General Preprocessing

General Preprocessing
Chapter Three General Preprocessing

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. March 29, 2005 Inventory #002215 3-2

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. March 29, 2005 Inventory #002215 3-3 Model shown is from a sample Mechanical Desktop assembly.

… 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. March 29, 2005 Inventory #002215 3-4

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. March 29, 2005 Inventory #002215 3-5

… 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 Good for general representation of CAD models March 29, 2005 Inventory #002215 3-6

… 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 Certain load types are unavailable with 2D geometry Be sure to consult the Simulation documentation for all details regarding 2D analysis March 29, 2005 Inventory #002215 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 March 29, 2005 Inventory #002215 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 thermal March 29, 2005 Inventory #002215 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. For surface bodies, “Surface Extension” and “Joint” operations are also available in DesignModeler to ensure congruent mesh at intersecting surfaces. Check to see if any CAD package supports parts vs. bodies March 29, 2005 Inventory #002215 3-10

… Multibody Parts Multibody parts allows the user to define more complex bodies with common nodes, as shown below: 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. March 29, 2005 Inventory #002215 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 or imported in the “Engineering Data” application. 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 directly from DesignModeler, if defined. March 29, 2005 Inventory #002215 3-12

… Geometry Worksheet A summary of bodies and assigned materials is available Select “Geometry” branch and then the “Worksheet” tab March 29, 2005 Inventory #002215 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. March 29, 2005 Inventory #002215 3-14

… 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” March 29, 2005 Inventory #002215 3-15 Model shown is from a sample SolidWorks assembly.

… 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 Note the non-matching mesh at the interface between parts. Mix of hexahedral elements contacting tetrahedral elements is possible. March 29, 2005 Inventory #002215 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 > Options… > Simulation: Contact: Transparency”. Transparency can be turned off in the Details view of the “Contact” branch 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. March 29, 2005 Inventory #002215 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 March 29, 2005 Inventory #002215 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 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. March 29, 2005 Inventory #002215 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. March 29, 2005 Inventory #002215 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 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. March 29, 2005 Inventory #002215 3-21

… Renaming Contact Regions
Select the “Contact” branch and right-click and select “Rename Based on Geometry” to rename all contact pairs, based on their constituent parts, for easier readability. March 29, 2005 Inventory #002215 3-22

… Verifying Contact Regions
Although Simulation automatically detects contact, one should review each contact pair to ensure that contact is properly defined. 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. March 29, 2005 Inventory #002215 3-23

… 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). March 29, 2005 Inventory #002215 3-24

… 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. The pinball region enables the user to verify that contact is detected for a large gap. March 29, 2005 Inventory #002215 3-25

D Solid Body Contact Surface contact for solids composed of 2D plane geometry is defined on edges rather than faces March 29, 2005 Inventory #002215 3-26

… Surface Body Contact For ANSYS Professional 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 ANSYS Professional will support 175 at 8.1. March 29, 2005 Inventory #002215 3-27

… Surface Body Contact Shell contact includes edge-to-face or edge-to-edge contact Shell contact is not turned on by default. However, default behavior can be changed under “Tools menu > Options … > Simulation: Contact: Auto Detection” Activate automatic shell contact detection under the “Contact” branch Tolerance controls include ability to input absolute 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 contact regions from being formed in a given region by setting priority. March 29, 2005 Inventory #002215 3-28

… 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. If “Pinball Region: Radius” is input under the Details view, the pinball region is shown graphically as a sphere. For bonded regions, the radius should be large enough to fill any ‘gap.’ Pinball region, by default, is based on the size of the underlying mesh (solid body) or thickness (surface body). 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. March 29, 2005 Inventory #002215 3-29

… Spot Weld Spot welds provide a means of connecting shell assemblies at discrete points For ANSYS DesignSpace 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 Simulation supports. Spotwelds can also be created in Simulation manually, but only at discrete vertices. March 29, 2005 Inventory #002215 3-30

… 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 March 29, 2005 Inventory #002215 3-31

… Contact Worksheet The “Worksheet” tab of the “Contact” branch provides a summary of various contact and spot weld definitions: Right-click on the spreadsheet to hide/show specific columns. March 29, 2005 Inventory #002215 3-32

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 Panel March 29, 2005 Inventory #002215 3-33 Model shown is from a sample Inventor assembly.

