Upcoming SlideShare
×

# Workshop12 skewplate

386

Published on

abaqus Workshop

Published in: Technology, Automotive
0 Likes
Statistics
Notes
• Full Name
Comment goes here.

Are you sure you want to Yes No
• Be the first to comment

• Be the first to like this

Views
Total Views
386
On Slideshare
0
From Embeds
0
Number of Embeds
0
Actions
Shares
0
80
0
Likes
0
Embeds 0
No embeds

No notes for slide

### Transcript of "Workshop12 skewplate"

1. 1. Workshop 12 Nonlinear Analysis of a Skew Plate Introduction You have been asked to model the plate shown in Figure W12–1. It is skewed 30° to the global 1-axis, is built-in at one end, and is constrained to move on rails parallel to the plate axis at the other end. You are to determine the midspan deflection when the plate carries a uniform pressure. You are to perform both linear and nonlinear static and dynamic analyses.
2. 2. Figure W12–1. Sketch of the skewed plate Defining the model geometry Start ABAQUS/CAE in the workshops/skewPlate directory, and enter the Part module. A default model name is assigned by ABAQUS/CAE (Model-1). However, since the linear analysis model will later form the basis of the nonlinear analysis model, you should rename the current model to give it a more descriptive name. · From the main menu bar, select ModelRenameModel-1. Rename the model linear. Create a three-dimensional, deformable body with a planar shell base feature. Name the part Plate, and specify an approximate part size of 4.0. A suggested approach to creating the part geometry is outlined in the following procedure: To sketch the plate geometry: 1. In the Sketcher create a vertical line of length 0.4 m using the Create Lines: Connected tool. W12.2
3. 3. 2. Using the Create Construction: Line at an Angle tool, create a construction line oriented 30° with respect to the horizontal through each of the line’s endpoints. 3. Using the Create Isolated Point tool, create an isolated point at a horizontal distance of 1.0 m to the right of the vertical line. Create a vertical construction line through this point. 4. Using the Create Lines: Connected tool, draw the skewed rectangle using the preselection points at the intersections of the construction lines to position the corner vertices. The final sketch is shown in Figure W12–2. Figure W12–2. Sketch of the plate geometry 5. In the prompt area, click Done to finish the sketch. Defining the material and section properties and the local material directions The plate is made of an isotropic, linear elastic material with a Young's modulus E = 30E9 Pa and a Poisson's ratio  = 0.3. Enter the Property module, and create the material definition; name the material Steel. The orientation of the structure in the global coordinate system is shown in Figure W12–1. 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 material 1-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 the 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 1-axis) and the local y’-direction is also in the plane of the plate. W12.3
4. 4. To define shell section properties and local material directions: 1. Define a homogeneous shell section named PlateSection. Assign a shell thickness of 0.8E-2 and the Steel material definition to the section. Specify that section integration be performed before the analysis since the material is linear elastic. 6. Define a rectangular datum coordinate system as shown in Figure W12–3 using the Create Datum CSYS: 2 Lines tool . Figure W12–3. Datum coordinate system used to define local material directions 7. From the main menu bar, select AssignMaterial Orientation and select the entire part as the region to which local material directions will be applied. In the viewport, select the datum coordinate system created earlier. Select Axis-3 for the direction of the approximate shell normal. No additional rotation is needed about this axis. Tip: To verify that the local material directions have been assigned correctly, select ToolsQuery 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. 8. Assign the section definition to the plate. Creating an assembly, defining an analysis step, and specifying output requests Instance the plate in the Assembly module. Before leaving the Assembly module, define geometry sets to facilitate output request and boundary condition definitions. You will first need to partition the plate in half to create a geometry set at the plate midspan. W12.4 Select this edge to be along the local x’-direction Select this edge to be in the local x’-y’ plane
5. 5. To partition the plate and define geometry sets: 1. Partition the plate in half using the Partition Face: Shortest Path Between 2 Points tool . Use the midpoints of the skewed edges of the plate to create the partition shown in Figure W12–4. Figure W12–4. Partition used to define a geometry set at the plate midspan 9. Select ToolsSetCreate to create a geometry set for the midspan named MidSpan. Similarly, create sets for the left and right edges of the plate and name them EndA and EndB, respectively. Next, create a single static, general step in the Step module. Name the step Apply Pressure, and specify the following step description: Uniform pressure (20 kPa) load. Accept all the default settings for the step. Among the output you will need are the nodal displacements and element stresses as field data. These data will be used to create deformed shape plots and contour plots in ABAQUS/Viewer. You will also want to write the displacements at the midspan as history data to create X–Y plots in ABAQUS/Viewer. To change the default output requests: 1. Edit the field output request so that only the nodal displacements and element stresses for the whole model are written as field data to the output database (.odb) file. 10. Edit the history output request so that only nodal displacements for the MidSpan geometry set are written as history data to the output database file. Prescribing boundary conditions and applied loads As shown in Figure W12–1, 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 aligned with the plate. You can use the datum coordinate system that you created earlier to define the local material directions. W12.5 EndB EndA MidSpan
6. 6. To assign boundary conditions in a local coordinate system: 1. Switch to the Load module. 11. Select BCCreate, and define a Displacement/Rotation mechanical boundary condition named Rail boundary condition in the Initial step. In this 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. 12. From the Region Selection dialog box that appears, select set 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. 13. In the Edit Boundary Condition dialog box, click Edit to specify the local coordinate system in which the boundary condition will be applied. In the viewport, select the datum coordinate system that was created earlier to define the local directions. The local 1-direction is aligned with the plate axis. 14. In the Edit Boundary Condition dialog box, fix all degrees of freedom except for U1. 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 (displacements, velocities, reaction forces, etc.) will be defined in this local coordinate system. Complete the boundary condition definition by fixing all degrees of freedom at the left edge of the plate (set EndA). Name this boundary condition Fix left end. Use the default global directions for this boundary condition. Finally, define 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 (Magenta) as the surface to which the pressure load will be applied. You may need to rotate the view to more clearly distinguish the top side of the plate. Specify a load magnitude of 2.0E4 Pa. Creating the mesh and defining a job Figure W12–5 shows the suggested mesh for this simulation. W12.6