Symmetric Model Generation

Duplicate nodes will be generated in certain situations. Such nodes can be eliminated to ensure that the mesh is connected properly. Duplicate nodes can be generated on the axis of revolution of a revolved model, on the connection planes between sectors of a periodic model, and on the connection plane between the two parts of a reflected model. You can specify the tolerance distance, d, to be used in the search for duplicate nodes. The default distance is 1.0% of the average element dimension. In some cases a tolerance distance that is smaller than the default value needs to be specified if, for example, the distance between two nodes on one of the connection planes in the original sector of a periodic model is smaller than the default tolerance distance. Closely spaced nodes elsewhere in the model, such as between interface surfaces or on parts of the model that are generated with any of the other model definition options, will not be eliminated.

SYMMETRIC MODEL GENERATION, PERIODIC, TOLERANCE=d
SYMMETRIC MODEL GENERATION, REVOLVE, TOLERANCE=d
SYMMETRIC MODEL GENERATION, REFLECT, TOLERANCE=d

You can specify the name of an external file (without an extension) to which the data for the new model definition will be written. The extension .axi will be added to the file name provided. The file can be edited to modify or to extend the model generated by Abaqus/Standard.

SYMMETRIC MODEL GENERATION, PERIODIC, FILE NAME=name
SYMMETRIC MODEL GENERATION, REVOLVE, FILE NAME=name
SYMMETRIC MODEL GENERATION, REFLECT,  FILE NAME=name

The symmetric model generation capability uses the restart (.res), analysis database (.stt and .mdl), and part (.prt) files from the old model to generate the new model. The name of the restart files from the old model must be specified when the new analysis is executed by using the oldjob parameter in the command for running Abaqus or by answering a request made by the command procedure (see Abaqus/Standard and Abaqus/Explicit Execution).

It is recommended that you verify the new model carefully before an analysis is performed. The symmetric model generation capability requires only information stored in the restart file during a data check run to generate the new model, which allows you to verify the new model before the analysis of the original model is performed. A data check analysis is performed by using the datacheck parameter in the command for running Abaqus (see Abaqus/Standard and Abaqus/Explicit Execution).

A local cylindrical orientation system is always used for element output of stress, strain, etc. A default local orientation definition is provided if the material in the original axisymmetric model does not contain an orientation definition. This default orientation is defined with the polar axis of the system along the axis of revolution, with an additional 90.0° rotation about the local 1-direction so that the local axes are 1=radial, 2=axial, and 3=circumferential. If shells or membranes are used, the projections of the local 2- and 3-axes onto the surface of the shell or membrane are taken as the local directions on the surface. This orientation system is always provided, even if an orientation is specified in the original axisymmetric model. However, if the results of the axisymmetric analysis are mapped onto the new three-dimensional model (see Transferring Results from a Symmetric Mesh or a Partial Three-Dimensional Mesh to a Full Three-Dimensional Mesh) and an orientation definition is associated with the material in the original model, the original orientation revolved about the axis of symmetry replaces this default orientation definition.

You can define the increments in numbers between each node and element around the circumference of the three-dimensional model. The numbering starts at the reference cross-section $\theta ={0.0}^{\circ }$. The reference cross-section uses the same numbering as the original axisymmetric model. The defaults are the largest node and element numbers used in the original axisymmetric model. Control over the numbering allows you to define additional parts of the model without the risk of conflicting element and node labels. Each offset value should be greater than or equal to the maximum node or element label, respectively, used in the original model. When specifying the offset value, care must be taken that the generated node or element does not exceed the maximum value allowed, which is 999,999,999.

SYMMETRIC MODEL GENERATION, REVOLVE, NODE OFFSET=offset, ELEMENT OFFSET=offset

The element type used in the original two-dimensional model determines the element type in the new three-dimensional model. You can specify whether the new element should be either a general three-dimensional element or a cylindrical element. General and cylindrical elements can be used in the same model.

