1 / 59

Meshing

Module 10. Meshing. Meshing Overview. Recall that meshing is a three-step procedure: Define element attributes Specify mesh controls Generate the mesh In this chapter, we will expand on each of these steps and also discuss additional meshing options. Topics covered:

dunne
Download Presentation

Meshing

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. Module 10 Meshing

  2. MeshingOverview • Recall that meshing is a three-step procedure: • Define element attributes • Specify mesh controls • Generate the mesh • In this chapter, we will expand on each of these steps and also discuss additional meshing options. • Topics covered: A. Multiple Element AttributesE. Hex-to-Tet Meshing B. Controlling Mesh DensityF. Mesh Extrusion C. Changing a MeshG. Sweep Meshing D. Mapped MeshingH. Workshop January 30, 2001 Inventory #001441 10-2

  3. MeshingA. Multiple Element Attributes • As we discussed earlier, every element has the following attributes associated with it: • Element type (TYPE) • Real constants (REAL) • Material properties (MAT) • Most FEA models have multiple attributes. For example, the silo shown here has two element types, three real constant sets, and two materials. TYPE 1 = shell TYPE 2 = beam MAT 1 = concrete MAT 2 = steel REAL 1 = 3/8” thickness REAL 2 = beam properties REAL 3 = 1/8” thickness January 30, 2001 Inventory #001441 10-3

  4. Meshing...Multiple Element Attributes • Whenever you have multiple TYPEs, REALs and MATs, you need to make sure that each element is assigned the proper attributes. There are three ways to do this: • Assign attributes to the solid model entities before meshing • Activate a “global” setting of MAT, TYPE, and REAL before meshing • Modify element attributes after meshing • If no assignments are made, ANSYS uses default settings of MAT=1, TYPE=1, and REAL=1 for all elements in the model. Note, the current active TYPE, REAL, and MAT dictates mesh operation. January 30, 2001 Inventory #001441 10-4

  5. Meshing...Multiple Element Attributes Assigning Attributes to the Solid Model 1. Define all necessary element types, materials, and real constant sets. 2. Then use the “Element Attributes” section of the MeshTool (Preprocessor > MeshTool): • Choose entity type and press the SET button. • Pick the entities to which you want to assign attributes. • Set the appropriate attributes in the subsequent dialog box. Or select the desired entities and use the VATT, AATT, LATT, or KATT command. 3. When you mesh an entity, its attributes are automatically transferred to the elements. January 30, 2001 Inventory #001441 10-5

  6. Meshing...Multiple Element Attributes Using Global Attribute Settings 1. Define all necessary element types, materials, and real constant sets. 2. Then use the “Element Attributes” section of the MeshTool (Preprocessor > MeshTool): • Choose Global and press the SET button. • Activate the desired combination of attributes in the “Meshing Attributes” dialog box. We refer to these as the active TYPE, REAL, and MAT settings. Or use the TYPE, REAL, and MAT commands. 3. Mesh only those entities to which the above settings apply. January 30, 2001 Inventory #001441 10-6

  7. Meshing...Multiple Element Attributes Modifying Element Attributes 1. Define all necessary element types, materials, and real constant sets. 2. Activate the desired combination of TYPE, REAL, and MAT settings: • Preprocessor > -Attributes- Define > Default Attribs... • Or use the TYPE, REAL, and MAT commands 3. Modify the attributes of only those elements to which the above settings apply: • Issue EMODIF,PICK or choose Preprocessor > Move/Modify > -Elements- Modify Attrib • Then pick the desired elements 4. In the subsequent dialog box, set attributes to “All to current.” January 30, 2001 Inventory #001441 10-7

  8. Some points to keep in mind: You can verify element attributes by activating attribute numbering: Utility Menu > PlotCtrls > Numbering Or /PNUM,attr,ON, where attr may be TYPE, MAT, or REAL Element attributes assigned directly to solid model entities will override the default attribute pointers. By assigning attributes to solid model entities, you can avoid having to reset attributes in the middle of meshing operations. This is advantageous because ANSYS meshing algorithms are most efficient when meshing all entities at once. Clearing a solid model entity of its mesh will not delete attribute assignments. Meshing...Multiple Element Attributes January 30, 2001 Inventory #001441 10-8

  9. Meshing...Multiple Element Attributes • Demo: • Resume ribgeom.db • List element types, real constants, and materials. One of each has been defined. • Bring up MeshTool, choose area attributes, and press Set • Pick the single area, show the Area Attributes dialog box, and press OK. (There is only one set of attributes, but this illustrates the general procedure.) January 30, 2001 Inventory #001441 10-9

  10. MeshingB. Controlling Mesh Density • ANSYS provides many tools to control mesh density, both on a global and local level: • Global controls • SmartSizing • Global element sizing • Default sizing • Local controls • Keypoint sizing • Line sizing • Area sizing January 30, 2001 Inventory #001441 10-10

  11. Meshing...Controlling Mesh Density SmartSizing • Determines element sizes by assigning divisions on all lines, taking into account curvature of the line, its proximity to holes and other features, and element order. • SmartSizing is off by default, but is recommended for free meshing. It does not affect mapped meshing. (Free meshing vs. mapped meshing will be discussed later.) January 30, 2001 Inventory #001441 10-11

  12. Meshing...Controlling Mesh Density • To use SmartSizing: • Bring up the MeshTool (Preprocessor > MeshTool), turn on SmartSizing, and set the desired size level. • Or use SMRT,level • Size level ranges from 1 (very fine) to 10 (very coarse). Defaults to 6. • Then mesh all volumes (or all areas) at once, rather than one-by-one. January 30, 2001 Inventory #001441 10-12

  13. Meshing...Controlling Mesh Density • Examples of different SmartSize levels are shown here for a tetrahedron mesh. • Advanced SmartSize controls, such as mesh expansion and transition factors, are available on the SMRT command (or Preprocessor > -Meshing- Size Cntrls > -SmartSize- Adv Opts...) • You can turn off SmartSizing using the MeshTool or by issuing smrt,off. January 30, 2001 Inventory #001441 10-13

  14. Global Element Sizing Allows you to specify a maximum element edge length for the entire model (or number of divisions per line): ESIZE,SIZE or Preprocessor > MeshTool > “Size Controls - Global” [Set] or Preprocessor > -Meshing- Size Cntrls > -Global- Size Can be used by itself or in conjunction with SmartSizing. Using ESIZE by itself (SmartSizing off) will result in a uniform element size throughout the volume (or area) being meshed. With SmartSizing on, ESIZE acts as a “guide,” but the specified size may be overridden to accommodate line curvature or proximity to features. Meshing...Controlling Mesh Density January 30, 2001 Inventory #001441 10-14

  15. Meshing...Controlling Mesh Density Default Sizing • If you don’t specify any controls, ANSYS uses default sizing, which assigns minimum and maximum line divisions, aspect ratio, etc. based on element order. • Meant for mapped meshing, but is also used for free meshing if SmartSizing is off. • You can adjust default size specifications using DESIZE or Preprocessor > -Meshing- Size Cntrls > -Global- Other. January 30, 2001 Inventory #001441 10-15

  16. Meshing...Controlling Mesh Density Keypoint Sizing • Controls element size at keypoints: • Preprocessor > MeshTool > “Size Controls: Keypt” [Set] • or KESIZE command • or Preprocessor > -Meshing- Size Cntrls > -Keypoints- Different keypoints can have different KESIZEs, giving you more control over the mesh. • Useful for stress concentration regions. • Specified sizes may be overridden by SmartSizing to accommodate line curvature or proximity to features. January 30, 2001 Inventory #001441 10-16

  17. Meshing...Controlling Mesh Density Line Sizing • Controls element size at lines: • Preprocessor > MeshTool > Size Controls: Lines [Set] • or LESIZE command • or Preprocessor > -Meshing- Size Cntrls > -Lines- Different lines can have different LESIZEs. • Size specifications may be “hard” or “soft.” • “Hard” sizes are always honored by the mesher, even if SmartSizing is on. They take precedence over all other size controls. • “Soft” sizes may be overridden by SmartSizing. • You can also specify a spacing ratio — ratio of last division to first. Used to bias the divisions towards one end or towards the middle. Yes for “soft” No for “hard” January 30, 2001 Inventory #001441 10-17

  18. Meshing...Controlling Mesh Density Area Sizing • Controls element size in the interior of areas: • Preprocessor > MeshTool > “Size Controls: Areas” [Set] • or AESIZE command • or Preprocessor > -Meshing- Size Cntrls > -Areas- Different areas can have different AESIZEs. • Bounding lines will use the specified size only if they have no LESIZE or KESIZE specified and if no adjacent area has a smaller size. • Specified sizes may be overridden by SmartSizing to accommodate line curvature or proximity to features. January 30, 2001 Inventory #001441 10-18

