1 / 66

ANSYS General Preprocessing Overview

This chapter provides an overview of performing analyses in ANSYS DesignSpace without the use of the Wizards. Topics covered include geometry, contact, meshing, named selections, and coordinate systems.

jbenavidez
Download Presentation

ANSYS General Preprocessing Overview

An Image/Link below is provided (as is) to download presentation Download Policy: Content on the Website is provided to you AS IS for your information and personal use and may not be sold / licensed / shared on other websites without getting consent from its author. Content is provided to you AS IS for your information and personal use only. Download presentation by click this link. While downloading, if for some reason you are not able to download a presentation, the publisher may have deleted the file from their server. During download, if you can't get a presentation, the file might be deleted by the publisher.

E N D

Presentation Transcript

  1. Chapter Three General Preprocessing

  2. Chapter Overview • In this chapter, performing analyses without the use of the Wizards will be covered: • Geometry • Contact • Meshing • Named Selections • Coordinate Systems • 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. August 26, 2005 Inventory #002265 3-2

  3. Introduction • In the previous chapter, the Simulation GUI was introduced by the use of the Simulation Wizards • In this chapter, navigating through the GUI without the Wizards will be covered. August 26, 2005 Inventory #002265 3-3 Model shown is from a sample Mechanical Desktop assembly.

  4. … Introduction • The Outline Tree is the main way of setting up the analysis • The Context Toolbar, Details View, and Graphics Window update, depending on which Outline Tree branch is selected • Use of the Outline Tree will be emphasized in this chapter Use of the Outline Tree is the means by which users navigate through the Simulation GUI. August 26, 2005 Inventory #002265 3-4

  5. A. Geometry Branch • After importing a model either (a) directly from a supported CAD system or (b) from the Context Toolbar in a blank database, the Geometry branch lists available parts. • In Simulation, there are three types of bodies which can be analyzed. • Solid bodies are general 3D or 2D volumes/areas/parts. • Surface bodies are only areas. • Line bodies are only curves. August 26, 2005 Inventory #002265 3-5

  6. … Types of Bodies • Solid bodies are geometrically and spatially 3D or 2D: • 3D solids are meshed with higher-order tetrahedral or hexahedral solid elements with quadratic shape functions • 2D solids are meshed with higher order triangle or quadrilateral solid elements with quadratic shape functions • Currently 2D geometry can be obtained from: • DesignModeler, ProEngineer, Solid Edge, SolidWorks and Unigraphics • Each node has three translational degrees of freedom (DOF) for structural or one temperature DOF for thermal August 26, 2005 Inventory #002265 3-6

  7. … Types of Bodies • Considerations for 2D Geometry: • Geometry must consist of surface models lying on the XY plane • The “2D” switch must be set on the Project page prior to import • Geometry type cannot be changed from 2D to 3D (or vice versa) after import • Plane stress, plane strain and axisymmetric behaviors are supported • Be sure to consult the Simulation documentation for all details regarding 2D analysis August 26, 2005 Inventory #002265 3-7

  8. … 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. • 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 August 26, 2005 Inventory #002265 3-8

  9. … 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 August 26, 2005 Inventory #002265 3-9

  10. … Multibody Parts • For many applications, bodies and parts are the same. In DesignModeler, however, multibody parts are possible. • 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. August 26, 2005 Inventory #002265 3-10

  11. Multibody parts made of surface and line bodies share nodes at common boundaries. This allows modeling of shells with stiffeners. Multibody parts made of solid bodies share nodes at common boundaries. Material properties can be different for each body. … Multibody Parts • Multibody parts allows the user to define bodies with common nodes, as shown below: August 26, 2005 Inventory #002265 3-11

  12. … 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 or imported in the “Engineering Data” application. The new material will then be available from the pull-down menu. • For surface bodies a thickness needs to be supplied as well • Thicknesses will import directlyfrom DesignModeler, if defined. August 26, 2005 Inventory #002265 3-12

  13. … Geometry Worksheet • A summary of bodies and assigned materials is available • Select “Geometry” branch and then the “Worksheet” tab August 26, 2005 Inventory #002265 3-13

  14. 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. August 26, 2005 Inventory #002265 3-14

  15. … Solid Body Contact • When an assembly is imported, contact surfaces are automatically detected and created • The mating relationships are not used from 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” August 26, 2005 Inventory #002265 3-15 Model shown is from a sample SolidWorks assembly.

