General Preprocessing

1. General Preprocessing Chapter Three

2. February 2, 2004 Inventory #002010 3-2 Chapter Overview In this chapter, performing analyses without the use of the Wizards will be covered: Geometry Contact Meshing The capabilities described in this section are generally applicable to the ANSYS DesignSpace Entra licenses and above and are noted in the lower-left hand tables.

3. February 2, 2004 Inventory #002010 3-3 Introduction In the previous chapter, the Design Simulation GUI was introduced by the use of the Simulation Wizards In this chapter, navigating through the GUI without the Wizards will be covered.

4. February 2, 2004 Inventory #002010 3-4 � Introduction The Outline Tree is the main way of setting up the analysis The Context Toolbar and the Details View update depending on what branch of the Outline Tree is selected Use of the Outline Tree will be emphasized in this chapter

5. February 2, 2004 Inventory #002010 3-5 A. Geometry Branch After importing a model either (a) directly from a supported CAD system or (b) from the Workbench Projects Page, the Geometry branch lists available parts. In Design Simulation, there are three types of bodies which can be analyzed. Solid bodies are general 3D volumes/parts. Surface bodies are only areas. Line bodies are only curves.

6. February 2, 2004 Inventory #002010 3-6 � Types of Bodies Solid bodies are geometrically and spatially 3D: These are meshed with higher-order tetrahedral or hexahedral solid elements with quadratic shape functions Each node has three translational degrees of freedom (DOF) for structural or one temperature DOF for thermal Good for general representation of CAD models

7. February 2, 2004 Inventory #002010 3-7 � Types of Bodies Surface bodies are geometrically 2D but spatially 3D: Surface bodies are meant to represent structures which are thin in one dimension (through-thickness), so that thickness is not explicitly modeled but supplied as an input value. For example, mid-surfaces extracted in the CAD software could be used, but the �sheet metal� or �shelled� parts are still 3D and are not considered surface bodies. Consequently, if a �sheet metal� or �shelled� part is to be analyzed as a surface body, the midsurface needs to be extracted first in the CAD system. Surface bodies are meshed with linear shell elements Each node has three translational and three rotational DOF for structural applications but one temperature DOF for thermal Efficient for representation of thin sheet-like parts Verify: MDT doesn�t support surface bodies? Surface bodies ARE supported in thermalVerify: MDT doesn�t support surface bodies? Surface bodies ARE supported in thermal

8. February 2, 2004 Inventory #002010 3-8 � Types of Bodies Line bodies are geometrically 1D but spatially 3D: Line bodies are meant to represent structures which are thin in two dimensions compared to the length, so the cross-section is not explicitly modeled. Currently, only DesignModeler supports creation of line bodies since it can define cross-sections and orientations of lines. Line bodies are modeled with linear beam elements Each node has three translational and three rotational DOF for structural analysis and one temperature DOF for thermal Good for representation of beam-like structures Line bodies are supported in thermalLine bodies are supported in thermal

9. February 2, 2004 Inventory #002010 3-9 � Multibody Parts For many applications, bodies and parts are the same. In DesignModeler, however, multibody parts are possible. In some CAD systems, multiple bodies in a single part is supported for import. However, these do not import as a single multibody part. The difference is that each body will be independently meshed. Support of mixed surface and solid bodies in the same part is not supported for most CAD systems. An assembly may contain surfaces and solids, but a single part cannot. In DesignModeler, multiple bodies can be joined together to form a multibody part. This means that if the parts share common boundaries, the nodes are shared at that interface. No contact is needed in these situations if the nodes are shared. Check to see if any CAD package supports parts vs. bodiesCheck to see if any CAD package supports parts vs. bodies

10. February 2, 2004 Inventory #002010 3-10 � Multibody Parts Multibody parts allows the user to define more complex bodies with common nodes, as shown below:

11. February 2, 2004 Inventory #002010 3-11 � Material Properties To assign material properties to a body, select that body from the tree and select a �Material� from the pull-down menu Materials can be selected from external XML files New material data can be added and input under the �Engineering� branch. The new material will then be available from the pull-down menu. For surface bodies, as noted earlier, a thickness needs to be supplied as well Thicknesses will import directlyfrom DesignModeler, if defined.

