1 of 59

Module 05: Mesh Control

Introduction to ANSYS Mechanical

17.0 Release

1

March 10, 2016

2 of 59

Module 05 Topics

Meshing in Mechanical
Global Mesh Controls
Local Mesh Controls
Troubleshooting
Virtual Topology
Direct Modeling
Mesh Quality Criteria

This module covers introductory topics for meshing and mesh control:

Workshop 05.1: Mesh Creation
Workshop 05.2: Mesh Control
Appendix 05.1: Model Assembly
Appendix 05.2: Mesh Quality Criteria

2

March 10, 2016

3 of 59

05.01 Meshing in Mechanical

The nodes and elements representing the geometry model make up the mesh:

A “default” mesh is automatically generated during a solution.
It is generally recommended that additional controls be added to the default mesh before solving.
A finer mesh produces more precise answers but also increases CPU time and memory requirements.

Generate the mesh or preview the surface of the mesh before solving (previewing the surface mesh is faster than generating the entire mesh).

3

March 10, 2016

4 of 59

05.02 Global Mesh Controls

Physics-Based Meshing allows the user to specify the metrics used in measuring element quality to be based on the kind of analysis being done.

Physics preferences are:

Mechanical
Electromagnetics
CFD
Explicit

Different analysis types define acceptable or favorable element shapes differently. For this course we limit the discussion to Mechanical.

4

March 10, 2016

5 of 59

05.02 Global Mesh Controls

Relevance is the most basic global size control and is set in the “Defaults” area of the mesh details.
Relevance is set between –100 and +100 (zero = default).

− Relevance = coarse mesh

+ Relevance = fine mesh

5

March 10, 2016

6 of 59

05.02 Global Mesh Controls

Sizing Control:

The points below assume that Size Function is set to “Adaptive.” (Size Function is discussed further on the next slide.)
Relevance Center sets the midpoint of the “Relevance” global control.
Element Size defines the maximum element size used for the entire model.
For most static structural applications the, default values for the remaining global controls are usually adequate.

Medium

Coarse

Fine

-100

+100

0

-100

+100

0

Relevance Center

6

March 10, 2016

7 of 59

05.02 Global Mesh Controls

Size Function provides several advanced automated control options over the global mesh sizing. It is controlled in the Mesh Details view.

While many of these controls are beyond the scope of an introductory course, we’ll review some of the advanced size controls here. As stated earlier, linear static analysis types usually do not share the same meshing demands as more advanced analysis types, and so advanced size controls are not often necessary.
“Adaptive” is the default setting for the Mechanical Physics Preference, and provides the highest level of automation.
Four advanced size functions can be employed: Proximity, Curvature, Uniform, and Proximity and Curvature (the last is just a combination of the first two).

7

March 10, 2016

8 of 59

05.02 Global Mesh Controls

The Uniform Size Function provides control based solely on the user-input parameters Min Size, Max Face Size, Max Tet Size, and Growth Rate.

The Curvature Size Function, as the name implies, is driven by the curvature encountered in the geometry: the higher the curvature, the higher the mesh density. For models dominated by lots of curved features this control provides a way to refine the mesh over much of the model without using numerous local controls. For models composed of mostly straight features, this control will have a lesser impact.

Curvature On

Curvature Off

8

March 10, 2016

9 of 59

05.02 Global Mesh Controls

The Proximity Size Function provides a means to control the mesh density in regions of the model where features are located more closely together. In cases where the geometry contains a number of such regions, this control provides a way to refine the mesh over much of the model without using numerous local controls.

As mentioned above, proximity and curvature can be combined.

Num Cells = 4

Num Cells = 12

9

March 10, 2016

10 of 59

05.02 Global Mesh Controls

Shape Checking:

Standard Mechanical is recommended for linear stress, modal, and thermal analyses.
Aggressive Mechanical is recommended for analyses involving large deformations and/or material nonlinearities.
Other settings are typically not used for mechanical analyses.

Element Midside Nodes:

Program Controlled (default), Dropped, or Kept (see below).

Number of Retries: If poor quality elements are detected, the mesher will try again using finer mesh controls. This setting limits the number of possible retries.

Kept

Dropped

Element A

Element B

10

March 10, 2016

11 of 59

05.03 Local Mesh Controls

Local Mesh Controls can be applied to either a Geometry Selection or a Named Selection. These are available only when the mesh branch is highlighted. Some of the available controls include :

Method Control
Sizing Control
Contact Sizing Control
Refinement Control
Face Meshing Control
Inflation Control
Pinch Control

11

March 10, 2016

12 of 59

05.03 Local Mesh Controls

Method Control: provides the user with options for the meshing algorithm to be used.

