ansys v12与v11sp1比较单元增减情况
增加的单元有：MPC184-Screw、CPT212、CPT213、CPT215、CPT216、CPT217、SOLID236、SOLID237、REINF264、SOLID272、SOLID273、PIPE288 、PIPE289、ELBOW290 和USER300 。
去除的单元有： SOLID46、VISCO88、VISCO89、SHELL91、SHELL93、SHELL99、VISCO106、VISCO107和VISCO108。 MPC184-Screw -- The screw joint element is a two-node element that allows a relative rotation around the screw axis as well as a relative displacement along the axis of the screw, similar to the cylindrical joint. The pitch of the screw relates the relative rotation angle (around the cylindrical or screw axis) to the relative displacement along the axis of the screw.
CPT212 -- This 2-D four-node coupled pore-pressure mechanical solid element has bilinear displacement behavior. The element has four nodes with three degrees of freedom at each node: translations in the nodal x and y directions, and one pore-pressure degree of freedom at each node.
CPT213 -- This 2-D eight-node coupled pore-pressure mechanical solid has quadratic displacement behavior. The element has eight nodes with two degrees of freedom at each node: translations in the nodal x and y directions, and one pore-pressure degree of freedom at each corner node.
CPT215 -- This 3-D eight-node coupled pore-pressure mechanical solid has eight nodes with three degrees of freedom at each node: translations in the nodal x, y, and z directions, and one pore-pressure degree at each corner node.
CPT216 -- This 3-D 20-node coupled pore-pressure mechanical solid is a higher-order version of CPT215.
CPT217 -- This 3-D 10-node coupled pore-pressure mechanical solid is a higher-order version of CPT213.
SOLID236 -- This 3-D 20-node electromagnetic solid is applicable to low-frequency magnetic field analyses: static, time-harmonic and time-transient. The element has 12 magnetic edge-flux degrees of freedom (AZ) associated with the midside nodes and 20 electric potential degrees of freedom (VOLT) at each element node. It can be degenerated into a pyramid, prism, or tetrahedron.
SOLID237 -- This 3-D 10-node electromagnetic solid is a tetrahedral-shaped version of SOLID236.
REINF264 -- Use this discrete reinforcing element with standard 3-D solid and shell elements (referred to as the base elements) to provide extra reinforcing to those elements. The element is suitable for simulating reinforcing fibers with arbitrary orientations.
SOLID272 -- Use this general axisymmetric solid element to model axisymmetric solid structures. It is defined by four nodes on the master plane, and nodes created based on the circumferential direction of the four nodes. The total number of nodes depends on the number of node planes (KEYOPT(2)). Each node has three degrees of freedom: translations in the nodal x, y and z directions. The element allows a triangle as the shape on the base plane to simulate irregular areas. The element has plasticity, hyperelasticity, stress-stiffening, large-deflection, and large-strain capabilities. It also has mixed-formulation capability for simulating deformations of nearly incompressible elastoplastic materials, and fully incompressible hyperelastic materials.
SOLID273 -- Use this general axisymmetric solid element to model axisymmetric solid structures. The element has quadratic displacement behavior on the master plane and is well suited to modeling irregular meshes on the master plane. It is defined by eight nodes on the master plane, and nodes created based on the circumferential direction of the four nodes. The total number of nodes depends on the number of node planes (KEYOPT(2)). Each node has three degrees of freedom: translations in the nodal x, y and z directions. The element allows a triangle as the shape on the base plane to simulate irregular areas. The element has plasticity, hyperelasticity, stress-stiffening, large-deflection, and large-strain capabilities. It also has mixed-formulation capability for simulating deformations of nearly incompressible elastoplastic materials, and fully incompressible hyperelastic materials.
SOLID285 -- This lower-order 3-D, four-node mixed u-P element has a linear displacement and hydrostatic pressure behavior. The element is suitable for modeling irregular meshes and general materials (including incompressible materials).
PIPE288 -- This 3-D linear (two-node) finite strain pipe element is suitable for analyzing slender to moderately stubby/thick pipe structures. Internal fluid and external insulation are supported. Added mass, hydraulic added mass, and hydrodynamic and buoyant loading, are available via the new ocean family of commands.
PIPE289 -- This 3-D quadratic (three-node) finite strain pipe element is suitable for analyzing slender to moderately stubby/thick pipe structures. Internal fluid and external insulation are supported. Added mass, hydraulic added mass, and hydrodynamic and buoyant loading, are available via the new ocean family of commands.