Regular axisymmetric elements (CAX), axisymmetric elements with twist (CGAX), shell elements, membrane elements, rigid elements, and surface elements can be used in the two-dimensional model; however, nonlinear axisymmetric elements (CAXA) cannot be used. A two-dimensional model that contains incompatible mode elements; first-order, reduced-integration, continuum elements; shell elements; or rigid elements cannot be used to generate cylindrical elements. The correspondence between the axisymmetric element type and the equivalent three-dimensional element type (general or cylindrical) is shown in Table 1.

SYMMETRIC MODEL GENERATION, REVOLVE
coordinates of points a and b
coordinates of point c
segment angle, number of elements per segment, bias ratio, CYLINDRICAL or GENERAL

SYMMETRIC MODEL GENERATION, REVOLVE
ax, ay, az, bx, by, bz
cx, cy, cz
300.0, 4, 1.0, CYLINDRICAL
60.0, 10, 1.0, GENERAL

• First- and second-order elements cannot be used together in the axisymmetric model.

• Nonaxisymmetric elements such as springs, dashpots, beams, and trusses will be ignored in the model generation.

• Only surface-based contact pairs can be revolved. Models using general contact cannot be revolved. Contact conditions modeled with contact elements will be ignored in the model generation.

• A two-dimensional model that includes incompatible mode elements; first-order, reduced-integration, continuum elements; shell elements; or rigid elements cannot be used to generate cylindrical elements.

• Rebar with nonuniform spacing in the radial direction of an axisymmetric element cannot be revolved.

• Most types of kinematic constraints cannot be revolved. However, surface-based constraints (Mesh Tie Constraints) and embedded element constraints (Embedded Elements) defined in the original model will be generated automatically in the new three-dimensional model.

• Only stress/displacement, heat transfer, coupled temperature-displacement, and acoustic elements can be revolved.

• Spatially varying fields defined using distributions (Distribution Definition) cannot be revolved.

To define a periodic model with a constant angle, you must specify the coordinates of points a and b shown in Figure 2 to define the symmetry axis. You then define the segment angle, $\theta$ (in degrees), of the original sector and the number of three-dimensional repetitive sectors, N, including the original sector, in the generated periodic model.

SYMMETRIC MODEL GENERATION, PERIODIC=CONSTANT
coordinates of points a and b
θ, N

To define a periodic model with a variable angle, the surfaces on both sides of the original sector must be completely planar. You specify the coordinates of points a and b shown in Figure 2 to define the symmetry axis. You then define the segment angle, $\theta$ (in degrees), of the original sector and the number of three-dimensional repetitive sectors, N, including the original sector, in the generated periodic model. Next, you specify an additional number of three-dimensional sectors to be generated, M, and the angular scaling factor, f, in the circumferential direction with respect to the original sector to be applied to these additional sectors. You can define pairs of additional sectors and scaling factors as needed.

SYMMETRIC MODEL GENERATION, PERIODIC=VARIABLE
coordinates of points a and b
θ, N
M1, f1
M2, f2
Etc.

SYMMETRIC MODEL GENERATION, PERIODIC=VARIABLE
ax, ay, az, bx, by, bz
20.0,2
3,1.5
2,2.0

If the symmetric surfaces in the original sector have precisely matched meshes, as shown in Figure 3, any duplicate nodes that are generated will be eliminated automatically to ensure that the mesh is connected properly between the neighboring sectors when revolving the original sector about the symmetry axis to create a periodic model.

Figure 3. Surfaces with precisely matching meshes on the original sector.

In all other cases you must define one or more pairs of corresponding surfaces on each side of the original sector (see About Surfaces) in the original model and specify the pairs of corresponding surfaces in the symmetric model generation definition.

Optionally, you can also specify the tolerance distance within which nodes on one surface of a sector must lie from the corresponding surface of the neighboring sector to be constrained. Nodes on the surface of the sector that are further away from the corresponding surface of the neighboring sector than this distance are not constrained. The default value for the tolerance distance is 5% or 10% of the typical element size in the surfaces of the original sector, depending on whether node-to-surface or surface-to-surface type constraints are used, respectively.

