1. ELEMENTS Chapter 2

2. Training Manual March 15, 2001 Inventory #001458 2-2 Chapter Objectives Upon completion of this chapter, students will be able to define and utilize explicit dynamic elements within the ANSYS/LS-DYNA Program. 1. Give an overview of the explicit dynamic family of elements 2. Describe reduced integration elements and hourglassing 3. Describe in detail each explicit dynamic element type 4. List guidelines for using explicit dynamic elements 5. Given step-by-step guidance, a deep drawing simulation is done

3. Training Manual March 15, 2001 Inventory #001458 2-3 Overview of Explicit Dynamic Elements The ANSYS/LS-DYNA program has 8 different element types that can be defined: –LINK160: explicit pin-jointed truss (similar to LINK8) –BEAM161: explicit beam (similar to BEAM4) –PLANE162: 2-D explicit planar solid (similar to PLANE42) –SHELL163: explicit thin shell (similar to SHELL181) –SOLID164: explicit brick (similar to SOLID185) –COMBI165: explicit spring and damper (similar to COMBIN14) –MASS166: explicit structural mass (similar to MASS21) –LINK167: explicit cable element (similar to LINK10) All of the explicit dynamic element types are 3-D except SOLID162

4. Training Manual March 15, 2001 Inventory #001458 2-4 (continued) Overview of Explicit Dynamic Elements The explicit family of elements are distinctly different from ANSYS implicit elements in the following aspects: –Each element type is valid for nearly all material models. In ANSYS implicit, different element types exist for specialized material models such as hyperelasticity (HYPER56, 58, and 74) and viscoplasticity (VISCO106 and 108). –Each element type may have several different formulations. If ANSYS implicit elements have more than one formulation, they are given different element names (e.g., SHELL43 and 63). In ANSYS/LS-DYNA, each element type can have multiple formulations - SHELL163 has the most with eleven. –All explicit dynamic elements have a linear displacement function. Higher order elements with a quadratic displacement function are not available. –Each explicit dynamic element uses single point integration by default. –Elements with extra shape functions and midside nodes are not available. P- elements are also not available. –Elements support all nonlinear options allowed in ANSYS/LS-DYNA.

5. Training Manual March 15, 2001 Inventory #001458 2-5 Reduced Integration Elements A reduced integration element is an element which uses a minimum number of integration points. A reduced integration brick element will have one integration point at its center and a reduced shell has one in-plane integration point. Fully integrated brick and shell elements have eight and four in-plane integration points, respectively. –One of the most CPU expensive portions of explicit dynamic analyses is element processing. –Since the number of integration points are directly proportional to CPU time, all explicit dynamic elements have reduced integration by default. –In addition to saving CPU, one point integration elements are also extremely robust in the case of large deformations. In fact, ANSYS/LS-DYNA elements can undergo much greater deformations than standard ANSYS implicit elements. –There are two basic disadvantages of reduced integration elements: Deformations with zero energy modes are possible (Hourglassing). The accuracy of stress results is directly related to the number of the integration points.

6. Training Manual March 15, 2001 Inventory #001458 2-6 Hourglassing Hourglassing is a zero-energy mode of deformation that oscillates at a frequency much higher than the structure’s global response. Hourglassing modes result in stable mathematical states that are not physically possible. They typically have no stiffness and give a zigzag deformation appearance to a mesh. –Single-point (reduced) integration elements are prone to zero energy modes. –The occurrence of hourglass deformations in an analysis can invalidate results and should always be minimized or eliminated. –If the overall hourglass energy is more than 10% of the internal energy of a model, there is likely a problem with the analysis. Determining hourglass energy will be discussed in Chapter 8 (GLSTAT and MATSUM files). Even 5% can be considered excessive, in some cases.

7. Training Manual March 15, 2001 Inventory #001458 2-7 Zero energy deformation for the one-point integrated solid element: There is a need to control the zero energy modes Hourglass control brings additional stiffness or viscous damping to prevent such modes. Elements - Hourglass Modes

8. Training Manual March 15, 2001 Inventory #001458 2-8 Solution: Analysis Options -> Bulk Viscosity It is not recommended to dramatically change the default values (1.5 and.06) of the EDBVIS command because of the adverse effects that they will have on the global modes of the structure. Minimizing Hourglassing In ANSYS/LS-DYNA there are several ways to minimize hourglassing: Method 1: Avoid single point loads –Single point loads are known to excite hourglass modes. Since one excited element transfers the mode to its neighbors, point loads should not be applied. Method 2: Use fully integrated elements –Fully integrated elements do not experience hourglassing modes. Defining part or all of a model with fully integrated elements (by KEYOPTS) will eliminate hourglassing. Not available for PLANE162. Method 3: Globally adjust the model’s bulk viscosity –Hourglass deformations are resisted by a structures bulk viscosity. It is possible to increase the bulk viscosity of a model using the linear and quadratic coefficients of the EDBVIS command:

9. Training Manual March 15, 2001 Inventory #001458 2-9 Care should be used when increasing the hourglassing coefficient. Values above.15 have been found to over- stiffen the models response during large deformations and cause instabilities. (continued) Minimizing Hourglassing Method 4: Globally adding elastic stiffness –Hourglassing can also be eliminated by adding elastic stiffness. This can be done for the entire model by increasing the hourglassing coefficient (HGCO) of the EDHGLS command: Solution: Analysis Options -> Hourglass Ctrls -> Global Method 5: Locally adding elastic stiffness –It is sometimes advantageous to resist hourglass deformations in high risk areas of a model without dramatically changing the model’s global stiffness. For such a purpose, the EDMP, HGLS command can be used to apply hourglass control only to a specific material. –Specify the hourglass control type (viscous or stiffness), hourglass coefficient, and bulk viscosity coefficient to minimize hourglassing.

10. Training Manual March 15, 2001 Inventory #001458 2-10 Defining Explicit Dynamic Elements Explicit dynamic elements are defined using standard ANSYS procedures –Step 1: Select LS-DYNA Explicit for ANSYS GUI filtering Main Menu : Preferences: Selecting LS-DYNA Explicit will limit the elements available in the current analysis to the explicit family. It is very important to remember that explicit and implicit elements can not be used in the same analysis. If implicit elements are defined in the same model, the analysis will automatically be terminated upon execution of the SOLVE command.

11. Training Manual March 15, 2001 Inventory #001458 2-11 STEP 2: Add element type Preprocessor: Element type -> Add/Edit/Dele.... Note that only the explicit elements 160 – 167 are available in the element library Real constants and KEYOPTS are defined for elements using standard ANSYS format. (continued) Defining Explicit Dynamic Elements

12. Training Manual March 15, 2001 Inventory #001458 2-12 LINK160 Pin-Jointed Truss Element This 3D spar element is used to carry an axial load. Three nodes are used to define the element. –The 3rd node is for the initial spar orientation.

13. Training Manual March 15, 2001 Inventory #001458 2-13 BEAM161 Beam Element This 3D beam is suited for rigid body rotations because it does not generate strains. Three nodes are used to define the element. –The 3rd node is for the initial orientation of the beam. Several standard beam cross sections can be defined.

14. Training Manual March 15, 2001 Inventory #001458 2-14 PLANE162 2D Element PLANE162 - 2D, 4-Node Solid –3-node triangle available (not recommended) –Only Lagrangian formulation supported –UX, UY, VX, VY, AX, AY degrees of freedom –Y axis = symmetry axis for axisymmetric models –NO mixing of 2D and 3D element types permitted –Fully integrated option not available PLANE162 KEYOPT Settings: –Keyopt(2) - Area weighted or volume weighted (AXISYM) –Keyopt(3) - Plane stress, axisymmetric, or plane strain Only one 2D type can be used in any given analysis (i.e., you cannot have both axisymmetric and plane stress elements present in the same model) I J K L SHELL162: 2-D PLANAR SOLID x y

15. Training Manual March 15, 2001 Inventory #001458 2-15 PLANE162 2D Element (continued) PLANE162 modeled in X-Y plane (+X for axisymmetric case) No real constants associated with PLANE162 18 materials (e.g., plasticity, composite, Mooney-Rivlin) supported RSYS supported for displacements and stresses (not strains) Lagrangian formulation is based on large strain deformation theory in which bodies of interest are discretized and the geometry is continuously updated over time as the mesh physically deforms. This formulation is used in implicit ANSYS, as well.

16. Training Manual March 15, 2001 Inventory #001458 2-16 SHELL163 Thin Shell Element Shell163 has 11 different element formulations. The most important are: Belytschko-Tsay (BT, KEYOPT(1)=2, default): – Simple shell element – Very fast – Wrong results for warping Belytschko-Wong-Chiang (BWC, KEYOPT(1)=10): – Performance factor 1.25 * BT – Correct results for warping – Recommended Belytschko-Leviathan (BL, KEYOPT(1)=8): – CPU factor 1.4 * BT – New and still in development – First element with physical hourglass control – (no parameters for EDMP,HGLS,Mat,Val1) S/R co-rotational Hughes-Liu (S/R CHL, KEYOPT(1)=7): – Shell without hourglassing – CPU factor 8.8 * BT

17. Training Manual March 15, 2001 Inventory #001458 2-17 CPU factor 2.45*BT KEYOPT(1)=1 1 integration point normalco-rotational normal “full reduced” selective reduced “full integrated” CPU factor 1.49*BT KEYOPT(1)=11 1 integration point CPU factor 20.01*BT KEYOPT(1)=6 4 integration points CPU factor 8.84*BT KEYOPT(1)=7 4 integration points This formulation is comparable to the formulation of SHELL143 SHELL163 Thin Shell Element (continued) The Hughes-Liu shell element formulation is available in 4 variations:

18. Training Manual March 15, 2001 Inventory #001458 2-18 SHELL163 Thin Shell Element (continued) The element formulations BT, BWC, BL uses only one integration point in plane but the S/R CHL uses 4-point integration. All shell elements can have an arbitrary number of integration points through the thickness. –2 integration points through the thickness are necessary for elastic behavior (default) –3 to 5 integration points through the thickness are necessary for plastic behavior (recommended) –Use the real constants to define the number of integration points R, nset, r1, r2, r3 –nset is the real constant set reference number –r1=shear factor, 5/6 is recommended for thin shells –r2=number of integration points –r3=element thickness

19. Training Manual March 15, 2001 Inventory #001458 2-19 (continued) SHELL163 Thin Shell Element Specify the number of integration points through the thickness for output with the EDINT command Solution: Output Ctrls -> Integ Pt Storage… –EDINT, SHELLIP, BEAMIP SHELLIP is the number of shell integration points for output SHELLIP > 3 Each integration point is associated with a LAYER Default is 3 for top, middle and bottom layers BEAMIP is the number of beam integration points for output

20. Training Manual March 15, 2001 Inventory #001458 2-20 (continued) SHELL163 Thin Shell Element Two element formulations for triangular shells: –C0 triangular shell (KEYOPT(1)=4) Based on Mindlin-Reissner plate theory Formulation is rather stiff, not recommended for constructing an entire mesh –BCIZ triangular shell (KEYOPT(1)=3) Based on Kirchhoff plate theory Slow –Nevertheless, in mixed meshes, C0 triangular shells are better than degenerated 4 noded element formulations. So always include the following command if area meshes are mixed (free meshing): EDSHELL,,,,,,ITRST –ITRST = 1 : degenerated quadrilateral shells are treated as triangular shells (default) –ITRST = 2 : degenerated quadrilateral shells remains unchanged Preprocessor: Shell Elem Ctrls > Full Sorting > OK

21. Training Manual March 15, 2001 Inventory #001458 2-21 SHELL163 Membrane Element Formulation Two membrane element formulations are available: –Belytschko-Tsay-Membrane (KEYOPT(1)=5): Simple membrane element with one point integration –Fully integrated Belytschko-Tsay-Membrane (KEYOPT(1)=9): Membrane element with 4-point integration

22. Training Manual March 15, 2001 Inventory #001458 2-22 SOLID164 8-noded Brick Element You can chose two element formulations: –one point integrated solid (constant stress over the element) The one point integrated element (default) is very fast and very robust for large element deformations. It may require hourglass controls to prevent hourglass modes. –fully integrated solid (2x2x2 integration) The fully integrated solid is slower, but has no hourglass modes. However, it can experience both shear locking and volumetric locking (for high Poisson’s ratios). More so than in standard ANSYS, a degenerated tetrahedral mesh is strongly not recommended. The mapped mesh is best suited for explicit dynamics; a dragged or extruded mesh with singular prisms is acceptable.

23. Training Manual March 15, 2001 Inventory #001458 2-23 COMBI165 Spring and Damper Element Defined using two nodes and discrete material properties It can be connected to all other elements It may have translational or torsional properties Complex nonlinear force-displacement relations are possible Unlike COMBIN14, springs and dampers must be separate elements Since only the spring or damper option can be used with COMBI165, two elements must be overlaid for a spring-damper assembly.

24. Training Manual March 15, 2001 Inventory #001458 2-24 MASS166 Mass Element MASS 166 is a point mass element having up to nine DOF’s: translations, velocities, and accelerations in x, y, and z directions. The element has additional option for rotary inertia without mass: KEYOPT(1)=0 3-D Mass without inertia: mass input KEYOPT(1)=1 3-D Rotary inertia (no mass): 6 inertia values input This element is used to adjust the mass of a complex model like a full car crash model, where many components (e.g., seats, headlights, instruments panel, dummy,...) are not modeled

25. Training Manual March 15, 2001 Inventory #001458 2-25 LINK167 Cable Element Three noded tension only element. – 3rd node initially orients element It can be used to model cables.

26. Training Manual March 15, 2001 Inventory #001458 2-26 General Element Guidelines Avoid small elements whenever possible as they will significantly reduce the time step size. If small elements are required, use mass scaling (see Chapter 7). Minimize the use of triangular/tetrahedron/prism elements. Although these elements are supported, they are highly not recommended. Avoid acute angled elements and warped shells, as they will degrade the accuracy of the results. Fully integrated elements can be defined in regions of a model where hourglass control is needed. Volumetric locking (due to Poisson’s ratios approaching 0.5) and shear locking (e.g., in the bending of a simply supported beam) are possible with fully integrated brick elements.

27. Training Manual March 15, 2001 Inventory #001458 2-27 Deep Drawing Exercise The exercise for this chapter begins on page E2-1of Volume II. A deep drawing simulation is used to demonstrate the tremendous capability of the ANSYS/LS-DYNA product. All of these features will be discussed in subsequent chapters, so just follow the detailed instructions for now. This exercise will then serve as a good review problem at the completion of the course.