mkb06-adapt.pdf

Chapter 4. Adaptive Meshing

Strona 1 z 8

Main TOC • Using Help • Copyright

Advanced Guide >Chapter 4. Adaptive Meshing

Chapter 4. Adaptive Meshing

4.1. What Is Adaptive Meshing?

The ANSYS program provides approximate techniques for automatically estimating mesh discretization

error for certain types of analyses. (See The General Postprocessor (POST1) in the ANSYS Basic Analysis

Guide for more information about error-value approximation.) Using this measure of mesh discretization

error, the program can then determine if a particular mesh is fine enough. If it is not, the program will

automatically refine the mesh so that the measured error will decrease. This process of automatically

evaluating mesh discretization error and refining the mesh, called adaptive meshing , continues through a

series of solutions until the measured error drops below some user-defined value (or until a user-defined

limit on the number of solutions is reached).

3.8. Sample Probabilistic Design

Analysis

Home

4.2. Prerequisites for Adaptive Meshing

Main TOC • Using Help • Copyright

Advanced Guide > Chapter 4. Adaptive Meshing >4.2. Prerequisites for Adaptive

Meshing

4.2. Prerequisites for Adaptive Meshing

The ANSYS program includes a prewritten macro, ADAPT.MAC , to perform adaptive meshing. Your model

must satisfy certain preconditions before you can successfully activate the ADAPT macro. (In some

cases, models that do not conform to these criteria can be adaptively meshed using a modified procedure,

as discussed below.) These requirements include the following:

The standard ADAPT procedure is valid only for single-solution linear static structural and linear

steady-state thermal analyses.

Your model should preferably use only one material type, as the error calculations are based in part

on average nodal stresses, and would thus often be invalid at the material interfaces. Also, an

element's error energy is affected by its elastic modulus. Therefore, even if the stress discontinuity

is the same in two adjoining elements, their error energy will be different if they have different

material properties. You should also avoid abrupt changes in shell thickness, as such discontinuities

will cause similar stress-averaging problems.

file://C:\Temp\~hh38FC.htm

06.11.02

Chapter 4. Adaptive Meshing

Strona 2 z 8

Your model must use element types that support error calculations. (See Element Types That can

be Used in Adaptive Meshing for a list of valid element types.)

You must build your model using meshable solid model entities: that is, characteristics that will

cause meshing failure must not be built into your model.

Table 4.1. Element Types That Can Be Used in Adaptive Meshing

Type

Element

Description

2-D Structural Solids

PLANE2

PLANE25

PLANE42

PLANE82

PLANE83

2-D 6-Node Triangular Solid

Axisymmetric Harmonic Solid

2-D 4-Node Isoparametric Solid

2-D 8-Node Solid

Axisymmetric Harmonic 8-Node Solid

3-D Structural Solids

SOLID45

SOLID64

SOLID92

SOLID95

3-D 8-Node Isoparametric Solid

3-D Anisotropic Solid

3-D 10-Node Tetrahedral Solid

3-D 20-Node Isoparametric Solid

3-D Structural Shells

SHELL43

SHELL63

SHELL93

Plastic Quadrilateral Shell

Elastic Quadrilateral Shell

8-Node Isoparametric Shell

2-D Thermal Solids

PLANE35

PLANE75

PLANE55

PLANE77

PLANE78

2-D 6-Node Triangular Solid

Axisymmetric Harmonic Solid

2-D 4-Node Isoparametric Solid

2-D 8-Node Solid

Axisymmetric Harmonic 8-Node Solid

3-D Thermal Solids

SOLID70

SOLID87

SOLID90

3-D 8-Node Isoparametric Solid

3-D 10-Node Tetrahedral Solid

3-D 20-Node Isoparametric Solid

3-D Thermal Shells SHELL57 Plastic Quadrilateral Shell

Chapter 4. Adaptive Meshing

Home

4.3. How to Use Adaptive Meshing:

Basic Procedure

Main TOC • Using Help • Copyright

Advanced Guide > Chapter 4. Adaptive Meshing >4.3. How to Use Adaptive Meshing:

Basic Procedure

4.3. How to Use Adaptive Meshing: Basic Procedure

The basic procedure for running the adaptive meshing macro follows these steps:

file://C:\Temp\~hh38FC.htm

06.11.02

Chapter 4. Adaptive Meshing

Strona 3 z 8

1. As in any linear static structural or steady state thermal analysis, first enter the preprocessor

( /PREP7 command or menu path Main Menu>Preprocessor ). Then, specify the element type,

real constants, and material properties, in accordance with the prerequisites listed above.

2. Model your system using solid modeling procedures, creating meshable areas or volumes that

describe the geometry of your system. You do not need to specify element sizes, nor do you need to

mesh these areas and volumes - the ADAPT macro will automatically initiate meshing for you. (If

you need to mesh your model with both area and volume elements, create an ADAPTMSH.MAC user

subroutine - see below.)

3. You can either proceed to SOLUTION ( /SOLU or menu path Main Menu>Solution ) or remain in

PREP7 to specify analysis type, analysis options, loads, and load step options. Apply only solid

model loads and inertia loads (accelerations, rotational accelerations, and rotational velocities) in a

single load step. (Finite element loads, coupling, and constraint equations can be introduced

through the ADAPTBC.MAC user subroutine. Multiple load steps can be introduced through the

ADAPTSOL.MAC subroutine. The subroutines are discussed later in this chapter.)

4. If in PREP7, exit the preprocessor [ FINISH ]. (You can invoke the ADAPT macro from either

SOLUTION or the Begin level.)

5. Invoke the adaptive solution. To do so, use one of these methods:

Command(s):

ADAPT

GUI:

Main Menu>Solution>Solve>Adaptive Mesh

Notice that you can use the ADAPT macro in either a thermal or a structural analysis, but that you

cannot mix the two disciplines in one adaptive solution. As the adaptive meshing iterations

proceed, element sizes will be adjusted (within the limits set by FACMN and FACMX ) to decrease and

increase the elemental error energies until the error in energy norm matches the target value (or

until the specified maximum number of solutions has been used).

After you have invoked the adaptive solution, this macro controls all program operations until the

solution is completed. The ADAPT macro will define element sizes, generate the mesh, solve,

evaluate errors, and iterate as necessary till the target value of error in energy norm is met. All these

steps are performed automatically, with no further input required from you.

6. Once adaptive meshing has converged, the program automatically turns element shape checking on

[ SHPP ,ON]. It then returns to the SOLUTION phase or to the Begin level, depending on which

phase you were in when you invoked ADAPT . You may then enter POST1 and postprocess as

desired, using standard techniques.

4.2. Prerequisites for Adaptive Meshing

Home

4.4. Modifying the Basic Procedure

Main TOC • Using Help • Copyright

Advanced Guide > Chapter 4. Adaptive Meshing >4.4. Modifying the Basic Procedure

file://C:\Temp\~hh38FC.htm

06.11.02

Chapter 4. Adaptive Meshing

Strona 4 z 8

4.4. Modifying the Basic Procedure

4.4.1. Selective Adaptivity

If you know that mesh discretization error (measured as a percentage) is relatively unimportant in some

regions of your model (for instance, in a region of low, slowly-changing stress), you can speed up your

analysis by excluding such regions from the adaptive meshing operations. Also, you might want to

exclude regions near singularities caused by concentrated loads. Selecting logic provides a way of

handling such situations.

Figure 4.1. Selective Adaptivity

Selective adaptivity can improve the performance of models having concentrated loads.

If you select a set of keypoints, the ADAPT macro will still include all your keypoints (that is, the

ADAPT macro will modify the mesh at both selected and non-selected keypoints), unless you also set

KYKPS = 1 in the ADAPT command ( Main Menu>Solution>Solve>Adaptive Mesh ).