… 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! March 29, 2005 Inventory #002215 3-34

… 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” Relevance = -100 Nodes: 9968 Elements: 5808 Relevance = 0 Nodes: 19040 Elements: 10909 Relevance = +100 Nodes: 40764 Elements: 24687 March 29, 2005 Inventory #002215 3-35

User can change to “Advanced” global controls Five options are 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 Simulation to put more elements near curvature or proximity of edges to each other Set slider bar from –100 to If “Element Size” left to “Default”, “Curv/Proximity” behaves the same as “Relevance” The “Proximity” of lines to each other is accounted for sweepable bodies or if “Part Proximity” branches are added (discussed later) “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”) March 29, 2005 Inventory #002215 3-36

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 Lower-order tetrahedral elements should not be used for structural analyses, as these result in constant strain tets (stiff behavior). Lower-order solid elements should not be requested with Hex-Dominant meshing (discussed later) for structural and thermal analyses since lower-order pyramids are not supported. This option not supported for Shape Optimization analyses “Initial Size Seed” controls what the mesh seeding is based on Assembly-Based Mesh Seeding Nodes: 13,001 Elements: 5,666 (Mesh seeding is more uniform between parts) Part-Based Mesh Seeding Nodes: 52,484 Elements: 19,816 (Mesh seeding is based on parts, so less uniform between parts) March 29, 2005 Inventory #002215 3-37

… Local Mesh Controls Part Relevance allows controlling mesh by parts
“Part Relevance” is similar to the “Basic” global mesh control except it is for selected parts Control is given with a slider (-100 to +100) Part Relevance=+100 Part Relevance=-100 March 29, 2005 Inventory #002215 3-38

… Local Mesh Controls Sizing allows for local element size specification An average element size, sphere of influence, or number of divisions per edge can be specified “Element Size” produces elements with specified average edge length “Number of Divisions” puts specified number of elements on edge(s) “Sphere of Influence” allows specification of a ‘sphere,’ where elements lying in sphere have a given average element size Sizing enables users to specify local mesh densities which are finer or coarser than global average element size Available options above depend on which entities are scoped: March 29, 2005 Inventory #002215 3-39

… Local Mesh Controls For the example on right, the left side has initial “Element Size” whereas the right size is left with default mesh settings. Note that the left side with sizing controls has a relatively uniform mesh density of the specified edge length. In the adjacent example, a “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. A surface (purple) has the sizing, so elements on the surface in the sphere of influence will have the average element size. March 29, 2005 Inventory #002215 3-40

… Local Mesh Controls Contact Sizing provides a way of generating similar-sized elements on contact faces Because contact regions define the interaction between parts, it may be preferred to have similar mesh densities between contact region surfaces An “Element Size” or “Relevance” can be specified for a given contact region 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. March 29, 2005 Inventory #002215 3-41

… Local Mesh Controls Element refinement divides existing mesh
Although transparent to the user, an ‘initial’ mesh is 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. For example shown, the left side has refinement level of 1 whereas the right side is left untouched with default mesh settings. Note that the refined mesh is not uniform since the original mesh is not uniform. The refined mesh breaks element edges in half. March 29, 2005 Inventory #002215 3-42

… 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). March 29, 2005 Inventory #002215 3-43

… Mapped Face Meshing Mapped Face Meshing allows for the generation of structured meshes on surfaces: In example below, mapped face meshing on the internal cylindrical face provides a more uniform mesh 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: March 29, 2005 Inventory #002215 3-44

… 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.) March 29, 2005 Inventory #002215 3-45

… Solid Element Shape By default, Simulation determines how to mesh solid bodies: Sweep-meshable volumes will have hex (and possible wedge) elements. Other volumes will be 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. 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. March 29, 2005 Inventory #002215 3-46