  19. Meshing...Controlling Mesh Density • Demo: • Resume ribgeom.db • Mesh with SMRT,6. (Not a very good mesh) • Re-mesh with SMRT,3 (good mesh) • Set ESIZE to 0.2 and re-mesh. The mesh becomes coarse even though SMRT is set to 3, because the smart-mesher takes ESIZE into account. Also note that the element sizes are not uniform (because SMRT is on). • Turn off SMRT and re-mesh. Element sizes are now uniform. January 30, 2001 Inventory #001441 10-19

  20. MeshingC. Changing a Mesh • If a mesh is not acceptable, you can always re-mesh the model by following these steps: 1. Clear the mesh. • The clear operation is the opposite of mesh: it removes nodes and elements. • Use the [Clear] button on the MeshTool, or use VCLEAR, ACLEAR, etc. (If you are using the MeshTool, you may skip this step since the program will prompt you whether to clear or not when you execute step 3.) 2. Specify new or different mesh controls. 3. Mesh again. January 30, 2001 Inventory #001441 10-20

  21. Meshing...Changing a Mesh • Another meshing option is to refine the mesh in specific regions. • Available for all area elements and only tetrahedral volume elements. • Easiest way is to use the MeshTool: • First save the database. • Then choose how you want to specify the region of refinement — at nodes, elements, keypoints, lines, or areas — and press the Refine button. • Pick the entities at which you want the mesh to be refined. (Not required if you choose “All Elems.”) • Finally, choose the level of refinement. Level 1 (minimal refinement) is a good starting point. January 30, 2001 Inventory #001441 10-21

  22. Meshing...Changing a Mesh • Demo: • Continuing the last demo… (ribgeom has been meshed with ESIZE = 0.2) • Choose refinement at Lines and press Refine • Pick the top line, then choose the default “minimal refinement” January 30, 2001 Inventory #001441 10-22

  23. MeshingD. Mapped Meshing • There are two main meshing methods: free and mapped. • Free Mesh • Has no element shape restrictions. • The mesh does not follow any pattern. • Suitable for complex shaped areas and volumes. • Mapped Mesh • Restricts element shapes to quadrilaterals for areas and hexahedra (bricks) for volumes. • Typically has a regular pattern with obvious rows of elements. • Suitable only for “regular” areas and volumes such as rectangles and bricks. January 30, 2001 Inventory #001441 10-23

  24. Free Mesh Easy to create; no need to divide complex shapes into regular shapes. Volume meshes can contain only tetrahedra, resulting in a large number of elements. Only higher-order (10-node) tetrahedral elements are acceptable, so the number of DOF can be very high. Mapped Mesh Generally contains a lower number of elements. Lower-order elements may be acceptable, so the number of DOF is lower. Areas and volumes must be “regular” in shape, and mesh divisions must meet certain criteria. Very difficult to achieve, especially for complex shaped volumes. Meshing...Mapped Meshing January 30, 2001 Inventory #001441 10-24

  25. Meshing...Mapped Meshing Creating a Free Mesh • Free meshing is the default setting for both area and volume meshes. • Create a free mesh is easy: • Bring up the MeshTool and verify that free meshing is set. • SmartSizing is generally recommended for free meshing, so activate it and specify a size level. Save the database. • Then initiate the mesh by pressing the Mesh button. • Press [Pick All] in the picker to choose all entities (recommended). • Or use the commands VMESH,ALL or AMESH,ALL. January 30, 2001 Inventory #001441 10-25

  26. Meshing...Mapped Meshing Creating a Mapped Mesh • This is not as easy as free meshing because the areas and volumes have to meet certain requirements: • Area must contain either 3 or 4 lines (triangle or quadrilateral). • Volume must contain either 4, 5, or 6 areas (tetrahedron, triangular prism, or hexahedron). • Element divisions on opposite sides must match. • For triangular areas or tetrahedral volumes, the number of element divisions must be even. January 30, 2001 Inventory #001441 10-26

  27. Meshing...Mapped Meshing • For quadrilateral areas or hexahedral volumes, unequal divisions are allowed, as shown in these examples, but the number of divisions must satisfy a formula (shown on the next page). January 30, 2001 Inventory #001441 10-27

  28. Meshing...Mapped Meshing January 30, 2001 Inventory #001441 10-28

  29. Meshing...Mapped Meshing • Thus mapped meshing involves a three-step procedure: • Ensure “regular” shapes, i.e, areas with 3 or 4 sides, or volumes with 4, 5, or 6 sides. • Specify size and shape controls • Generate the mesh January 30, 2001 Inventory #001441 10-29

  30. Meshing...Mapped Meshing Ensure regular shapes • In most cases, the model geometry is such that the areas have more than 4 sides, and volumes have more that 6 sides. To convert these to regular shapes, you may need to do one or both of these operations: • Slice the areas (or volumes) into smaller, simpler shapes. • Concatenate two or more lines (or areas) to reduce the total number of sides. January 30, 2001 Inventory #001441 10-30