If you select a set of areas or volumes, the ADAPT macro will adjust element sizes only in those regions

that are in the selected set. You will have to mesh your entire model in PREP7 before executing ADAPT .

4.4.2. Customizing the ADAPT Macro with User Subroutines

The standard ADAPT macro might not always be applicable to your particular analysis needs. For

instance, you might need to mesh both areas and volumes, which is not possible with the standard macro.

For this and other such situations, you can modify the ADAPT macro to suit your analysis needs. By

using a macro to perform the adaptive meshing task, we have intentionally given you access to the logic

involved, and have thereby furnished you with the capability for modifying the technique as you might

desire.

Fortunately, you do not always need to change the coding within the ADAPT macro to customize it.

Three specific portions of the macro can be readily modified by means of user subroutines , which are

file://C:\Temp\~hh38FC.htm

06.11.02

Chapter 4. Adaptive Meshing

Strona 5 z 8

separate user files that you can create and that will be called by the ADAPT macro. The three features

that can be modified by user subroutines are:

the meshing command sequence

the boundary condition command sequence,

the solution command sequence

The corresponding user subroutine files must be named ADAPTMSH.MAC , ADAPTBC.MAC , and

ADAPTSOL.MAC , respectively.

4.4.2.1. Creating a Custom Meshing Subroutine (ADAPTMSH.MAC)

By default, if your model contains one or more selected volumes, the ADAPT macro will mesh only

volumes (no area meshing will be done). If you have no selected volumes, then the ADAPT macro will

mesh only areas. If you desire to mesh both volumes and areas, you can create a user subroutine,

ADAPTMSH.MAC , to perform all the desired operations. You will need to clear any specially-meshed entities

before remeshing. Such a subroutine might look like this:

C*** Subroutine ADAPTMSH.MAC - Your name - Job Name - Date Created

TYPE,1 ! Set element TYPE attribute for area meshing

ACLEAR,3,5,2 ! Clear areas and volumes to be meshed by this subroutine

VCLEAR,ALL

AMESH,3,5,2 ! Mesh areas 3 and 5 (no other areas will be meshed by ADAPT)

TYPE,2 ! Change element type for volume mesh

VMESH,ALL ! Mesh all volumes

Please see the TYPE , ACLEAR , VCLEAR , AMESH , and VMESH command descriptions for more

information.

We strongly recommend that you include a comment line (C***) to identify your macro uniquely. This

comment line will be echoed in the job printout, and will provide assurance that the ADAPT macro has

used the correct user subroutine.

4.4.2.2. Creating a Custom Subroutine for Boundary Conditions (ADAPTBC.MAC)

The ADAPT macro clears and remeshes with every new solution loop. As a result, your model's nodes

and elements will be repeatedly changing. This situation generally precludes the use of finite element

loads, DOF coupling, and constraint equations, all of which must be defined in terms of specific nodes

and elements. If you need to include any of these finite-element-supported items, you can do so by

writing a user subroutine, ADAPTBC.MAC . In this subroutine, you can select nodes by their location, and

can then define finite element loads, DOF coupling, and constraint equations for the selected nodes. A

sample ADAPTBC.MAC subroutine follows:

C*** Subroutine ADAPTBC.MAC - Your name - Job Name - Date Created

NSEL,S,LOC,X,0 ! Select nodes @ X=0.0

D,ALL,UX,0 ! Specify UX=0.0 for all selected nodes

NSEL,S,LOC,Y,0 ! Select nodes @ Y=0.0

D,ALL,UY,0 ! Specify UY=0.0 for all selected nodes

NSEL,ALL ! Select all nodes

4.4.2.3. Creating a Custom Solution Subroutine (ADAPTSOL.MAC)

The default solution command sequence included in the ADAPT macro is simply:

/SOLU

file://C:\Temp\~hh38FC.htm

06.11.02

Plik z chomika:

Inne pliki z tego folderu:

Inne foldery tego chomika: