Meshing is a critical step in the finite element simulation process, as the quality of the mesh largely determines the accuracy of the results. When using ANSYS for finite element meshing, you may need to familiarize yourself with the APDL commands listed in this article.
There are two types of meshing methods in ANSYS:
Free Meshing: There are no restrictions on the shape of the elements, and there are no specific requirements for the geometry model. However, the relative number of elements is high, analysis time is long, and accuracy is low. When choosing free meshing, you can use commands such as AESIZE, LESIZE, KESIZE, and ESIZE to manually set the size of the mesh.
Mapped Meshing: The mesh is arranged in a regular pattern, with high accuracy, but the partitioning area must satisfy certain topological conditions. For complex-shaped boundaries, its modeling capability is not as good as that of free meshing. In ANSYS, to achieve the requirements of mapped meshing, you can use the LCCAT command to connect certain edges of polygons with four sides or more into one edge, and the ACCAT command to cut and connect certain faces of polyhedrons with six or more sides into one face.
ANSYS meshing consists of three steps.
Step 1: Define element attributes, including specifying the element type, material properties, and other options.
The ITYPE is the element type number, and Ename is the name of the element type selected by the user from the ANSYS element library, such as BEAM3 or PLANE42. KOP1,…,KOP6 are options switches that mainly include stiffness formula terms and print output control. INOPR is used to compress all results output for the element.
Material properties are defined using the MP command. When the material properties are fixed, their value is C0. When they vary with temperature, they are controlled by the last four parameters. MAT is the material property number, and Lab is the material property category, including elastic modulus (EX, EY, EZ), density (DENS), Poisson’s ratio (NUXY, NUYZ, NUXZ, PRXY, PRYZ, PRXZ), shear modulus (GXY, GYZ, GXZ), and coefficient of thermal expansion (ALPX, ALPY, ALPZ).
Real constants are used to supplement the geometric characteristics of an element, such as the area of a beam element or the thickness of a shell element. The parameters must be consistent with the order of the element type. NSET is the number of the real constant.
ITYPE, MAT, and NSET are used to declare which group of defined element types, material properties, and real constants will be used.
“TYPE, ITYPE”: This command lets you choose which set of pre-defined unit types to use. It works together with the “ET” command.
“REAL, NSET”: This command lets you choose which set of pre-defined real constants to use. It works together with the “R” command.
“MAT, MAT”: This command lets you choose which set of pre-defined material properties to use. It works together with the “MP” command.
Step 2: Meshing control includes controlling the shape, size, and type of the mesh.
① The shape of the element can be a triangle, quadrilateral, tetrahedron, or hexahedron, and the shape options differ depending on the type of object and mesh type.
② The size of the element can be controlled, for example, to obtain a relatively dense mesh in areas of high curvature in the model.
③ The type of mesh can be selected, including free meshing or mapped meshing.
The MSHKEY command is used to declare the meshing method, where KEY=0 indicates free meshing, KEY=1 indicates mapped meshing, and KEY=2 prioritizes mapped meshing.
The MSHAPE command is used to declare the meshing shape, where KEY=0 indicates quadrilateral meshing and KEY=1 indicates triangular meshing in 2D, and KEY=0 indicates tetrahedral meshing and KEY=1 indicates hexahedral meshing in 3D.
ESIZE, SIZE, and NDIV are used to set the length or the number of divisions for the segments of the unit to be partitioned. SIZE sets the length of the unit’s edges, and the number of divisions for the line is automatically calculated based on its length. If SIZE is set to 0 or left blank, NDIV is used instead. NDIV is used to set the number of divisions for the unit on the line, but it is not effective if SIZE is already set.
AESIZE, ANUM, and SIZE are used to set the partition size of the unit on the surface. ANUM is the surface number, which can also be set to ALL, P, or the name of the component. SIZE is the value of the unit size. If “ASIZE” controls the size of the boundary and intelligent grid division is set to ON, the size of the boundary may be refined for curved or transitional regions.
LESIZE is used to set the size of the grid unit for the selected line.
NL1 is the line number, which can also be set to ALL, P, or the name of the component. SIZE refers to the length of the unit’s edges if NDIV is left blank, and the number of divisions is automatically calculated. ANGSIZ is used to divide the curve into many angles, and the angle span on the curve is the size of the grid unit. ANGSIZ is only used when SIZE and NDIV are set to 0 or left blank.
NDIV represents the number of divisions for each line if it is a positive value. If NDIV is set to -1 (and KFORC=1), it means that the unit subdivision number for each line is 0. SPACE is the ratio of the interval of the divided line segment, with the default value of 1.0, which represents an even spacing. For layered grids, SPACE is usually set to 1.0. If SPACE is set to FREE, the step ratio is determined by other factors. If SPACE is a positive value, it represents the ratio of the spacing at the end of the line segment to the spacing at the beginning of the line segment. If SPACE is negative, it represents the ratio of the spacing in the middle of the line segment to the spacing at both ends.
KFORC is a value ranging from 0 to 3, and it is only used when NL1 is set to ALL to determine the selection line to be modified. LAYER1 specifies the thickness of the inner grid, with a default value of 0, and LAYER2 specifies the thickness of the outer grid, with a default value of 0. When KYNDIV is set to 0, No, or Off, intelligent grid division is not effective. When KYNDIV is set to 1, Yes, or On, intelligent grid division is prioritized for large curvature or adjacent areas.
Set the size of the edge of the unit closest to the key point.
NPT: the key point number, can also be ALL, P, or the name of the component.
SIZE: the value of the unit edge length closest to the key point NPT (overrides any other size). If SIZE is 0 or empty, use FACT1 or FACT2.
FACT1: a proportion factor that applies to the previously specified SIZE. Only used when SIZE is 0 or empty.
FACT2: a proportion factor that applies to the minimum unit subdivision specified on the line connected to the key point NPT. Used for adaptive grid subdivision. Only used when SIZE and FACT1 inputs are 0 or empty.
Step 3: Generate the mesh using the commands that have been defined in steps 1 and 2.
LCCAT, NL1, NL2
Connect multiple lines into a single connecting line for easier mapping of the grid. NL1 and NL2 are the line numbers to be connected, can also be ALL, P, or the name of the component.
(Note: ①For a shape with irregular boundaries and more than 4 boundary lines, mapping grid division cannot be used without any processing. ②The lines connected by this command are only used for grid division and cannot be used for any other purposes. The lines and the face containing the connecting lines cannot participate in any other operational commands of the solid model.)
ACCAT, NA1, NA2
Connect multiple faces into a single face for easier mapping of the grid.
LMESH, NL1, NL2, NINC
Divide a group of lines into a grid.
NINC is the increment, default is 1.
AMESH, NA1, NA2, NINC
Divide a group of faces into a grid.
VMESH, NV1, NV2, NINC
Divide a group of solids into a grid.