1. Static Structural Analysis Chapter Four

2. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-2 Chapter Overview In this chapter, performing linear static structural analyses in Simulation will be covered: –Geometry and Elements –Contact and Types of Supported Assemblies –Environment, including Loads and Supports –Solving Models –Results and Postprocessing The capabilities described in this section are generally applicable to ANSYS DesignSpace Entra licenses and above. –Some options discussed in this chapter may require more advanced licenses, but these are noted accordingly. –Free vibration, harmonic, and nonlinear structural analyses are not discussed here but in their respective chapters.

3. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-3 Basics of Linear Static Analysis For a linear static structural analysis, the displacements {x} are solved for in the matrix equation below: Assumptions: –[K] is constant Linear elastic material behavior is assumed Small deflection theory is used Some nonlinear boundary conditions may be included –{F} is statically applied No time-varying forces are considered No inertial effects (mass, damping) are included It is important to remember these assumptions related to linear static analysis. Nonlinear static and dynamic analyses are covered in later chapters.

4. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-4 A. Geometry In structural analyses, all types of bodies supported by Simulation may be used. For surface bodies, thickness must be supplied in the “Details” view of the “Geometry” branch. The cross-section and orientation of line bodies are defined within DesignModeler and are imported into Simulation automatically. –For line bodies, only displacement results are available.

5. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-5 … Point Mass A Point Mass is available under the Geometry branch to mimic weight not explicitly modeled –A point mass is associated with surface(s) only –The location can be defined by either: (x, y, z) coordinates in any user-defined Coordinate System Selecting vertices/edges/surfaces to define location –In a structural static analysis, the point mass is affected by “Acceleration,” “Standard Earth Gravity,” and “Rotational Velocity”. No other loads affect a point mass. –The mass is ‘connected’ to selected surfaces assuming no stiffness between them. –No rotational inertial terms are present.

6. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-6 … Point Mass A point mass will be displayed as a round, grey sphere –a point mass in a linear static analysis can be used to account for the additional mass of a structure not modeled –No results are obtained for the Point Mass itself

7. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-7 … Material Properties Young’s Modulus and Poisson’s Ratio are required for linear static structural analyses –Material input is handled in the “Engineering Data” application –Materials are assigned per part in the geometry branch –Mass density is required if any inertial loads are present –Thermal expansion coefficient and thermal conductivity are required if any thermal loads are present –Stress Limits are needed if a Stress Tool result is present –Fatigue Properties are needed if Fatigue Tool result is present Requires Fatigue Module add-on license

8. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-8 … Material Properties Engineering Data view shown below:

9. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-9 B. Assemblies – Solid Body Contact When importing assemblies of solid parts, contact regions are automatically created between the solid bodies. –Contact allows non-matching meshes at boundaries between solid parts –Tolerance controls under “Contact” branch allows the user to specify distance of auto contact detection via slider bar

10. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-10 … Assemblies – Solid Body Contact In Simulation, the concept of contact and target surfaces are used for each contact region –One side of a contact region is referred to as a contact surface, the other side is referred to as a target surface –The contact surfaces are restricted from penetrating through the target surfaces however the opposite is not true When one side is the contact and the other side is the target, this is called asymmetric contact. If both sides are made to be contact & target this is called symmetric contact By default, Simulation uses symmetric contact for solid assemblies For ANSYS Professional licenses and above, the user may change to asymmetric contact, as desired

11. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-11 … Assemblies – Solid Body Contact Four contact types are available: –Bonded and No Separation contact are basically linear and require only 1 iteration –Frictionless and Rough contact are nonlinear and require multiple iterations (small deflection theory is still assumed) An “interface treatment” option is available: –“Add Offset”: input zero or non-zero value for initial adjustment –“Adjusted to Touch”: ANSYS closes any gap to a just touching position (ANSYS Professional and above)

12. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-12 … Assemblies – Solid Body Contact For the advanced user, some of the contact options can be modified –Formulation can be changed from “Pure Penalty” to “Augmented Lagrange,” “MPC,” or “Normal Lagrange.” “MPC” is applicable to bonded contact only “Augmented Lagrange” is used in classic ANSYS Note: the MPC formulation writes constraint equations relating the movement of parts at an interface. This can be an attractive alternative to penalty method for bonded contact. Additional information on advanced contact is presented in the Workbench nonlinear course as well as the ANSYS documentation

13. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-13 … Assemblies – Solid Body Contact Advanced options (continued): –Pin Ball Region: Inside pinball = near-field contact Outside pinball = far-field contact Allows the solver to more efficiently process contact calculations Other advanced contact options will be discussed in Chapter 11. In this case, the gap between the two parts is bigger than the pinball region, so no automatic gap closure will be performed.

14. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-14 … Assemblies – Surface Body Contact For ANSYS Professional licenses and above, mixed assemblies of shells and solids are supported –More contact options are exposed to the user –Contact postprocessing is also available (discussed later)

15. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-15 … Assemblies – Surface Body Contact Edge contact is a subset of general contact –For contact including shell faces or solid edges, only bonded or no separation behavior is allowed –For contact involving shell edges, only bonded behavior using MPC formulation is allowed If a gap exists the pinball region can be used to detect contact beyond the gap.

16. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-16 … Assemblies – Contact Summary Summary of contact types and options available in Simulation:

17. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-17 … Assemblies – Spot Weld Spot welds provide a means of connecting shell assemblies at discrete points –Spotweld definition is done in the CAD software. Currently, only DesignModeler and Unigraphics define spotwelds in a manner that Simulation supports. –Spotwelds can also be created in Simulation manually, but only at discrete vertices.

18. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-18 C. Loads and Supports There are four types of structural loads available: –Inertial loads These loads act on the entire system Density is required for mass calculations These are only loads which act on defined Point Masses –Structural Loads These are forces or moments acting on parts of the system –Structural Supports These are constraints that prevent movement on certain regions –Thermal Loads Structurally speaking, the thermal loads result in a temperature field, which causes thermal expansion on the model.

19. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-19... Time Type A time type option is available at certain license levels The default time type for loading is “static” “Transient” and “harmonic” time types are available as options Sequence loading allows a series of static time steps to be set up in advance and solved at once Sequenced results can be reviewed step by step

20. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-20... Time Type Specify the desired number of sequence steps in the “Steps” field in the main toolbar. Enter the value of the load for each step by first highlighting the desired step in the graphics window. The chart in the graphics window displays the variation of the load while a legend in the graphics window displays the current view setting.

21. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-21... Time Type Results of a sequenced simulation can be reviewed by highlighting the solution of interest on the graph, “RMB > Retrieve Results”.

22. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-22 … Directional Loads For most loads/supports which have an orientation, the direction can be defined by components in any Coordinate System –In the Details view, change “Define By” to “Components”. Then, select the appropriate CS from the pull-down menu. –Specify x, y, and/or z components, which are relative to the selected Coordinate System –Not all loads/supports support use of CS: Loads/Supports not listed in the table do not have direction associated with it, so Coordinate Systems are not applicable.

23. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-23 … Acceleration & Gravity Acceleration: –Acts on entire model in length/time 2 units. –Note, inertial forces are in the opposite direction to applied acceleration –Acceleration can be defined by Components or Vector Standard Earth Gravity: –Value applied is 9.80665 m/s 2 (in SI units) –Standard Earth Gravity direction can only be defined along one of three World Coordinate System axes –“Standard Earth Gravity” is defined as an acceleration. Define the direction opposite to gravitational force

24. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-24 … Rotational Velocity Rotational velocity: –Entire model spins about an axis at a given rate –Define by vector using geometry for axis of rotation –Define by components supplying origin and components in global or local coordinate system –Input can be in radians per second (default) or RPM

25. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-25 … Forces and Pressures Pressure loading: –Applied to surfaces, acts normal to the surface –Positive value into surface, negative value acts out of surface –Units of pressure are in force per area Force loading: –Forces can be applied on vertices, edges, or surfaces. –The force will be evenly distributed on all entities. Units are mass*length/time 2 –Force can be defined via vector or component methods

26. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-26 … Bearing Load Bearing Load (cylindrical surfaces only): –Radial component will be distributed on compressive side using projected area (see below) –Axial component is distributed evenly on cylinder –Use only one bearing load per cylindrical surface. If the cylindrical surface is split be sure to select both halves of cylindrical surface when applying this load. –Load is in units of force –Bearing load can be defined via vector or component method

27. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-27 … Moment Load Moment Load: –For solid bodies, a moment can be applied on any surface –If multiple surfaces are selected, the moment load is evenly distributed –Vector or component method can be used. The moment acts about the vector using the right-hand rule –For surface bodies, a moment can also be applied to a vertex or edge with similar definition –Units of moment are in Force*length.

28. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-28 … Remote Load Remote Load: –applies an offset force on a surface or edge of a surface body –The user supplies the origin of the force (vertices, cylinder or x, y, z coordinates). A user-defined Coordinate System may be used to reference the location. –Can be defined using vector or component method –Applies an equivalent force and moment on the surface –Units are in force (mass*length/time 2 ) Load transfer surface

29. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-29... Bolt Load Bolt Load: –Applies a pretension load to a cylindrical section simulating bolt tightening –Apply pretension load (force) or adjustment (length) as initial condition –For sequenced loading additional options are available (see next page)

30. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-30... Bolt Load For static analyses the preload is applied in an initial solution and external loads are applied in a subsequent solution –Note this 2 step sequence is automatic and transparent The bolt load is automatically locked during the second solution For sequence analyses users may choose to lock or open the bolt load in any load step except the first

31. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-31... Bolt Load Bolt Load Tips: –Can be used only in 3D simulations –Can be applied to cylindrical surfaces or bodies. Bodies require a local coordinate system with the Z axis representing the pretension direction –A refined mesh is recommended (must be more than 1 element along the bolt section)

32. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-32 … Supports (General) Fixed Support: –Constraints all degrees of freedom on vertex, edge, or surface Solid bodies: constrains x, y, and z Surface and line bodies: constrains x, y, z, rotx, roty and rotz Given Displacement: –Applies known displacement on vertex, edge, or surface –Allows for imposed translational displacement in x, y, and z (in user-defined Coordinate System) –Entering “0” means that the direction is constrained. –Leaving the direction blank means that the entity is free to move in that direction

33. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-33 … Supports (Solid Bodies) Frictionless Support: –Applies constraint in normal direction on surfaces –For solid bodies, this support can be used to apply a ‘symmetry’ plane boundary condition since ‘symmetry’ plane is same as normal constraint Cylindrical Constraint: –Applied on cylindrical surfaces –User can specify whether axial, radial, or tangential components are constrained –Suitable for small-deflection (linear) analysis only

34. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-34 … Supports (Solid Bodies) Compression Only Support: –Applies a constraint in the normal compressive direction –Can be used on a cylindrical surface to model a pin (referred to as “Pinned Cylinder” 7.1) –Notice in the example above the outline of the undeformed cylinder is shown. The compressive side retains the shape of the original cylinder, but the tensile side is free to deform. –This requires an iterative (nonlinear) solution.

35. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-35 … Supports (Line/Surface Bodies) Simply Supported: –Can be applied on edge or vertex of surface or line bodies –Prevents all translations but all rotations are free Fixed Rotation: –Can be applied on surface, edge, or vertex of surface or line bodies –Constrains rotations but translations are free

36. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-36 … Thermal Loading Temperature causes thermal expansion in the model –Thermal strains are calculated as follows: where  is the thermal expansion coefficient (CTE), T ref is the reference temperature at which thermal strains are zero, T is the applied temperature, and  th is the thermal strain. –CTE is a material property defined in “Engineering Data” and has units of strain per temperature –The reference temperature is defined in the “Environment” branch

37. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-37 … Thermal Loading Thermal loads: –Any temperature loading can be applied (see Chapter 6 on Thermal Analysis for details) –Simulation will always perform a thermal solution first, then use the calculated temperature field as input when solving the structural solution.

38. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-38 Workshop 4.1 – Linear Structural Analysis Goal: –A 5 part assembly representing an impeller type pump is analyzed with a 100N preload on the belt. D. Workshop 4.1 – Linear Structural Analysis

39. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-39 E. Solution Options Solution options can be set under the “Solution” branch –Save ANSYS db: Useful if you want to open a database in ANSYS –Two solvers are available in Simulation: The “Direct” solver is useful for models containing thin surface and line bodies. It is a robust solver and handles any situation (Sparse solver in ANSYS) The “Iterative” solver is most efficient when solving large, bulky solid bodies. It can handle large models well, although it is less efficient for beam/shells (PCG solver in ANSYS)

40. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-40 … Solution Options –Weak springs can be added to stabilize model If “Program Controlled” is set, Simulation tries to anticipate under- constrained models. If no “Fixed Support” is present, it may add weak springs and provide an informative message letting the user know that it has done so This can be set to “On” or “Off”.

41. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-41 … Solution Options –Solution Information: Analysis Type: Static Structural, thermal, etc Nonlinear solution: indicated when options cause the solution to be nonlinear. These type of solutions require multiple iterations and take longer than linear solutions. Solver Working Directory: –Location where scratch files are saved during solution –Default is the TEMP directory on Windows systems –Can be changed in “Tools > Options … > Simulation: Solution > Solver Working Directory” –Solver Messages: review messagges triggered during the solution by clicking “Solver Messages” field

42. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-42 … Solving the Model To solve the model, request results first (covered next) and click on the “Solve” button on the Standard Toolbar –By default, two processors (if present) will be used for parallel processing. To set the number, use “Tools > Options … > Simulation: Solution > Number of Processors to Use”

43. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-43 F. Results and Postprocessing Various results are available for postprocessing: –Directional and total deformation –Components, principal, or invariants of stresses and strains –Contact output Requires ANSYS Professional and above –Reaction forces In Simulation, results are usually requested before solving, but they can be requested afterwards, too. –If you solve a model then request results afterwards, click on the “Solve” button, and the results will be retrieved. A new solution is not required for linear analyses

44. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-44 … Plotting Results All of the contour and vector plots are usually shown on the deformed geometry. Use the Context Toolbar to change the scaling or display of results to desired settings.

45. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-45 … Deformation The deformation of the model can be plotted: –Total deformation is a scalar quantity: –The x, y, and z components of deformation can be requested under “Directional.” –if a “Coordinate System” branch is present, users can request directional results in a given coordinate system. –Vector plots of deformation are available.

46. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-46 … Deformation Deformation results are available for line, surface, and solid bodies –Because deformation (displacements) are DOF which Simulation solves for, the convergence behavior is well- behaved when using the Convergence tool

47. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-47 … Stresses and Strains Stresses and strains: –Stresses and (elastic) strains have six components (x, y, z, xy, yz, xz) while thermal strains have three components (x, y, z) –For stresses and strains, components can be requested under “Normal” (x, y, z) and “Shear” (xy, yz, xz). For thermal strains, (x, y, z) components are under “Thermal.”

48. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-48 … Stress Tools Safety Factors (choose from 4 failure theories): –Ductile Theories: Maximum Equivalent Stress Maximum Shear Stress –Brittle Theories: Mohr-Coulomb Stress Maximum Tensile Stress –Within each stress tool safety factor, safety margin and stress ratio can be plotted

49. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-49 … Contact Results Contact Results: If asymmetric or auto-asymmetric contact is used, then contact results will be reported on the ‘contact’ surfaces only. The ‘target’ surfaces will report zero values, if requested. If symmetric contact is used, then contact results will be reported on both surfaces. For values such as contact pressure, the actual contact pressure will be an average of both surfaces in contact. –Contact results are first requested via a “Contact Tool” under the Solution branch.

50. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-50 … Contact Results The user can specify contact output under “Contact Tool” –The Worksheet view easily allows users to select which contact regions will be associated with the “Contact Tool” –Results on ‘contact’ or ‘target’ sides (or both) can be selected from the spreadsheet (symmetric vs. asymmetric contact) –Specific contact results chosen from Context Toolbar Select contact regions you want to review (add more “Contact Tool” branches to look at contact region output separately). Right-click on the worksheet to see other available options. For the “Contact Tool”, then request contact output results, and those results will correspond to selected contact regions.

51. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-51 … Contact Results Contact Results: –Pressure: shows distribution of normal contact pressure –Penetration/Gap: shows the resulting amount of penetration or gap (within pinball radius). –Sliding Distance: distance one surface has slid with respect to the other. –Frictional Stress: is tangential contact traction due to frictional effects. –Status: open or closed For the open state, near-field means that it is within pinball region, far-field means that it is outside of pinball region. Contour results are plotted with the rest of the model being translucent for easier viewing.

52. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-52 … Contact Forces Contact Reactions: requested for “Contact Tool”, forces and moments are reported for the requested contact regions –Under the “Worksheet” tab, contact forces for all requested contact regions will be tabulated –Under the “Geometry” tab, symbols will show direction of contact forces and moments.

53. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-53 … Reaction Forces at Supports Reaction forces and moments are output for each support –Reaction forces and moments are shown in the details for each support. X, Y, and Z components are reported with respect to the world coordinate system. Moments are reported at the centroid of the support. –The reaction force for weak springs, if used, are listed under the “Environment” branch Details. The weak spring reaction forces should be small to ensure that the effect of weak springs is negligible.

54. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-54 … Reaction Forces at Supports The “Worksheet” tab for “Environment” branch has a summary of reaction forces and moments –If a support shares a vertex, edge, or surface with another support, contact pair, or load, the reported reaction forces may be incorrect.

55. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-55 … Fatigue If the Fatigue Module add-on license is available, additional post-processing involving fatigue calculations is possible –The “Fatigue Tool” provides stress-based fatigue calculations to aid the design engineer with evaluating the life of components in the system –Constant or variable amplitude loading, proportional or non- proportional loading is possible Damage Matrix at Critical LocationContour of Safety Factor

56. Training Manual Linear Static Structural Analysis August 26, 2005 Inventory #002265 4-56 G. Workshop 4.2 – 2D vs 3D Analysis Workshop 4.2 – Comparing 2D and 3D Structural Analysis Comparing 2D and 3D structural analyses. Shown here are the 3D sector model and the 2D axisymmetric model. Pressure Cap Retaining Ring