Method = Automatic (default):

Body will be swept if possible. Otherwise, the “Patch Conforming Tetrahedron” mesher will be used.

12

March 10, 2016

13 of 59

05.03 Local Mesh Controls

Mesh Methods for 3D bodies:

Automatic
Tetrahedrons

Patch Conforming
Patch Independent

MultiZone

Mainly hexahedral elements

Hex dominant
Sweep

Mesh Methods for 2D bodies:

Automatic Method (Quad Dominant)
Triangles
Uniform Quad/Tri
Uniform Quad

Triangle (Tri)

Quadrilateral (Quad)

13

March 10, 2016

14 of 59

05.03 Local Mesh Controls

Method = Tetrahedrons:

An all-tetrahedron mesh is generated (not usually requested for mechanical applications).
Can use Patch Conforming or Patch Independent Meshing algorithms.

Patch Conforming

Patch Independent

Underlying Geometry

14

March 10, 2016

15 of 59

05.03 Local Mesh Controls

Method = Hex Dominant: Creates a free hex-dominant mesh

Recommended for meshing bodies with large interior volumes.
Not recommended for thin or highly complex shapes.
Useful for meshing bodies that cannot be swept.

Solid Model with Hex dominant mesh (approximate percentages):

Tetrahedrons – 443 (9.8%)

Hexahedron – 2801(62.5%)

Wedge – 124 (2.7%)

Pyramid – 1107 (24.7%)

15

March 10, 2016

16 of 59

05.03 Local Mesh Controls

Method = Sweep (hex and possibly wedge shapes):

Source/Target Selection: Manually select the start/end faces for sweeping or allow the mesher to choose.
Can include size controls and/or biasing along sweep.

Source

Target

Note: the geometry shown here has six different possible sweep directions.

16

March 10, 2016

17 of 59

05.03 Local Mesh Controls

Method = MultiZone:

Based on blocking approach used in ANSYS ICEM CFD Hexa

Automatically decomposes geometry

Uses structured and unstructured blocks
Can have multiple source and target faces
Depends on settings of Free Mesh Type

Structured blocks are meshed with Hexa or Hexa/Prism
If Free Mesh Type is set to other than Not Allowed then unstructured blocks are meshed with Tetra, Hexa Dominant or Hex Core based on the selected method
Program Controlled inflation
Access

RMB on Mesh
Insert → Method
Definition → Method → MultiZone

MultiZone Mesh

17

March 10, 2016

18 of 59

05.03 Local Mesh Controls

Method = MultiZone—Controls:

Src/Trg Selection = Automatic

Details View of MultiZone Method

Geometry for MultiZone Meshing

MultiZone Mesh

18

March 10, 2016

19 of 59

05.03 Local Mesh Controls

Method = MultiZone—Controls:

Src/Trg Selection = Manual

Details View of MultiZone Method

Geometry for MultiZone Meshing

Cut section of MultiZone Mesh

19

March 10, 2016

20 of 59

05.03 Local Mesh Controls

Method = MultiZone—Controls:

Free Mesh Type = Tetra, �Tetra/Pyramid, Hexa �Dominant, or Hexa Core

Geometry

Type: Tetra

Type: Hexa Dominant

Type: Hexa Core

Type: Tetra/Pyramid

20

March 10, 2016

21 of 59

05.03 Local Mesh Controls

Method = MultiZone—Controls:

Local Defeaturing Tolerance

Can be also controlled with global defeaturing tolerance

Geometry with a sliver face

Sliver face captured in mesh

No Defeaturing

Using Defeaturing

Sliver face ignored in�mesh

21

March 10, 2016

22 of 59

05.03 Local Mesh Controls

Surface Body Methods:

Quadrilateral Dominant (default): attempts to mesh with as many quadrilateral elements as possible, fills in with triangles.

Triangles: all triangular shapes are used.

MultiZone Quad/Tri: Depending on settings, quad or tri shapes are created using a patch independent algorithm.

Note: Each method contains a unique set of options in the details allowing additional configuration.

22

March 10, 2016

23 of 59

05.03 Local Mesh Controls

Sizing:

Element Size (element edge length)
Number of Divisions
Sphere of Influence (see next page)

“Soft” control may be overridden by other mesh controls, “Hard” may not.

23

March 10, 2016

24 of 59

05.03 Local Mesh Controls

Sizing—sphere of Influence:

Center is located using a coordinate system.
All scoped entities within the sphere are affected by size settings.
Only the portion of the scoped face or body within the sphere is included in the scope of the mesh control.

