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 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. 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 “Execution procedure for ABAQUS/Standard and ABAQUS/Explicit,” Section 3.2.2).

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 “Execution procedure for ABAQUS/Standard and ABAQUS/Explicit,” Section 3.2.2).

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,” Section 10.3.2) 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 . 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.

*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

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 10.3.1–1.

To define a periodic model with a constant angle, you must specify the coordinates of points a and b shown in Figure 10.3.1–2 to define the symmetry axis. You then define the segment angle, (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, you specify the coordinates of points a and b shown in Figure 10.3.1–2 to define the symmetry axis. You then define the segment angle, (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 10.3.1–3, 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.

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% of the typical element size in the surfaces of the original sector.

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,” Section 28.3.1) when revolving the original sector about the symmetry axis to create a periodic model. The first surface of each specified pair is the slave surface, and all degrees of freedom of the nodes in the surface will be eliminated by internally generated multi-point constraints.

*SURFACE, NAME=master
*SURFACE, NAME=slave

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

*SYMMETRIC MODEL GENERATION, PERIODIC=VARIABLE
ax, ay, az, bx, by, bz
θ, N
M, f
slave, master, 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,” Section 2.2.5), 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

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