  16. Note the non-matching mesh at the interface between parts. Mix of hexahedral elements contacting tetrahedral elements is possible. … Solid Body Contact • Contact elements, which act as a ‘skin’ on the surface of the contacting regions, provides the relationship between parts. • Each part maintains a separate mesh. This means that one small part will not drive mesh density of the entire assembly and/or the user can make parts of interest have a finer mesh than other parts August 26, 2005 Inventory #002265 3-16

  17. The contacting bodies are partially transparent. Bodies not in the contact region are more fully transparent. The contacting surfaces which are oriented with surface normals pointing towards the view are opaque for easier viewing. … 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 > Options… > Simulation: Contact: Transparency”. Transparency can be turned off in the Details view of the “Contact” branch August 26, 2005 Inventory #002265 3-17

  18. … 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 August 26, 2005 Inventory #002265 3-18

  19. Selection of contact and target surfaces is performed in the “Details” view. The contact bodies associated with selected surfaces will be listed below. Ensure that unique bodies are for each “Contact” and “Target” body. The “Contact” surfaces will be shown in red while “Target” surfaces will be displayed in blue. … 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 August 26, 2005 Inventory #002265 3-19

  20. … 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. August 26, 2005 Inventory #002265 3-20

  21. When moving the cursor over selection planes, those surfaces will get highlighted. Use of wireframe mode may make visualization easier. One can select a particular surface or even use Ctrl-select to select multiple surfaces. In this example, two surfaces highlighted on the screen are selected to define a contact pair manually. Without selection planes, the selection of the specific surfaces would be tedious. … Selection Planes • The use of selection planes streamlines the identification of contact regions • Example below shows two surfaces selected from two parts. Selection Point August 26, 2005 Inventory #002265 3-21

  22. … Renaming Contact Regions • Select the “Contact” branch and right-click and select “Rename Based on Geometry” to rename all contact pairs based on part names August 26, 2005 Inventory #002265 3-22

  23. In this example, because of the tolerance used by automatic contact detection, some fillets shown here are included in the contact definition. The user may wish to remove the fillets from the contact region definition, especially in the case of bonded contact, in order to prevent spurious behavior. … Verifying Contact Regions • Although Simulation automatically detects contact, one should review each contact pair to ensure that contact is properly defined. August 26, 2005 Inventory #002265 3-23

  24. … Advanced Solid Body Contact • For ANSYS Professional licenses and above, advanced contact options are available. • Auto detection dimension and slider • Asymmetric contact • Contact results tool • More contact formulations available • Pinball control (see next page) August 26, 2005 Inventory #002265 3-24

  25. The pinball region enables the user to verify that contact is detected for a large gap. … Advanced Solid Body Contact • The Pinball region represents a contact detection zone: • Contact calculation/detection occurs when contact gap is within the pinball radius • The pinball radius dimension may be entered to ensure that bonded contact is established for a large clearance or gap • Pinball radius is displayed as a sphere in the graphics window August 26, 2005 Inventory #002265 3-25

  26. . . . 2D Solid Body Contact • Surface contact for solids composed of 2D plane geometry is defined on edges rather than faces August 26, 2005 Inventory #002265 3-26

  27. … Surface Body Contact • For ANSYS Professional licenses and above, mixed assemblies of shells and solids are also supported August 26, 2005 Inventory #002265 3-27

  28. … Surface Body Contact • Shell contact includes edge-to-face or edge-to-edge contact • Shell contact is not turned on by default. • Tolerance controls absolute search distance for detecting contact. Useful 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. August 26, 2005 Inventory #002265 3-28

  29. If needed, use the “Label” button on the Graphical Toolbar to move the “Contact Region” label & pinball sphere to a location which may be more convenient. … 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. • For bonded regions the radius should be set large enough to fill any ‘gap.’ • The default Pinball region is based on the size of the underlying mesh (solid body) or thickness (surface body). August 26, 2005 Inventory #002265 3-29

  30. … Spot Weld • Spot welds provide a means of connecting shell assemblies at discrete points • Spot weld definition is done in the CAD software. Currently, only DesignModeler and Unigraphics define spot welds supported by Simulation • Spot welds can be created in Simulation manually at discrete vertices. August 26, 2005 Inventory #002265 3-30

  31. Right-click on the spreadsheet to hide/show specific columns. … Contact Worksheet • The “Worksheet” tab of the “Contact” branch provides a summary of various contact and spot weld definitions: August 26, 2005 Inventory #002265 3-31

  32. C. Meshing • The nodes and elements of the mesh participate in the finite element solution • 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 • Note: previewing a mesh will create the nodes and elements. A solve following a preview will not require re-meshing. August 26, 2005 Inventory #002265 3-32 Model shown is from a sample Inventor assembly.