12. February 2, 2004 Inventory #002010 3-12 � Geometry Worksheet A summary of bodies and assigned materials is available Select �Geometry� branch and then the �Worksheet� tab

13. February 2, 2004 Inventory #002010 3-13 B. Contact When multiple parts are present, a means of defining the relationship between parts is needed. Contact regions define how solid and/or shell parts interact with each other. Spot welds provide a means of defining shell assemblies. Without contact or spot welds, parts will not interact with each other In structural analyses, contact and spot welds prevent parts from penetrating through each other and provide a means of load transfer between parts. In thermal analyses, contact and spot welds allow for heat transfer across parts. Contact will be introduced first, then spot welds.

14. February 2, 2004 Inventory #002010 3-14 � Solid Body Contact When an assembly is imported, contact surfaces are automatically detected and created The mating relationships are not used in the CAD software. Proximity of surfaces is used instead to define contact. Tolerance for contact detection is available under the �Contact� branch as a slider bar in �Tolerance Slider�

15. February 2, 2004 Inventory #002010 3-15 � Solid Body Contact Proven ANSYS Contact Technology allows the user to model without shared nodes between parts Contact elements, which act as a �skin� on the surface of the contacting regions, provides the relationship between parts. This means that one small part will not drive mesh density of the entire assembly. The user can make parts of interest have a finer mesh than other parts

16. February 2, 2004 Inventory #002010 3-16 � Solid Body Contact When a contact region is highlighted in the �Contact� branch, parts are made translucent for easier viewing Selecting a contact pair makes the other bodies not involved in that contact region translucent Amount of translucency is controlled via �Tools > Control Panel > Contact: Transparency�. Transparency can be turned off in the Details view of the �Contact� branch

17. February 2, 2004 Inventory #002010 3-17 � Solid Body Contact If a geometric entity is highlighted, use right-mouse button in the Graphics window to quickly select associated contact The right-mouse pop-up menu allows the user to select the corresponding body in the �Geometry� branch or highlight all associated contact regions under the �Contact� branch

18. February 2, 2004 Inventory #002010 3-18 � Solid Body Contact Defining a contact pair involves selecting �contact� and �target� surfaces. In ANSYS DesignSpace, the distinction between �contact� and �target� is unimportant. Select surfaces for one body as �contact� and choose the surfaces for the other as �target�. Using �Contact� from the Context Toolbar allows manual definition of contact regions

19. February 2, 2004 Inventory #002010 3-19 � Selection Planes Selection planes allow for users to easily select surfaces which are hidden from view by other surfaces. User selects a plane; if more planes lie directly underneath the cursor, selection planes appear. Selection planes are color-coded with the same color as its parent part and are ordered by depth from the cursor.

20. February 2, 2004 Inventory #002010 3-20 � Selection Planes Through the use of selection planes, users can define contact regions more easily Example below shows two surfaces selected from two parts. A contact region can be defined manually with these surfaces

21. February 2, 2004 Inventory #002010 3-21 � Advanced Solid Body Contact For ANSYS Professional licenses and above, advanced contact options are available. Auto detection of contact surfaces supports entering value rather than just using a slider Specification of asymmetric contact possible Postprocessing contact results possible For each contact region, changing contact formulations, etc. possible, including entering & visualizing pinball radius (discussed next).

22. February 2, 2004 Inventory #002010 3-22 � Advanced Solid Body Contact Example of the use of the pinball region: The pinball radius may be entered to ensure that bonded contact is established for a large clearance or gap In the example below, the visualization of the pinball region enables the user to verify that the pinball region covers the gap between the hole and shaft.

23. February 2, 2004 Inventory #002010 3-23 � Surface Body Contact For ANSYS Professional1 licenses and above, mixed assemblies of shells and solids are also supported Allows for more complex modeling of assemblies, taking advantage of the benefits of shells, when applicable More contact options are exposed to the user Contact postprocessing is also available ANSYS Professional license does not support 175 at 8.0. ANSYS Professional will support 175 at 8.1.ANSYS Professional license does not support 175 at 8.0. ANSYS Professional will support 175 at 8.1.

24. February 2, 2004 Inventory #002010 3-24 � Surface Body Contact Shell contact includes edge-to-face or edge-to-edge contact Shell contact is not turned on by default. Activate automatic shell contact detectionunder the �Contact� branch Tolerance controls include ability to inputabsolute search distance to detect contact,very important for shell assemblies with gaps. User can turn on detection of face-to-edge or edge-to-edge contact Priority can be set to prevent multiple contactregions from being formed in a given regionby setting priority.

25. February 2, 2004 Inventory #002010 3-25 � Surface Body Contact Another example of the use of the pinball region is below: Surfaces represent midplanes of thin structure. At the �T� intersection of two shells, a gap is present If the pinball region is large enough, bonded contact can be established between the shells despite the gap. Too large of a value makes the solution inefficient, however. Pinball region is shown graphically as a sphere with radius input under Details view, �Pinball Region: Radius� value. Pinball should be large enough to �fill gap� between surfaces. Pinball region, by default, is determined by the value used for tolerance of auto-contact detection

26. February 2, 2004 Inventory #002010 3-26 � Spot Weld Spot welds provide a means of connecting shell assemblies at discrete points For ANSYS DesignSpace and ANSYS Professional licenses, shell contact is not supported, so spotwelds are the only way to define a shell assembly. Spotweld definition is done in the CAD software. Currently, only DesignModeler and Unigraphics define spotwelds in a manner that Design Simulation supports. Spotwelds can also be created in Design Simulation manually, but only at discrete vertices.

27. February 2, 2004 Inventory #002010 3-27 � Contact Options The different contact options will be covered in detail in later chapters: In structural analysis, contact elements allow for various interactions between parts In thermal analysis, contact elements allow for heat transfer and thermal contact resistance between parts

28. February 2, 2004 Inventory #002010 3-28 � Contact Worksheet The �Worksheet� tab of the �Contact� branch provides a summary of various contact and spot weld definitions:

29. February 2, 2004 Inventory #002010 3-29 C. Meshing The nodes and elements of the mesh participate in the finite element solution The solid model geometry is meshed, and the resulting mesh is solved in the matrix equation. A �default� mesh is automatically generated during initiation of the solution The user can �preview� the mesh to check whether it is adequate or not for his/her needs. Talk about meshing options in Control PanelTalk about meshing options in Control Panel

30. February 2, 2004 Inventory #002010 3-30 � Meshing The user needs to balance the computational cost with the numerical accuracy of the mesh A finer mesh produces more precise answers but also increases CPU time and memory requirements Ideally, having a solution not dependent on the mesh density is what users want (i.e., answers do not change appreciably as mesh is refined) Convergence controls (discussed later) aid in this A finer mesh does not compensate for incorrect assumptions and inputs, however!

31. February 2, 2004 Inventory #002010 3-31 � Global Meshing Controls Basic meshing controls are available under the �Mesh� branch With �Global Controls� as �Basic� (default), user has control with a single slider bar �Relevance� setting between �100 and +100 Default Relevance is set to 0 but can be changed in �Tools > Control Panel > Meshing: Relevance�

32. February 2, 2004 Inventory #002010 3-32 � Global Meshing Controls User can change to �Advanced� global controls Four main options available to user: �Element Size� defines average element edge size One way to determine this is to use the �edge� selection filter and select a representative edge (like thickness of a rib) to use �Curv/Proximity� tells Design Simulation to put more elements near curvature or proximity of edges to each other Set slider bar from �100 to +100. If �Element Size� left to �Default�, �Curv/Proximity� behaves the same as �Relevance� �Shape Checking� defines element shape quality tests used For linear analysis, �Standard� is suitable. For nonlinear analysis or field analyses, stricter tests may be needed (�Aggressive�) �Solid Element Order� allows users to toggle between lower- or higher-order (default) solid elements. Not supported for Shape Optimization analyses

33. February 2, 2004 Inventory #002010 3-33 � Global Meshing (ANSYS Details) Comparisons of meshing in Design Simulation and ANSYS: Global �Element Size� is similar to ESIZE The �Curv/Proximity� setting in Design Simulation is somewhat similar to SMRTSIZE meshing in ANSYS Both consider curvature and proximity of curves Meshing behavior produces different results, however, so these two settings are not exactly the same The �Shape Checking� toggle is SHPP,LSTET,ON Use of Jacobian tests at integration points is the �Standard� or SHPP,LSTET,ON method, suitable for linear analyses Use of Jacobian tests at corner nodes is the �Aggressive� or SHPP,LSTET,OFF method. This is generally a more conservative approach and may be preferred for nonlinear analyses. This is because elements which undergo distortion during solution should have a good quality shape to begin with. Because Design Simulation uses its own criteria for shape tests, SHPP,OFF is set when exporting a mesh to ANSYS.

