partitioned, as shown in Figure W6a4, by following the steps outlined below.Figure W6a4. View of the partitioned flangeYou may find it useful to display only the part instance of interest (Hinge-Hole in this case). From the main menu bar, select ViewAssembly Display Options to control the display. To partition the areas surrounding the holes in the flange:7. From the Create Partition dialog box, select the Define cutting plane method and click Apply.8. Select the flange of the hinge piece with the lubrication hole. Notice that ABAQUS/CAE provides three methods for specifying the cutting plane. The cutting plane need not be defined in the cell being partitioned. The plane extends infinitely in all directions and partitions the selected cell anywhere there is an intersection between the plane and the cell. From the buttons in the prompt area, select 3 Points. ABAQUS/CAE highlights points that you can select.9. Select three points that cut the flange in half, as shown in Figure W6a5.Figure W6a5. Three points to partition the flange10. From the prompt area, click Create Partition. ABAQUS/CAE creates the desired partition. You have now partitioned the flange into two regions; you need to create a partition that cuts the curved region in half, as shown in Figure W6a6.Figure 6a6. Further divisions of the flange11. Use the Define cutting plane method to create the desired partition.12. ABAQUS/CAE colors the region containing the lubrication hole orange to indicate that it still cannot be meshed. Use the Define cutting plane method to partition the cell containing the lubrication hole into four regions, as shown in Figure W6a7.Figure W6a7. Partitioning the region with the lubrication hole13. ABAQUS/CAE colors the rest of the flange orange again to indicate that this region cannot be meshed with the partitions that you have added. You will need to partition the model once more.14. From the Create Partition dialog box, select the Extend face method and click Apply. Select the base of the flange (the orange portion). Select the partition that intersects the lubrication hole as the face to extend as the partitioning tool, as shown in Figure W6a8 (use the selection filters to cycle through the list of possible faces). From the prompt area, click Create Partition. ABAQUS/CAE creates the desired partition, as shown in Figure W6a9.Figure W6a8. Select the face to extendFigure W6a9. Final view of the partitioned model15. The coloring of the model indicates that it can now be meshed completely with hexahedral elements.16. Turn on the other part instances so that the complete assembly is displayed. Click Cancel to close the Create Partition dialog box.Assigning mesh controlsIn this section you will use the Mesh Controls dialog box to examine the techniques that ABAQUS/CAE will use to mesh the model and the shape of the elements that ABAQUS/CAE will generate.1. From the main menu bar, select MeshControls.2. You need to select the two hinge pieces, which have now been partitioned into several regions. Use the following technique to select the two hinge pieces without selecting the pin. The pin is an analytical rigid surface and cannot be meshed:a. Drag a square around the model to select the entire model. b. Ctrl+Click the pin to deselect it.c. Click Done to indicate that you have finished selecting the regions to mesh.The two hinge pieces appear red in the viewport to indicate that you have selected them, and ABAQUS/CAE displays the Mesh Controls dialog box.3. In the dialog box, accept Hex as the default Element Shape selection.4. Accept As is as the meshing technique that ABAQUS/CAE will use. (ABAQUS/CAE will use structured meshing for green regions and swept meshing for yellow regions.)5. Click OK to assign the mesh controls and to close the dialog box.Selecting the ABAQUS element typeTo assign an ABAQUS element type:1. From the main menu bar, select MeshElement Type.2. Select the two hinge pieces using the same technique described earlier. ABAQUS/CAE displays the Element Type dialog box.3. In the dialog box, accept Standard as the Element Library selection.4. Accept Linear as the Geometric Order selection.5. Accept 3D Stress as the default Family of elements.6. In the Hex folder, select Reduced integration as the Element Controls method if it is not already selected. A description of the default element type, C3D8R, appears at the bottom of the dialog box. ABAQUS/CAE will now associate C3D8R elements with the elements in the mesh.7. Click OK to assign the element type and to close the dialog box.Seeding the part instancesThe next step of the meshing process is to seed each of the part instances. Seeds represent the approximate locations of nodes and indicate the target density of the mesh you would like to generate. You can select seeding based on the number of elements to generate along an edge or the average element size, or you can bias seed distribution toward one end of an edge. For this workshop seed the entire assembly so that the hinge pieces have an average element size of 0.004. To seed the part instances:1. From the main menu bar, select SeedInstance.2. Select one hinge piece, and Shift+Click the second hinge piece to append it to your selection. When both hinge pieces are highlighted, click mouse button 2 to indicate that your selection is complete.3. In the text box in the prompt area, enter an approximate part element size of 0.004 and press Enter.4. Seeds appear on all the edges.5. Click Done to exit the seeding utility. Meshing the assemblyYou are now ready to mesh the assembly.1. From the main menu bar, select MeshInstance. ABAQUS/CAE prompts you to select the part instances to mesh.2. Select one hinge piece, and Shift+Click the second hinge piece to append it to your selection. When both hinge pieces are highlighted, click mouse button 2 to indicate that your selection is complete.3. The cursor changes to an hourglass while ABAQUS/CAE meshes the assembly. 4. Click Done after the meshing operation is comple