… Solid Element Shape The “Element Shape” branch provide the user with control over how selected solid bodies are meshed: “Auto Sweep if Possible” lets Simulation mesh sweepable volumes with hexahedra (and possibly also pentahedra) “All Tetrahedrons” lets Simulation mesh all volumes with tetrahedras “Hex Dominant” only appears with ANSYS Structural licenses and above March 29, 2005 Inventory #002215 3-47

. . . Match Face Meshing Matches mesh pattern on symmetry faces to facilitate cyclic symmetry analyses typical of rotating machinery Because cyclic symmetry employs constraint equations linking each cut boundary the nodal locations on each face must be identical except for the offset (see below) Cut Boundaries Full Model Cyclic Symmetry Model Matched Faces March 29, 2005 Inventory #002215 3-48

. . . 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 March 29, 2005 Inventory #002215 3-49

… Hex-Dominant Meshing
Advanced Structural Meshing introduction: 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 ANSYS Structural license and above “Control Messages” will appear to warn user if volume may not be suitable for hex-dominant meshing March 29, 2005 Inventory #002215 3-50

Example of hex-dominant mesh shown below: 10,918 brick (39%) 6,289 tetra (23%) 907 wedges (3%) 9,631 pyramids (35%) Use macro March 29, 2005 Inventory #002215 3-51

In some cases, such as for hex-dominant meshing, it may be useful to use FE Modeler to determine the number of degenerate elements which may be present Select the top-most “[Project]” tab. Open an Environment in FE Modeler Selecting “Element Types” on the left menu provides a listing of the number of tetra, penta, hexa, and wedge elements present in the model. The user can also see where these elements are in the mesh. March 29, 2005 Inventory #002215 3-52

Default Mesh w/ Part Proximity
Part Proximity specifies that the proximity of small lines to each other will affect mesh density Useful for thin parts or for parts where features of interest are close to each other Sweepable volumes always have proximity on Degree controlled by global “Relevance” or “Curv/Proximity” Default Mesh Default Mesh w/ Part Proximity March 29, 2005 Inventory #002215 3-53

… 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. March 29, 2005 Inventory #002215 3-54

… Meshing Failures In the “ Tools menu > Options … > Simulation: 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. March 29, 2005 Inventory #002215 3-55

… 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 March 29, 2005 Inventory #002215 3-56

… 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. March 29, 2005 Inventory #002215 3-57

… Virtual Topology When creating virtual cells, select surfaces first, then add a virtual cell: One cannot add a blank “Virtual Cell” branch because the surfaces to be joined need to be evaluated beforehand. Only after 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. A “Model” branch containing a “Virtual Topology” branch cannot be duplicated or copied March 29, 2005 Inventory #002215 3-58

… Virtual Topology Example
Consider the example below: The small chamfer causes a finer elements near cylindrical area. Virtual cell (red) of two surfaces (top surface and chamfer surface) created Original model contains a small cylindrical surface, which forms the chamfer Resulting mesh is not driven by small features anymore. March 29, 2005 Inventory #002215 3-59

… 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. On the right, the higher-order element’s edge is shown as a solid yellow line. The contour of the original chamfer and top surface is shown as a dotted blue line. The midside node of the element is projected onto the top surface, but the chamfer representation is no longer present because no nodes lie on the boundary between the chamfer and top surface. March 29, 2005 Inventory #002215 3-60

… Virtual Topology Typical error messages which may be encountered:
Surface normals differ significantly, preventing creation of virtual cell: More than one surface needs to be selected: Adjacent surfaces need to be selected: Virtual cells containing other virtual cells cannot be created: March 29, 2005 Inventory #002215 3-61

… 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 March 29, 2005 Inventory #002215 3-62

D. Named Selections The Named Selection Toolbar provides functionality for grouping together geometric entities: Named Selections allow users to group together vertices, edges, surfaces, or bodies together Named Selections can be used to select items for certain branches that require geometry selection in Details view: Defining mesh controls Applying loads and supports Use of Named Selections makes it easy for the user to reselect groups that are referenced often for other tasks as well Defining contact regions Scoping results Create Defined Names Manipulate Show/Hide Supress/Unsuppress March 29, 2005 Inventory #002215 3-63

… Defining Named Selections
To create Named Selections: Simply select the vertices, edges, surfaces, or bodies of interest, then click on the “Create Selection Group” icon. A dialog box will appear, and a name can be given to the newly created Named Selection. The newly created Named Selection will appear in the Named Selection Toolbar as well as in the Outline Tree Please note the following: Only one type of entity can be in a particular Named Selection. For example, vertices and edges cannot exist in the same Named Selection. Named Selection groups can be imported from some CAD systems (see Chapter 10) March 29, 2005 Inventory #002215 3-64

… Using Named Selections (1)
Specifically for mesh controls and loads/supports, Named Selections can be referenced directly: First, make sure the applicable types of bodies are created in a Named Selection In the Details view, change “Method” from “Geometry Selection” to “Named Selection” Select the “Named Selection” from the pull-down menu Simulation will filter non-applicable types of Named Selections. For example, if the mesh control or load/support can only be applied on surfaces, only Named Selections containing surfaces will appear in the pull-down menu. March 29, 2005 Inventory #002215 3-65

… Using Named Selections (2)
Named Selections can also be used in other situations where geometry must be picked in the Details view: Select “Geometry” from the Details view to enter picking mode Toggle the Named Selection to select from the Toolbar From the “Selection” icon, select the applicable choice “Select Items in Group” selects the current Named Selection “Add to Current Selection” adds the current Named Selection to any entities already selected “Remove from Current Selection” removes any currently selected entity which belongs to the referenced Named Selection Then, click on “Apply” in the Details view 1 2 3 March 29, 2005 Inventory #002215 3-66

… Named Selections and Bodies
The associated bodies of a Named Selection group can be hidden or suppressed: This functionality makes it easier to hide or show certain groups of bodies rather than needing to select the bodies from the Geometry branch to change their visibility status If surface Named Selections are hidden, the associated bodies will be hidden graphically. Show/hide and Suppress/Unsuppress functionality work on bodies, not individual lines or surfaces. March 29, 2005 Inventory #002215 3-67

E. Coordinate Systems The Coordinate Systems branch is usually not displayed by default, but it can be added from the Model tree Coordinate systems are currently used for “Sphere of Influence” mesh controls, “Point Mass” (discussed later), direction loads, and results postprocessing. Coordinate systems allow users to specify directions or origins other than global Cartesian. After adding Coordinate Systems branch, the “Global Coordinate System” will be added, based on the origin of the CAD model. Coordinate Systems can be imported from some CAD systems (see Chapter 10) March 29, 2005 Inventory #002215 3-68

… Coordinate Systems New Coordinate Systems can be defined by selecting “Coordinate System” icon from the Context toolbar By changing “Type” in the Details view, a coordinate system can be cartesian or cylindrical. Local coordinate systems can be defined by selecting a vertex for the origin or by selecting a cylinder. The orientation can then be changed by selecting “X/Y/Z Direction” and selecting an appropriate surface to define the direction Recall that flipping the direction can be done in the Graphics window after selecting a surface. March 29, 2005 Inventory #002215 3-69

… Coordinate Systems If the Coordinate Systems branch is present, the defined coordinate systems will be available from the applicable pull-down menu in the Details view Sizing w/ Sphere of Influence Option Force Load (Directional Load) Point Mass Directional Results March 29, 2005 Inventory #002215 3-70

F. Workshop 3 Workshop 3 – Mesh Control Goal:
Use the various DS mesh controls to enhance the mesh for the crankshaft model. March 29, 2005 Inventory #002215 3-71

General Preprocessing

Similar presentations

Presentation on theme: "General Preprocessing"— Presentation transcript:

Similar presentations

About project

Feedback

Log in

Auth with social network:

General Preprocessing

Similar presentations

Presentation on theme: "General Preprocessing"— Presentation transcript:

Similar presentations

About project

Feedback