34. February 2, 2004 Inventory #002010 3-34 � Local Mesh Controls Sizing allows for local element size specification For sizing, specify average element size onselected edges, surfaces, or parts For edges, users can also specify number ofdivisions along length instead Sizing enables users to specify a relatively uniform mesh density which is finer or coarser than global edge length

35. February 2, 2004 Inventory #002010 3-35 � Local Mesh Controls Element refinement divides existing mesh Although transparent to the user, an �initial� meshis created with global and local size controls first,then element refinement is performed on the specified vertices, edges, or surfaces. Refinement level of �1� is recommended. This breaks up the edges of the elements in the �initial� mesh in half. Refinement is an easy way to get a finer mesh in areas of interest after generating a coarse mesh.

36. February 2, 2004 Inventory #002010 3-36 � Local Mesh Controls There is considerable difference between using sizing and refinement Sizing puts constraints on the mesh on the average element edge length prior to meshing. Generally speaking, this produces a uniform mesh on specified geometric entities, and the mesh transition is smoother. Refinement breaks elements after an �initial� mesh. If the original mesh is non-uniform, the refined mesh will be non-uniform, also. Refinement also leads to less smooth transitions, although a smoothing algorithm is used. Sizing and refinement controls can be specified on the same surface. Sizing will occur first during the �initial� mesh, then it will be refined in the second pass during meshing (all transparent to the user).

37. February 2, 2004 Inventory #002010 3-37 � Mapped Face Meshing Mapped Face Meshing allows for the generationof structured meshes on surfaces: In example below, mapped face meshing on theinternal cylindrical face provides a more uniformmesh pattern. This may be useful to provide better resolution If surface cannot be mapped mesh for any reason, meshing will continue and this will be shown in Outline Tree with icon:

38. February 2, 2004 Inventory #002010 3-38 � Mapped Face Meshing Mapped quad or tri mesh also available for surface bodies A surface can be mapped meshed with quadrilateral or triangular elements. (It is not recommended to use triangular shell elements whenever possible due to accuracy reasons.)

39. February 2, 2004 Inventory #002010 3-39 � Solid Body Meshing By default, Design Simulation determines how to mesh solid bodies: Sweep-meshable volumes will have hex (and possible wedge) elements. Other volumes willbe meshed with tet elements. Sweep-meshing is done in cases where a volume has the same topology in one direction. Right-click on �Mesh� branch gives user ability to see what volumes may be �swept� with �Preview Sweep�. Sweepable solid bodies will be selected.

40. February 2, 2004 Inventory #002010 3-40 � Solid Body Meshing The �Element Shape� branch provide the userwith control over how selected solid bodies aremeshed: �Auto Sweep if Possible� lets Design Simulation mesh sweepable volumes with hexahedra (and possibly also pentahedra). �All Tetrahedrons� lets Design Simulation mesh all volumes with tetrahedras. �Hex Dominant� only appears if the Advanced Meshing Module add-on license is available (introduced next).

41. February 2, 2004 Inventory #002010 3-41 � Hex-Dominant Meshing Advanced Meshing Module introduction: In some instances, users may wish to generate a hex-dominant mesh for certain analyses. The hex-dominant meshing algorithm creates a quad-dominant surface mesh first, then extrudes those bricks/wedges inward. Pyramid and tetrahedral elements are then filled in. This generally results in hexahedral elements on the outside and tetrahedral elements on the inside, which is preferred. As noted in the previous slide, the �Hex Dominant� option for the �Element Shape� branch is only available with the Advanced Meshing Module add-on license. �Control Messages� will appear to warn user if volume may not be suitable for hex-dominant meshing

42. February 2, 2004 Inventory #002010 3-42 � Hex-Dominant Meshing Example of hex-dominant mesh shown below: 14,402 brick (40%) 6,674 tetra (20%) 955 wedges (3%) 10957 pyramids (33%) Use macroUse macro