  31. Meshing...Mapped Meshing • Slicing can be accomplished with the Boolean divide operation. • Remember that you can use the working plane, an area, or a line as the slicing tool. • Sometimes, it may be easier to create a new line or a new area than to move and orient the working plane in the correct direction. January 30, 2001 Inventory #001441 10-31

  32. Concatenating these two lines makes this a 4-sided area Meshing...Mapped Meshing • Concatenation creates a new line (for meshing purposes) that is a combination of two or more lines, thereby reducing the number of lines making up the area. • Use the LCCAT command or Preprocessor > -Meshing- Concatenate > Lines, then pick the lines to be concatenated. • For area concatenation, use ACCAT command or Preprocessor > -Meshing- Concatenate > Areas January 30, 2001 Inventory #001441 10-32

  33. Meshing...Mapped Meshing • You can also imply a concatenation by simply identifying the three or four corners of the area. In this case, ANSYS internally generates the concatenation. • To do this, choose Quad shape and Map mesh in the MeshTool. • Then change 3/4 sided to Pick corners. • Press the Mesh button, pick the area, and then pick the 3 or 4 corners that form the regular shape. January 30, 2001 Inventory #001441 10-33

  34. Meshing...Mapped Meshing • Notes on concatenation: • It is purely a meshing operation and therefore should be the last step before meshing, after all solid modeling operations. This is because the output entity obtained from a concatenation cannot be used in any subsequent solid modeling operation. • You can "undo" a concatenation by deleting the line or area it produced. • Concatenating areas (for mapped volume meshing) is generally much more complicated because you may also need to concatenate some lines. Lines are automatically concatenated only when two adjacent, 4-sided areas are concatenated. • Consider the add (Boolean) operation if the lines or areas meet at a tangent. January 30, 2001 Inventory #001441 10-34

  35. Meshing...Mapped Meshing Specify size and shape controls • This is the second step of the three-step mapped meshing procedure. • Choosing the shape is simple. In the MeshTool, choose Quad for area meshing, and Hex for volume meshing, then click on Map. • Commonly used size controls and the order in which they are applied: • Line sizing [LESIZE] is always honored. • Global element size , if specified, will be applied to “unsized” lines. • Default element sizing [DESIZE] will be applied to unsized lines only if ESIZE is not specified. • (SmartSizing is not valid.) January 30, 2001 Inventory #001441 10-35

  36. Meshing...Mapped Meshing • If you specify line divisions, remember that: • divisions on opposite sides must match, but you only need to specify one side. The map mesher automatically transfers divisions to the opposite side. • if you have concatenated lines, divisions can only be applied to the original (input) lines, not the composite line. 6 divisions specified on each original line. 12 divisions will be automatically applied to this line (opposite to composite line). How many divisions are used for the other two lines? (Upcoming demo will answer it.) January 30, 2001 Inventory #001441 10-36

  37. Meshing...Mapped Meshing Generate the mapped mesh • Once you have ensured regular shapes and assigned the appropriate divisions, generating the mesh is easy. Just press the Mesh button in the MeshTool, then press [Pick All] in the picker or choose the desired entities. January 30, 2001 Inventory #001441 10-37

  38. Meshing...Mapped Meshing • Question: How would you slice this model for mapped meshing? • Answer: It may not be worth the effort! January 30, 2001 Inventory #001441 10-38

  39. Meshing...Mapped Meshing • Demo: • Resume ribfull.db • Bring up MeshTool and apply 6 divisions to top and right lines • Map-mesh the area using “Pick corners.” Notice that the left and bottom lines get only two divisions each (from DESIZE). • Now specify ESIZE,,4 (4 divisions per line) and re-mesh • Finally, clear line divisions, specify ESIZE,0.1 (size), and re-mesh January 30, 2001 Inventory #001441 10-39

  40. MeshingE. Hex-to-Tet Meshing • For volume meshing, we have only seen two options so far: • Free meshing, which creates an all-tet mesh. This is easy to achieve but may not be desirable in some cases because of the large number of elements and total DOF created. • Mapped meshing, which creates an all-hex mesh. This is desirable but usually very difficult to achieve. • Hex-to-tet meshing provides a third option that is the “best of both worlds.” It allows you to have a combination of hex and tet meshes without compromising the integrity of the mesh. January 30, 2001 Inventory #001441 10-40