You can also specify whether surface-to-surface (default) or node-to-surface constraints should be used. Constraints between the automatically generated neighboring pairs of corresponding surfaces are then applied with an automatically generated surface-based tie constraint (Mesh Tie Constraints) when revolving the original sector about the symmetry axis to create a periodic model. The first surface of each specified pair is the secondary surface, and all degrees of freedom of the nodes in the surface will be eliminated by internally generated multi-point constraints.

SURFACE, NAME=main
SURFACE, NAME=secondary

SYMMETRIC MODEL GENERATION, PERIODIC=CONSTANT
ax, ay, az, bx, by, bz
θ, N
secondary, main, tolerance distance, SURFACE or NODE

SYMMETRIC MODEL GENERATION, PERIODIC=VARIABLE
ax, ay, az, bx, by, bz
θ, N
M, f
secondary, main, tolerance distance, SURFACE or NODE

A local cylindrical orientation system is always used for element output of stress, strain, etc. If an orientation is specified in the original three-dimensional sector (see Orientations), the orientation system in the new model is defined by revolving the original orientation system about the symmetry axis. If shells or membranes are used, the projections of the local 2- and 3-axes onto the surface of the shell or membrane are taken as the local directions on the surface. If the material in the original three-dimensional sector does not contain an orientation definition, a default local orientation definition is provided. This default orientation is defined by revolving the global coordinate system in the original model about the axis of symmetry in the new model.

You can define the increments in numbers between each node and element around the circumference of the three-dimensional model. The numbering starts at the original three-dimensional repetitive sector. The original three-dimensional repetitive sector uses the same numbering as the original model. The defaults are the largest node and element numbers used in the original model. Control over the numbering allows you to define additional parts of the model without the risk of conflicting element and node labels. Each offset value should be greater than or equal to the maximum node or element label, respectively, used in the original model. When specifying the offset value, care must be taken that the generated node or element does not exceed the maximum value allowed, which is 999,999,999.

SYMMETRIC MODEL GENERATION, PERIODIC, 
NODE OFFSET=offset, ELEMENT OFFSET=offset

• Only surface-based contact pairs can be revolved. Models using general contact cannot be revolved. Contact conditions modeled with contact elements will be ignored in the model generation.

• Most types of kinematic constraints cannot be revolved. However, surface-based constraints (Mesh Tie Constraints) and embedded element constraints (Embedded Elements) defined in the original model will be generated automatically in the new three-dimensional model. One exception is that surface-based ties for enforcing cyclic symmetric constraints are not revolved.

• Surface-based distributed coupling constraints—e.g., couplings (Coupling Constraints), shell-to-solid couplings (Shell-to-Solid Coupling), and fasteners (Mesh-Independent Fasteners)—cannot be revolved and must be redefined.

• Only stress/displacement, heat transfer, coupled temperature-displacement, and acoustic elements can be revolved. Beam and frame elements cannot be revolved.

• Spatially varying fields defined using distributions (Distribution Definition) cannot be revolved.

You can specify constants that must be added to the original node and element numbers for numbering the reflected part of the three-dimensional model. The defaults are the maximum node and element numbers used in the original model. Control over the numbering allows you to define additional parts of the model without the risk of conflicting element and node labels.

SYMMETRIC MODEL GENERATION, REFLECT, 
NODE OFFSET=offset, ELEMENT OFFSET=offset

• Only surface-based contact pairs can be reflected. Models using general contact cannot be reflected. Contact conditions modeled with contact elements will be ignored in the model generation.

• You must ensure that main surfaces remain continuous after reflection. A discontinuous surface is created when the surface in the original model does not intersect the connection plane between the two parts of the symmetric structure.

• Rigid surfaces cannot be reflected. The rigid surface definition of the original model is simply repeated in the new model. You must, therefore, specify the complete rigid surface in the original model.

• Most types of kinematic constraints cannot be reflected. However, surface-based constraints (Mesh Tie Constraints) and embedded element constraints (Embedded Elements) defined in the original model will be generated automatically in the new three-dimensional model.

• Only stress/displacement, heat transfer, coupled temperature-displacement, and acoustic elements can be reflected.

• Nonaxisymmetric elements such as springs, dashpots, beams, and trusses cannot be reflected.

• Spatially varying fields defined using distributions (Distribution Definition) cannot be reflected.