ELBOW290 -- This 3-D quadratic finite strain pipe is suitable for analyzing pipe structures with an initially circular cross-section and a thin to moderately thick pipe wall. The element accounts for cross-section distortion, which can be commonly observed in curved pipe structures under loading. The following elements have been enhanced in this release:
COMBIN14 -- This spring-damper element now supports a preload defined via an initial length (real constant ILENGTH) or an initial force (real constant IFORCE) input. This preload is applicable to 2-D and 3-D springs only.
HF119 and HF120 -- New material property options are available for these high-frequency elements using the TB command. You can now specify frequency-dependent lossy dielectric properties (TB,HFFDLD) and anisotropic electric and magnetic loss tangents (TB,LSEM) in a TB table.
PLANE121 and PLANE230 -- A thickness input option (KEYOPT(3) =3) is now available for these electrostatic solid and electric solid elements.
TARGE169 and TARGE170 -- These target elements now support a new POINT target segment. This segment type can be defined on a rigid body where no predefined node exists and can be used to apply boundary conditions (point loads, displacement constraints, etc.) at that point. In addition, you can now use the KEYOPT(2) = 1 setting to apply boundary conditions on any rigid target nodes rather than only on the pilot node.
TARGE169, TARGE170, CONTA171, CONTA172, CONTA173, CONTA174 -- These contact and target elements now support a fluid pressure penetration load that models surrounding fluid or air penetrating into the contact interface. The load is applied via the SFE command. Additional input is supplied via the new KEYOPT(14) and two new real constants on the contact elements. KEYOPT(14) controls how the load is applied, and real constants PPCN and FPAT specify a pressure penetration criterion and a fluid penetration acting time.
TARGE170 -- This target element has a new option for shell-solid assemblies (KEYOPT(5) = 5) that improves the stress distribution at the shell-solid interface for this assembly type.
CONTA171, CONTA172, CONTA173, CONTA174, CONTA175, CONTA176, CONTA177, and CONTA178 -- These contact elements now support user-defined friction via the userfric subroutine.
LINK180 – This 3-D spar element now supports tension-only (cable) and compression-only (gap) options (specified via the third real constant). The element also offers new options (via KEYOPT(15)) for specifying the results file output; you can store averaged results at each section corner node (the default behavior), or you can store non-averaged results at each section integration point.
SHELL181, SHELL208, SHELL209, and SHELL281-- These structural and axisymmetric shell elements have a new nonlinear thickness-update algorithm that accounts for actual material properties. This option also improves convergence in general. You also have the option of using the legacy algorithm for thickness updating, which is based on preserving the element volume.
MPC184 -- The hysteretic friction capability for MPC184 joint elements has been removed in lieu of the Coulomb friction model.
BEAM188 -- This 3-D two-node beam element is used for analyzing slender to moderately stubby/thick beam structures. The element offers a new cubic option (KEYOPT(3) = 3) that uses cubic shape functions for all displacement and rotation degrees of freedom, and is capable of representing quadratically varying bending moments accurately. It offers superior accuracy over the linear (KEYOPT(3) = 0) or the quadratic (KEYOPT(3) = 2) options, particularly when higher-order element interpolations are desired. The element also offers new options (via KEYOPT(15)) for specifying the results file output; you can store averaged results at each section corner node (the default behavior), or you can store non-averaged results at each section-integration point.
BEAM189 -- This 3-D three-node beam element is also used for analyzing slender to moderately stubby/thick beam structures. The element now offers options (via KEYOPT(15)) for specifying the results file output. You can store averaged results at each section corner node (the default behavior), or you can store non-averaged results at each section integration point.
INTER192, INTER193, INTER194, INTER195 – Now by default, these elements are capable of both through-thickness and transverse-shear deformations (KEYOPT(2) = 1). Also by default, INTER193 and INTER194 adopt a full integration scheme (KEYOPT(4) = 2). The full-integration scheme and the inclusion of transverse-shear stiffness are generally required when the interfaces between the gasket and the mating parts are modeled as sliding contact.
PLANE223, SOLID226, and SOLID227 -- New material property options are available for these coupled-field elements using the TB and MP commands. Elastic properties (TB,ELASTIC) and structural damping (TB,SDAMP) are available for analyses with structural degrees of freedom. Electrical resistivities (MP,RSVX ) (also RSVY and RSVZ) are available for piezoelectric and thermal-piezoelectric analyses. These coupled-field elements now also support prestress effects in piezoelectric and structural-thermal analyses..
SHELL281 -- This eight-node shell element now offers an improved shell-formulation, activated via KEYOPT(2) = 1). Use this option for curved shell simulation, especially when thickness strain is significant or when material anisotropy in the thickness direction cannot be ignored.
页:
[1]