  33. … 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! August 26, 2005 Inventory #002265 3-33

  34. Relevance = -100 Nodes: 9968 Elements: 5808 Relevance = 0 Nodes: 19040 Elements: 10909 Relevance = +100 Nodes: 40764 Elements: 24687 … 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 August 26, 2005 Inventory #002265 3-34

  35. … Global Meshing Controls • User can change to “Advanced” global controls • Five options are available to user: • “Element Size” defines average element edge size • “Curv/Proximity” places 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 • Standard: For linear analyses • Aggressive: For nonlinear or field type analyses August 26, 2005 Inventory #002265 3-35

  36. Part-Based Mesh Seeding Nodes: 52,484 Elements: 19,816 (Mesh seeding is based on parts, so less uniform between parts) Assembly-Based Mesh Seeding Nodes: 13,001 Elements: 5,666 (Mesh seeding is more uniform between parts) … Global Meshing Controls • Five options are available to user (cont’d): • “Solid Element Order” allows users to toggle between lower- or higher-order solid elements. • Higher-order solid elements are default • “Initial Size Seed” controls what geometry the mesh seeding is based on August 26, 2005 Inventory #002265 3-36

  37. … Solid Element Shape • The “Method” control provides the user with options as to how solid bodies are meshed: • “Auto Sweep if Possible”: sweeps volumes using brick or wedge shaped elements • “All Tetrahedrons”: meshes all volumes with tetrahedral elements • “Hex Dominant”: attempts to mesh using brick shapes but will contain some pyramid and tet shapes. (only available with ANSYS Structural licenses and above) August 26, 2005 Inventory #002265 3-37

  38. For model shown on right, the solid body in middle is swept-meshed with hexahedral (and pentahedral) elements, whereas other volumes are meshed with tetrahedral elements. … Solid Element Shape • Sweep Meshing: • 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. August 26, 2005 Inventory #002265 3-38

  39. … Local Mesh Controls • Sizing: • “Element Size” specifies average element edge length • “Number of Divisions” specifies number of elements on edge(s) • “Sphere of Influence” elements within the sphere have a given average element size • Available options above depend on which entities are scoped: August 26, 2005 Inventory #002265 3-39

  40. … Local Mesh Controls Scoped to single surface “Sphere of Influence” (shown in red) has been defined. Elements lying in that sphere for that scoped entity will have a given average element size. • Sphere center located using local coordinate system • All scoped entities within sphere are affected by size settings Scoped to 3 surfaces August 26, 2005 Inventory #002265 3-40

  41. In this example, the contact region between the two parts has a Contact Sizing specified (by Element Size). Note that the mesh is now consistent at the contact region. … Local Mesh Controls • Contact Sizing provides a way of generatingsimilar-sized elements on contact faces • An “Element Size” or “Relevance” can be specified for a given contact region August 26, 2005 Inventory #002265 3-41

  42. … Local Mesh Controls • Element refinement divides existing mesh • An ‘initial’ mesh is created with global and local size controls first, then element refinement is performed at the specified location(s). • Refinement level of “1” is recommended. This breaks up the edges of the elements in the ‘initial’ mesh in half. For example shown, the left side has refinement level of 1 whereas the right side is left untouched with default mesh settings. August 26, 2005 Inventory #002265 3-42

  43. … 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. • If surface cannot be mapped mesh for any reason, meshing will continue and this will be shown in Outline Tree with icon: August 26, 2005 Inventory #002265 3-43

  44. … Mapped Face Meshing • Mapped quad or tri mesh also available for surface bodies August 26, 2005 Inventory #002265 3-44

  45. Cut Boundaries Matched Faces Full Model Cyclic Symmetry Model . . . Match Face Meshing • Matches mesh pattern on symmetry faces to facilitate cyclic symmetry analyses typical of rotating machinery • For cyclic symmetry the nodal locations on each cut face must be identical except for the offset (see below) August 26, 2005 Inventory #002265 3-45

  46. . . . Match Face Meshing • Procedure: • Insert “Match Face Meshing” control under Mesh branch • Identify faces of symmetry boundary • Identify the coordinate system (Z axis is rotation axis) Rotation CS August 26, 2005 Inventory #002265 3-46

  47. Part Relevance=+100 Part Relevance=-100 … Local Mesh Controls • Part Relevance allows controlling mesh by parts • Control is given with a slider (-100 to +100) August 26, 2005 Inventory #002265 3-47

  48. Default Mesh Default Mesh w/ Part Proximity … Part Proximity • Part Proximity specifies that the proximity ofsmall lines to each other will affect mesh density • Degree is controlled by global “Relevance” or “Curv/Proximity” August 26, 2005 Inventory #002265 3-48

  49. … Hex-Dominant Meshing • Advanced Structural Meshing introduction: • The hex-dominant meshing algorithm creates a quad-dominant surface mesh first, then pyramid and tetrahedral elements are filled in as needed. • “Hex Dominant” option for the “Element Shape” branch is only available with ANSYS Structural licenses and above • “Control Messages” will appear to warn user if volume may not be suitable for hex-dominant meshing August 26, 2005 Inventory #002265 3-49

  50. … Hex-Dominant Meshing • Example of hex-dominant mesh shown below: • 10,918 brick (39%) • 6,289 tetra (23%) • 907 wedges (3%) • 9,631 pyramids (35%) August 26, 2005 Inventory #002265 3-50

More Related