43. February 2, 2004 Inventory #002010 3-43 � Local Meshing (ANSYS Details) Internally, the following is used: �Sizing� is similar to LESIZE, AESIZE �Refinement� is similar to KREFINE, LREFINE, AREFINE �Mapped Face Meshing� is similar to MSHKEY,1 with appropriate MSHAPE setting �Element Shape� is similar to using VMESH (free) or VSWEEP. Hex-dominant meshing capabilities are not present in ANSYS. Note that some lower-order element types (e.g., SOLID45) do not support pyramid shape. If hex-to-tet transitions (multibody parts) or the hex-dominant meshing (Adv. Struct. Meshing Module) is used, do not set to lower-order elements in �Meshing� branch Use of an APDL macro (example �sortelem.mac� supplied) will allow ANSYS users to check number of hexa, tetra, penta, or pyramid elements generated from hex-dominant meshing

44. February 2, 2004 Inventory #002010 3-44 � Meshing Failures If the mesher is not able to generate well-shaped elements, an error message will be returned: The problematic geometry will be highlighted on the screen, and a named selection group �Problematic Geometry� will be created, so the user may review the model.

45. February 2, 2004 Inventory #002010 3-45 � Meshing Failures In the � Tools menu > Control Panels: Meshing,� some default options can be set Changing �Unmeshable Areas� to �Show All Failed� allows users to change the meshing behavior such that, if problematic geometry exists (previous slide), the mesher will continue to find all problematic geometry that failed to mesh instead of stopping after the first problematic geometry it may encounter.

46. February 2, 2004 Inventory #002010 3-46 � Meshing Failures Meshing failures can be caused by a number of things: Inconsistent sizing controls specified on surfaces, which would result in the creation of poorly-shaped elements Difficult CAD geometry, such as small slivers or twisted surfaces Stricter shape checking (�Aggressive� setting in Mesh branch) Some ways to avoid meshing failures: Specify more reasonable sizing controls on geometry Specify smaller sizing controls to allow the mesher to create better-shaped elements In the CAD system, use hidden line removal plots to see sliver or unwanted geometry and remove them Use virtual cells to combine sliver or very small surfaces This option will be discussed next

47. February 2, 2004 Inventory #002010 3-47 � Virtual Topology Virtual Topology allows users to combine surfaces for the purposes of meshing �Virtual Topology� branch not added by default. Can add the branch from Context Toolbar under �Model� branch A �Virtual Cell� is a surface defined by multiple adjacent surfaces. Select surfaces first, then add �Virtual Cell� Virtual cells enable users to combine sliver surfaces to larger surfaces for the purposes of meshing. Small sliver surfaces will not drive mesh density or possibly cause meshing failures Interior lines of original surfaces belonging to a virtual cell will no longer be honored by meshing process. Because of this, topology of mesh may differ slightly from original geometry. For other operations (such as applying Loads and Supports), individual surfaces are no longer recognized, and virtual cell is referenced instead.

48. February 2, 2004 Inventory #002010 3-48 � Virtual Topology When creating virtual cells, select surfaces first, then add a virtual cell: One cannot add a �Virtual Cell� branch first because Design Simulation must evaluate the surfaces to be joined to verify if the process can be completed. Only after Design Simulation determines that surfaces can be joined will a new Virtual Cell branch be created. When a virtual cell is added, the entities cannot be changed Details View will show the �Geometry� field as grey (unmodifiable) Since surfaces need to be evaluated before the virtual cell is defined, the surfaces cannot be changed afterwards If a virtual cell needs to be changed, delete the existing branch, select the new surfaces, then add a new Virtual Cell branch.

49. February 2, 2004 Inventory #002010 3-49 � Virtual Topology Example Consider the example below:

50. February 2, 2004 Inventory #002010 3-50 � Virtual Topology Example Keep in mind that topology changes slightly, however! Because chamfer is added to top surface in virtual cell, the interior lines are not recognized anymore. Because of this, the position of the mesh is slightly lower than originally expected, and the topology changes slightly.

51. February 2, 2004 Inventory #002010 3-51 � Virtual Topology Virtual cells provide the user with another set of tools to aid in controlling the mesh Use of virtual cells is useful in the following cases: Reducing mesh density in certain areas by eliminating small features Avoiding mesh failure problems by eliminating problematic geometry such as slivers or very tiny surfaces However, care should be taken when using virtual cells since virtual cells change the original topology: Internal features cannot be referenced anymore for such items as loads, supports, or results scoping Some problems may be encountered with meshing because of the new topology

52. February 2, 2004 Inventory #002010 3-52