  41. This option works by creating pyramid-shaped elements in the transition region between hex and tet regions. Requires the hex mesh to be available (or at least a quad mesh at the shared area). The mesher first creates all tets, then combines and rearranges the tet elements in the transition region to form pyramids. Available only for element types that support both pyramid and tet shapes, e.g: Structural SOLID95, 186, VISCO89 Thermal SOLID90 Multiphysics SOLID62, 117, 122 Results are good even in the transition region. Element faces are compatible even when transitioning from a linear hex element to a quadratic tet element. SOLID95 Meshing...Hex-to-Tet Meshing January 30, 2001 Inventory #001441 10-41

  42. 20-Node Hex 13-Node Pyramid 10-Node Tet 8-Node Hex 9-Node Pyramid 10-Node Tet Meshing...Hex-to-Tet Meshing • Hex-to-tet meshing is valid for both quadratic-to-quadratic and linear-to-quadratic transitions. Element type must support a 9-node pyramid for the latter. Hex Mesh Transition Layer Tet Mesh Quadratic to Quadratic Linear to Quadratic January 30, 2001 Inventory #001441 10-42

  43. Meshing...Hex-to-Tet Meshing Procedure involves four steps: 1. Create the hex mesh. • Start by map-meshing the regular-shaped volumes. (Or mesh the shared areas with quads.) • For stress analysis, use either an 8-node brick (SOLID45 or SOLID185) or a 20-node brick (SOLID95 or SOLID186). January 30, 2001 Inventory #001441 10-43

  44. Meshing...Hex-to-Tet Meshing 2. Activate an element type that supports both pyramids and tets. • These are usually brick elements that can degenerate into pyramids and tets. Check the Elements Manual, available on-line, to find out which element types are valid. • Examples: • Structural SOLID95, 186, VISCO89 • Thermal SOLID90 • Multiphysics SOLID62, 117, 122 January 30, 2001 Inventory #001441 10-44

  45. Meshing...Hex-to-Tet Meshing 3. Generate the tet mesh. • First activate free meshing. • Then mesh the volumes that are to be tet-meshed. Pyramids are automatically generated at the interface. January 30, 2001 Inventory #001441 10-45

  46. Meshing...Hex-to-Tet Meshing 4. Convert degenerate tets to true 10-node tets. • The tet mesh created by the transition mesher consists of degenerate elements — 10-node tetrahedra derived from 20-node bricks, for example. • These elements are not as efficient as true 10-node tets such as SOLID92, which use less memory and write smaller files during solution. • To convert the degenerate tets into true tets: • Preprocessor > -Meshing- Modify Mesh > Change Tets... • Or use the TCHG command. January 30, 2001 Inventory #001441 10-46

  47. Meshing...Hex-to-Tet Meshing • Demo: • Resume hextet.db • Show element type list using Element Type > Add/Edit/Delete. There are two element types: SOLID45 & 95 • Bring up MeshTool and set ESIZE,1 (size) • Map-mesh the regular shaped volume • Set element type to 2, and activate tet-meshing • Free-mesh the other volume • Convert degenerate tets to SOLID92 • Show element type list. There are now three element types. • Select elements of type 2 (SOLID95 pyramids) and plot elements January 30, 2001 Inventory #001441 10-47

  48. MeshingF. Mesh Extrusion • When you extrude an area into a volume, you can extrude the area elements along with it, resulting in a meshed volume. This is called mesh extrusion. • Advantage: Easy to create a volume mesh with all bricks (hexahedra) or a combination of bricks and prisms. • Obvious requirement: Shape of the volume must lend itself to extrusion. Extrude January 30, 2001 Inventory #001441 10-48

  49. Meshing...Mesh Extrusion Procedure 1. Define two element types — an area element and a volume element. • Area element: Choose MESH200 quadrilaterals. MESH200 is a mesh-only (Not Solved) element and has no DOFs or material properties associated with it. • Volume element: Should be compatible with the MESH200 element type. For example, if you choose midside nodes for MESH200, the 3-D solid element should also have midside nodes. • ET command or Preprocessor > Element Type > Add/Edit/Delete January 30, 2001 Inventory #001441 10-49

  50. 2. Mesh the area to be extruded with MESH200 elements. Use mapped or free meshing with desired mesh density. Preprocessor > MeshTool 3. Choose element extrusion options. EXTOPT command or Preprocessor > Operate > Extrude > Elem Ext Opts Typical options are: Active TYPE attribute (should be 3-D solid). Number of element divisions in the extrusion direction (i.e, number of elements through the thickness). Must be greater than zero; otherwise, only the area will be extruded, without elements. Meshing...Mesh Extrusion January 30, 2001 Inventory #001441 10-50

More Related