24

March 10, 2016

25 of 59

05.03 Local Mesh Controls

Contact Sizing: generates similarly-sized elements on contact faces for face/face or face/edge contact regions.

“Element Size” or “Relevance” can be specified.
Can drag and drop a Contact Region object onto the “Mesh” branch as a shortcut.

25

March 10, 2016

26 of 59

05.03 Local Mesh Controls

Refinement:

An initial mesh is created using the global and local size settings, then elements are divided at the scoped locations (up to 3 times).

Note: The refinement method generally offers less control and/or predictability over the final mesh, since the initial mesh is simply split. This splitting process may adversely affect other meshing controls.

26

March 10, 2016

27 of 59

05.03 Local Mesh Controls

Mapped Face Meshing: generates structured meshes on surfaces

Mapped quad or tri mesh also available for surface bodies.

27

March 10, 2016

28 of 59

05.03 Local Mesh Controls

Mapped Face Meshing:

For some geometry mapping will fail if an obvious pattern is not recognized.
By specifying side, corner or end vertices a mapped face can be achieved.

Original mapping failed as indicated by the status icon.

By specifying side and end vertices, the mapped face mesh succeeds.

28

March 10, 2016

29 of 59

05.03 Local Mesh Controls

Inflation: useful for adding layers of elements along specific boundaries.

Note: Inflation is used more often in CFD and EMAG applications, but may occasionally be useful for capturing stress concentrations etc. in structural applications.

29

March 10, 2016

30 of 59

05.03 Local Mesh Controls

Pinch: allows the removal of small features by “pinching” out small edges and vertices.

Master: geometry that retains the original geometry profile.
Slave: geometry that changes to move toward the master.
Can be automatic (mesh branch details) or local (add Pinch branch).

30

March 10, 2016

31 of 59

05.04 Troubleshooting

Mesh Metrics

Requested in the “statistics” section
Select individual bars in the graph to view the �elements graphically.

Mesh metrics are described further Section 05.07 “Mesh Quality Criteria” and in Appendix 05.2 “Mesh Quality Criteria.”

31

March 10, 2016

32 of 59

05.04 Troubleshooting

If the mesher is not able to generate a mesh, an error message will be returned:

Double click the message field in the status bar to open the messages window.
Double click individual messages to show the error in a separate window.

When possible, Mechanical will �graphically display the problem �region(s) (RMB in the message �window). Using the wireframe view �will make finding these areas easier.

32

March 10, 2016

33 of 59

05.04 Troubleshooting

The mesher also provides visual cues to identify obsolete and/or failed meshes. As shown in the figures below, failed meshes are shaded in maroon and obsolete meshes are shaded in yellow.

33

March 10, 2016

34 of 59

05.05 Virtual Topology

Virtual topology is a feature that can aid you in reducing the number of elements in the model, simplifying small features out of the model, and simplifying load abstraction. The “Virtual Topology” branch is added below the “Model” branch.

For meshing certain CAD models you may want to group faces and/or edges together allowing you to form virtual cells in order to reduce or improve the elements.
You can split a face to create two virtual faces, or split an edge to create two virtual edges for improved meshing.
Virtual Cells can be created automatically.

34

March 10, 2016

35 of 59

05.05 Virtual Topology

In this example, one edge of this multibody part has a size control assigned which causes irregularities in the overall mesh.

In the figure at upper right, 3 edges are �“virtually” split to produce improved �elements shapes.

Initial Mesh

Final Mesh

Virtual Split Edges

Size Control

35

March 10, 2016

36 of 59

05.05 Virtual Topology

Surface Model Example:

Virtual Cell

36

March 10, 2016

37 of 59

05.05 Virtual Topology

A “Virtual Topology” branch is added below the “Model” branch:

Individual virtual entities do not appear in the tree. Instead, a statistics section in the details lists virtual entities.
Virtual Cells can be created manually:

Select the entities to be included in the virtual cell.
Choose “Merge Cells” in the context menu (or RMB > Insert > Virtual Cell)

Virtual Cells can be created automatically:

Low, Medium, High: Indicates how aggressively virtual topology will be searched for.
Edges Only: Searches for adjacent edges to be combined.
Custom: users have control on specific options

37

March 10, 2016

38 of 59

05.05 Virtual Topology

In some instances it may be desirable to modify topology to allow application of some desired effect (e.g., mesh control, load, support, …):

Split face at vertices

Split Edge

Add a hard vertex

38

March 10, 2016

39 of 59

05.05 Virtual Topology

Virtual entities can be reviewed, edited or deleted from the context toolbar (highlight Virtual Topology branch):

Use the arrow keys to cycle through next/previous virtual entities.
The virtual entity is highlighted graphically and the status bar (bottom of graphics window) indicates the current selection.
The Edit icon allows access to an editor window where modifications to the virtual entity definition can be made.
Use “Delete” to remove unwanted virtual entities.

