Workshop8 creep-mesh
Upcoming SlideShare
Loading in...5
×
 

Workshop8 creep-mesh

on

  • 555 views

abaqus Workshop

abaqus Workshop

Statistics

Views

Total Views
555
Views on SlideShare
555
Embed Views
0

Actions

Likes
0
Downloads
47
Comments
0

0 Embeds 0

No embeds

Accessibility

Upload Details

Uploaded via as Adobe PDF

Usage Rights

© All Rights Reserved

Report content

Flagged as inappropriate Flag as inappropriate
Flag as inappropriate

Select your reason for flagging this presentation as inappropriate.

Cancel
  • Full Name Full Name Comment goes here.
    Are you sure you want to
    Your message goes here
    Processing…
Post Comment
Edit your comment

    Workshop8 creep-mesh Workshop8 creep-mesh Document Transcript

    • Workshop 8 Structured Hex Meshing: Pipe Creep Model You need to consider the type of element that will be used before you start building the mesh for a particular problem. A suitable mesh design that uses quadratic elements may very well be unsuitable if you change to linear, reduced-integration elements. For this example use 20-node hexahedral elements with reduced integration (C3D20R). Once you have selected the element type, you can design the mesh for the intersecting pipes. A possible mesh for the intersecting pipes is shown in Figure W8–1. Figure W8–1. Suggested mesh of C3D20R elements for the intersecting pipe model ABAQUS/CAE offers a variety of meshing techniques to mesh models of different topologies. The different meshing techniques provide varying levels of automation and user control. The following three types of mesh generation techniques are available: Structured meshing Structured meshing applies pre-established mesh patterns to particular model topologies. Complex models, however, must generally be partitioned into simpler regions to use this technique. Swept meshing Swept meshing extrudes an internally generated mesh along a sweep path or revolves it around an axis of revolution. Like structured meshing, swept meshing is limited to models with specific topologies and geometries. Free meshing The free meshing technique is the most flexible meshing technique. It uses no pre- established mesh patterns and can be applied to almost any model shape.
    • When you enter the Mesh module, ABAQUS/CAE color codes regions of the model according to the methods it will use to generate a mesh: · Green indicates that a region can be meshed using structured methods. · Yellow indicates that a region can be meshed using sweep methods. · Pink indicates that a region can be meshed using the free method. · Orange indicates that a region cannot be meshed using the default element shape assignment and must be partitioned further. In this problem you will create a structured mesh. You will find that the model must first be partitioned further to use this mesh technique. After the partitions have been created, a global part seed will be assigned and the mesh will be created. To begin this workshop, start a new session of ABAQUS/CAE from the workshops/pipeCreep directory. Open the database containing the pipe creep model. To partition the pipe model: 1. From the Module list located under the toolbar, select Mesh to enter the Mesh module. The part is colored orange initially, indicating that with the default set of mesh controls, a hexahedral mesh cannot be created. Cell partitions are required to permit structured meshing. 2. Partition the pressure vessel in half as shown in Figure W8–2: A. From the main menu bar, select ToolsPartition to open the Create Partition dialog box. B. In this dialog box, select Cell as the type and Define cutting plane as the method. C. Click OK. D. In the prompt area, choose the Point & Normal technique to define the cutting plane. Choose the point indicated in Figure W8–2 as the point through which the cutting plane will pass and any vertical edge of the pipe as the normal to the plane. The bottom half of the vessel turns green, indicating it is structured meshable. W8.2
