김경종
15 KiB
Use the following option to invoke the incompressible hybrid formulation:
*USER MATERIAL, TYPE=MECHANICAL,
CONSTANTS=number_of_constants,
HYBRID FORMULATION=INCOMPRESSIBLE
Abaqus/CAE Usage: Specification of the hybrid formulation is not supported in Abaqus/CAE.
Material state
Many mechanical constitutive models require the storage of solution-dependent state variables (plastic strains, “back stress,” saturation values, etc. in rate constitutive forms or historical data for theories written in integral form). You should allocate storage for these variables in the associated material definition (see “Allocating space” in “User subroutines: overview,” Section 18.1.1). There is no restriction on the number of state variables associated with a user-defined material.
The user material subroutines are provided with the material state at the start of each increment, as described below. They must return values for the new stresses and the new internal state variables. State variables associated with UMAT and VUMAT can be output to the output database file (.odb) and results file (.fil) using the output identifiers SDV and SDVn (see “Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2).
Material state in Abaqus/Standard
User subroutine UMAT is called for each material point at each iteration of every increment. It is provided with the material state at the start of the increment (stress, solution-dependent state variables, temperature, and any predefined field variables) and with the increments in temperature, predefined state variables, strain, and time.
In addition to updating the stresses and the solution-dependent state variables to their values at the end of the increment, subroutine UMAT must also provide the material Jacobian matrix, \partial \triangle \sigma / \partial \triangle \varepsilon . , for the mechanical constitutive model. This matrix will also depend on the integration scheme used if the constitutive model is in rate form and is integrated numerically in the subroutine. For any nontrivial constitutive model these will be challenging tasks. For example, the accuracy with which the Jacobian matrix is defined will usually be a major determinant of the convergence rate of the solution and, therefore, will have a strong influence on computational efficiency.
If you specify the viscoelastic behavior of materials in the frequency domain, user subroutine UMAT must also provide the damping (loss modulus) contribution to the material Jacobian matrix, in addition to the stiffness (storage modulus) contribution.
Material state in Abaqus/Explicit
User subroutine VUMAT is called for blocks of material points at each increment. When the subroutine is called, it is provided with the state at the start of the increment (stress, solution-dependent state variables). It is also provided with the stretches and rotations at the beginning and the end of the increment. The VUMAT user material interface passes a block of material points to the subroutine on each call, which allows vectorization of the material subroutine.
The temperature is provided to user subroutine VUMAT at the start and the end of the increment. The temperature is passed in as information only and cannot be modified, even in a fully coupled thermalstress analysis. However, if the inelastic heat fraction is defined in conjunction with the specific heat and conductivity in a fully coupled thermal-stress analysis in Abaqus/Explicit, the heat flux due to inelastic energy dissipation will be calculated automatically. If the VUMAT user subroutine is used to define an adiabatic material behavior (conversion of plastic work to heat) in an explicit dynamics procedure, you must specify both the inelastic heat fraction and the specific heat for the material, and you must store the temperatures and integrate them as user-defined state variables. Most often the temperatures are provided by specifying initial conditions (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1) and are constant throughout the analysis.
Deleting elements from a mesh using state variables
Element deletion in a mesh can be controlled during the course of an Abaqus analysis through user subroutine VUMAT or UMAT. Deleted elements have no ability to carry stresses and, therefore, have no contribution to the stiffness of the model. You specify the state variable number controlling the element deletion flag. For example, specifying a state variable number of 4 indicates that the fourth state variable is the deletion flag in the user subroutine. The deletion state variable should be set to a value of one or zero. A value of one indicates that the material point is active, while a value of zero indicates that Abaqus should delete the material point from the model by setting the stresses to zero. In Abaqus/Explicit the structure of the block of material points passed to user subroutine VUMAT remains unchanged during the analysis; deleted material points are not removed from the block. Abaqus/Explicit will pass zero stresses and strain increments for all deleted material points. Once a material point has been flagged as deleted, it cannot be reactivated. An element will be deleted from the mesh only after all of the material points in the element are deleted. The status of an element can be determined by requesting output of the variable STATUS. This variable is equal to one if the element is active and equal to zero if the element is deleted.
Input File Usage: *DEPVAR, DELETE=variable number
Abaqus/CAE Usage: Property module: material editor: General→Depvar: Variable number controlling element deletion: variable number
Hourglass control and transverse shear stiffness
Normally the default hourglass control stiffness for reduced-integration elements in Abaqus/Standard and the transverse shear stiffness for shell, pipe, and beam elements are defined based on the elasticity associated with the material (“Section controls,” Section 27.1.4; “Shell section behavior,” Section 29.6.4; and “Choosing a beam element,” Section 29.3.3). These stiffnesses are based on a typical value of the initial shear modulus of the material, which may, for example, be given as part of an elastic material behavior (“Linear elastic behavior,” Section 22.2.1) included in the material definition. However, the shear modulus is not available during the preprocessing stage of input for materials defined with user subroutine UMAT or VUMAT. Therefore, you must provide the hourglass stiffness parameters (see “Methods for suppressing hourglass modes” in “Section controls,” Section 27.1.4) when using UMAT to define the material behavior of elements with hourglassing modes; and you must specify the transverse shear stiffness (see “Choosing a beam element,” Section 29.3.3, or “Shell section
behavior,” Section 29.6.4) when using UMAT or VUMAT to define the material behavior of beams and shells with transverse shear flexibility.