39

March 10, 2016

40 of 59

05.05 Virtual Topology

Keep in mind that the underlying “real” topology can change!

Example: a chamfer is included along with the top surface in this virtual cell. The interior lines are not recognized anymore.

Original mesh

The resulting element’s edge is shown as a solid line and the original chamfer and top surface is shown as a dotted line.

The chamfer representation is no longer present.

Mesh with virtual topology

40

March 10, 2016

41 of 59

05.06 Direct Meshing

Bodies can be meshed/remeshed individually in any desired order

Subsequent bodies will use the attached face mesh
The meshing results will depend on the meshing order
RMB on the body/bodies to generate the mesh locally

Automated meshing

Meshing first the block then the pipe

Hexas

Wedges

Meshing first the pipe then the block

Hexas

41

March 10, 2016

42 of 59

05.07 Mesh Quality Criteria

You can check mesh quality using Mesh Metrics.

Remember: Each physics type has its own quality criteria.

42

March 10, 2016

43 of 59

05.07 Mesh Quality Criteria

The Mesh Details Display Style option can be used to display the mesh color-coded by the various mesh quality measures:

43

March 10, 2016

44 of 59

05.07 Mesh Quality Criteria

Example mesh metric : Element Quality

This metric is based on the ratio of the volume to the edge length for a given element.

0 1

Bad Perfect

44

March 10, 2016

45 of 59

05.07 Mesh Quality Criteria

For additional information on mesh metrics, see�Appendix 05.2: Mesh Quality Criteria

45

March 10, 2016

46 of 59

05.08 Workshop 05.1: Mesh Creation

Goal:

Use the various mesh controls to mesh a small assembly.

46

March 10, 2016

47 of 59

05.09 Workshop 05.2: Mesh Control

Goal:

Use the various mesh controls to enhance the mesh for a small assembly.

47

March 10, 2016

48 of 59

05.10 Appendix 05.1

Model Assembly

48

March 10, 2016

49 of 59

05.10 Appendix 05.1: Model Assembly

Geometry is not only the starting point for a Workbench-based structural simulation.

Multiple finite element models can be assembled to leverage all Mechanical functionalities, including contact detection.

49

March 10, 2016

50 of 59

05.10 Appendix 05.1: Model Assembly

You can import mesh data (solids and shells) from *.cdb^† files into Workbench using the External Model component system and scale, rotate, and/or translate parts as needed.

Contact detection will be performed as if you were working with geometry data.

^† A *.cdb file is an ANSYS format that contains model information in terms of ANSYS Mechanical APDL commands.

50

March 10, 2016

51 of 59

05.10 Appendix 05.1: Model Assembly

Multiple Workbench systems can also be combined. Geometry, Mesh, and Named Selections are retrieved.

51

March 10, 2016

52 of 59

05.11 Appendix 05.2

Mesh Quality Criteria

52

March 10, 2016

53 of 59

05.11 Appendix 05.2: Mesh Quality Criteria

Aspect Ratio:

1 5-10 20 ∞

Perfect Bad

53

March 10, 2016

54 of 59

05.11 Appendix 05.2: Mesh Quality Criteria

Jacobian Ratio:

1 10 30 ∞

Perfect Bad

54

March 10, 2016

55 of 59

05.11 Appendix 05.2: Mesh Quality Criteria

Warping Ratio:

0 0.2 0.4 ∞

Perfect Bad

0 0.1 1 ∞

Perfect Bad

55

March 10, 2016

56 of 59

05.11 Appendix 05.2: Mesh Quality Criteria

Parallel Deviation:

0 170

Perfect Bad

56

March 10, 2016

57 of 59

05.11 Appendix 05.2: Mesh Quality Criteria

Maximum Corner Deviation:

90 180

Perfect Bad

60 165

Perfect Bad

57

March 10, 2016

58 of 59

05.11 Appendix 05.2: Mesh Quality Criteria

Skewness:

0 0.75 1

Perfect Bad

58

March 10, 2016

59 of 59

05.11 Appendix 05.2: Mesh Quality Criteria

Orthogonal Quality:

0 1

Bad Perfect

59

March 10, 2016