Ansys beam problem
- 2. Beam elements are line elements used to create a one-dimensional idealization of a 3- D structure. They are computationally more efficient than solids and shells and are heavily used in several industries: ◦ Building construction ◦ Bridges and roadways ◦ People movers (trams, railcars, buses) ◦ Etc.
- 3. A brief introduction to beam modeling via the following topics: A. Beam Properties B. Beam Meshing C. Loading, Solution, Results
- 4. The first step in beam modeling, as with any analysis, is to create the geometry — usually just a framework of keypoints and lines. Then define the following beam properties: ◦ Element type ◦ Cross section ◦ Material
- 5. Element Type Choose one of the following types: ◦ BEAM188 — 3-D, linear (2-node) ◦ BEAM189 — 3-D, quadratic (3-node) ANSYS has many other beam elements, but BEAM188 & 189 are generally recommended. ◦ Applicable to most beam structures ◦ Support linear as well as nonlinear analyses, including plasticity, large deformation, and nonlinear collapse ◦ Ability to include multiple materials to simulate layered materials, composites, reinforced sections, etc. ◦ Ability to create “user defined” section geometry ◦ Easy to use, both in preprocessing and postprocessing phases
- 6. Cross Section To completely define a BEAM188 or 189 element, you also need to specify its cross section properties. The BeamTool provides a convenient way to do this. ◦ Preprocessor > Sections > Common Sectns... ◦ Select the desired shape, then enter its dimensions. ◦ Press the Preview button to view the shape, then OK to accept it. ◦ If there are multiple cross sections, specify a different section ID number (and an optional name) for each.
- 7. A sample preview (SECPLOT) of an I-beam cross section is shown below. In addition to the predefined cross-section shapes, ANSYS allows you to create your own, “user-defined” shape by building a 2-D solid model. You can save user-defined sections as well as standard sections with the desired dimensions in a section library for later use. See Chapter 15 of the ANSYS Structural Analysis Guide for more information.
- 8. Material Properties Both linear and nonlinear material properties are allowed. After all beam properties are defined, the next step is to mesh the geometry with beam elements.
- 9. Meshing the geometry (lines) with beam elements involves three main steps: ◦ Assign line attributes ◦ Specify line divisions ◦ Generate the mesh The MeshTool provides a convenient way to perform all three steps.
- 10. Step 1: Line Attributes Line attributes for beam meshing consist of: ◦ Material number ◦ Section ID ◦ Orientation keypoint Determines how the cross section is oriented with respect to the beam axis. Must be specified for all cross-section types. A single keypoint can be assigned to multiple lines (i.e, no need to specify a separate keypoint for each line). Each end of a line can have its own orientation keypoint, allowing the cross section to be “twisted” about the beam axis.
- 11. Examples of using orientation keypoints:
- 12. To assign line attributes, use the “Element Attributes” section of the MeshTool (or select desired lines and use the LATT command). Pick lines Additional attributes for BEAM188 & 189
- 13. Step 2: Line Divisions For BEAM188 and 189 elements, a single element spanning the entire beam length is not recommended. Use the “Size Controls” section of the MeshTool (or the LESIZE command) to specify the desired number of line divisions.
- 14. Step 3: Generate the Mesh First save the database (Toolbar > SAVE_DB or SAVE command). Then press the Mesh button in the MeshTool (or issue LMESH,ALL) to generate the mesh. Pick lines
- 15. To see the cross-section shape in the element display, activate the element shape key: ◦ Utility Menu > PlotCtrls > Style > Size and Shape… ◦ Or /ESHAPE,1
- 16. After beam meshing is completed, the next step is to apply loads and solve.
- 17. Typical loading for beam models consists of: ◦ Displacement constraints applied at keypoints or nodes ◦ Forces applied at keypoints or nodes ◦ Pressures load per unit length applied on element faces Solution > Apply > Pressures > On Beams Or SFBEAM command ◦ Gravity or rotational velocity acts on entire structure
- 18. To obtain the solution: ◦ First save the database. ◦ Then solve. (Or write the loads to a load step file and solve all load steps later.) Results review is the same as for other stress analyses: ◦ View the deformed shape ◦ Check reaction forces ◦ Plot stresses and strains The main advantage of BEAM188 and 189 is that with the element shape key activated (/ESHAPE,1), stresses can be directly viewed on the elements (similar to solids and shells).
- 19. Demo: ◦ Resume frame.db (contains lines, kp’s, loading, element type, material, and two cross sections) ◦ Plot the two cross section already defined (SECPLOT,1 & 2) ◦ Define a third cross section using the BeamTool: ID=3: Name = peak, Sub-type = box (hollow rectangle), W1=6, W2=6; T1=T2=T3=T4=0.25 ◦ Bring up MeshTool, GPLOT, then assign the following line attributes: Sloping lines: mat=1, secnum=3, orientation KP = topmost KP (#100) Left vertical lines: mat=1, secnum=2, orientation KP = #102 Right vertical lines: mat=1, secnum=2, orientation KP = #101 Left & front horizontal lines: mat=1, secnum=1, orientation KP = #1 Right & back horizontal lines: mat=1, secnum=1, orientation KP = #3 ◦ Specify size=20 on all lines ◦ Save, then LMESH,ALL; then EPLOT with /ESHAPE,1 ◦ Constrain the 4 bottom keypoints in all DOFs and apply a force of -10,000 lb in the fy direction on keypoint #9 ◦ Solve, then review results: deformed shape (animate), reaction forces, SX stresses (= axial + bending). Select elements with section ID=3 and replot stresses. Repeat for ID=2. October 30, 2001 Inventory #001571 5-19
- 20. This workshop consists of the following problem: W4. Building Frame Please refer to your Workshop Supplement for instructions. October 30, 2001 Inventory #001571 5-20