    • Figure W8–2. Cell partition The region containing the pipe intersection will be partitioned using a combination of face and cell partitions. These partitions are described next. 3. Partition the faces of the pipes on the symmetry planes as follows: A. From the main menu bar, select ToolsPartition to open the Create Partition dialog box. E. In this dialog box, select Face as the type and Sketch as the method. F. Click OK. G. Select the face shown in Figure W8–3 as the face to be partitioned. H. Choose the edge shown in Figure W8–3 as the edge that will appear vertical and on the right side of the sketch. I. From the main menu bar, select AddConstruction to define two Vertical and two Horizontal construction lines, as indicated in Figure W8–4. J. Use the Create Lines: Connected tool to define two sketch lines as indicated in Figure W8–4. K. Repeat steps A through G for the symmetry face shown in Figure W8–5. Create the construction geometry and sketch lines indicated in Figure W8–6. The partitioned symmetry faces appear as shown in Figure W8–7. Point through which cutting plane passes Normal to the cutting plane W8.3
    • Figure W8–3. First face partition Figure W8–4. Construction geometry for first face partition Partition this face Edge that will appear vertical and on the right of the sketch Horizontal construction line through vertex A A B Vertical construction line through vertex B Additional horizontal and vertical construction lines W8.4 Sketch lines; use intersections of construction lines as snap points
    • Figure W8–5. Second face partition Figure W8–6. Construction geometry for second face partition W8.5 C Horizontal and vertical construction lines through vertex C Additional vertical construction line Horizontal sketch line from vertex C to the intersection of the construction lines Skewed sketch line from vertex D to the intersection between construction line and curved edge of part D Partition this face Edge that will appear vertical and on the right of the sketch
    • Figure W8–7. Partitioned symmetry faces 4. Partition the inner surface of the pressure vessel using a curved path between two edges: A. From the main menu bar, select ToolsPartition to open the Create Partition dialog box. L. In this dialog box, select Face as the type and Curved path normal to 2 edges as the method. M. Click OK. N. Select the face shown in Figure W8–8 as the face to be partitioned. O. In the prompt area, choose Pick as the method by which to select the edge points. P. Select the edges and points indicated in Figure W8–9 to define the partition. The partitioned face appears as shown in Figure W8–10. W8.6
    • Figure W8–8. Inner surface of pressure vessel Figure W8–9. Edges and points used to define partition W8.7 edge point edge point
    • Figure W8–10. Partitioned inner face 5. Finally, partition the cells of the pipe using the n-sided patch technique: A. From the main menu bar, select ToolsPartition to open the Create Partition dialog box. Q. In this dialog box, select Cell as the type and N-sided patch as the method. R. Click OK. S. Select the top half of the pipe as the region to be partitioned. In the prompt area, click Select Corner Points as the method by which to specify the patch. Use 4 corner points to define the patch. T. Select the points indicated in Figure W8–11 as the points defining the patch, and create the partition. Be sure to select the points in the order indicated in the figure. The top portion of the pipe is now colored green. U. Repeat the above steps to partition the center cell of the model using the points indicated in Figure W8–12 as the points defining the 4-sided patch. 6. After you have partitioned the part, all part regions should be colored green, as shown in Figure W8–13. This indicates structured hexahedral element meshing will be used everywhere. W8.8
    • Figure W8–11. First 4-sided patch Figure W8–12. Second 4-sided patch W8.9 Point 1 Point 2 Point 3 Point 4 Point 3 Point 4 Point 1 Point 2
    • Figure W8–13. Partitioned geometry To assign a global part seed and create the mesh: 1. From the main menu bar, select SeedInstance; specify a target global element size of 0.027. Seeds appear on all the edges. 7. From the main menu bar, select MeshElement Type to choose the element type for the part. Because of the partitions you have created, the part is now composed of several regions. A. Use the cursor to draw a box around the entire part and, thus, select all regions of the part. Click Done in the prompt area. V. In the Element Type dialog box that appears, select the Standard element library, 3D Stress family, Quadratic geometric order, and Hex, Reduced integration element. Click OK to accept the choice of C3D20R as the element type. 8. From the main menu bar, select MeshInstance. Click Yes in the prompt area to mesh the part instance. The resulting mesh is shown in Figure W8–1. 9. Save your model database, and exit your ABAQUS/CAE session. W8.10