Use of UMAT with other subroutines
Various utility subroutines are also available in Abaqus/Standard for use with subroutine UMAT. These utility subroutines are discussed in “Obtaining stress invariants, principal stress/strain values and directions, and rotating tensors in an Abaqus/Standard analysis,” Section 2.1.11 of the Abaqus User Subroutines Reference Guide.
User subroutine UMATHT can be used in conjunction with UMAT to define the constitutive thermal behavior of the material. The solution-dependent variables allocated in the material definition are accessible in both UMAT and UMATHT. In addition, user subroutines FRIC, GAPCON, and GAPELECTR are available for defining mechanical, thermal, and electrical interactions between surfaces.
Use with other material models
A number of material behaviors can be used in the definition of a material when its mechanical behavior is defined by user subroutine UMAT or VUMAT. These behaviors include density, thermal expansion, permeability, and heat transfer properties. Thermal expansion can alternatively be an integral part of the constitutive model implemented in UMAT or VUMAT.
The temperature available in UMAT is always the interpolated temperature field at the element integration points. Naturally, if the thermal expansion behavior is implemented in UMAT, it is defined in terms of the integration point temperature. When the temperature field is interpolated differently within an element compared to the displacement field in Abaqus/Standard, implementing the thermal expansion behavior in UMAT may lead to differences compared to the built-in thermal expansion behavior. This situation commonly arises for coupled temperature-displacement elements. For example, for first-order coupled temperature-displacement elements, the built-in thermal expansion behavior uses a constant temperature field over the whole element (see “Fully coupled thermal-stress analysis,” Section 6.5.3), while the behavior in UMAT will be defined in terms of a linear temperature field.
For a material defined by user subroutine UMAT or VUMAT, mass proportional damping can be included separately (see “Material damping,” Section 26.1.1), but stiffness proportional damping must be defined in the user subroutine by the Jacobian (Abaqus/Standard only) and stress definitions. Stiffness proportional damping cannot be specified if the user material is used in the direct steady-state dynamics procedure.
Elements
User subroutines UMAT and VUMAT can be used with all elements in Abaqus that include mechanical behavior (elements that have displacement degrees of freedom).
26.7.2 USER-DEFINED THERMAL MATERIAL BEHAVIOR
Products: Abaqus/Standard Abaqus/CAE
References
• “UMATHT,” Section 1.1.45 of the Abaqus User Subroutines Reference Guide
• *USER MATERIAL
• *DEPVAR
• “Defining constants for a user material,” Section 12.8.4 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
Overview
User-defined thermal material behavior in Abaqus/Standard:
• is provided by means of an interface whereby any thermal constitutive model can be added to the library;
• requires that a constitutive model (or a library of models) is programmed in user subroutine UMATHT; and
• requires considerable effort and expertise: the feature is very general and powerful, but its use is not a routine exercise.
Material constants
Any material constants that are needed in user subroutine UMATHT must be specified as part of a userdefined thermal material behavior definition. Any other thermal material behaviors included in the same material definition will be ignored: the user-defined thermal material behavior requires that all thermal behavior calculations are programmed in user subroutine UMATHT.
Input File Usage: *USER MATERIAL, TYPE=THERMAL, CONSTANTS=number_of_constants
You must specify the number of constants being entered.
Abaqus/CAE Usage: Property module: material editor: General→User Material: User material type: Thermal
Unsymmetric equation solver
When the conductivity is defined in user subroutine UMATHT as a strong function of temperature, the heat transfer equilibrium equations become nonsymmetric and you may choose to invoke the unsymmetric equation solution capability; otherwise, convergence may be poor.
Input File Usage: *USER MATERIAL, TYPE=THERMAL, CONSTANTS=number_of_constants, UNSYMM
Abaqus/CAE Usage: Property module: material editor: General→User Material: User material type: Thermal, toggle on Use unsymmetric material stiffness matrix
Material state
Many thermal constitutive models require the storage of solution-dependent state variables. These state variables might include microstructure or phase content information when the material undergoes phase changes. You should allocate storage for these variables in the associated material definition (see “Allocating space” in “User subroutines: overview,” Section 18.1.1). There is no restriction on the number of state variables associated with a user-defined material.
User subroutine UMATHT is called for each material point at each iteration of every increment. It is provided with the thermal state of the material at the start of the increment (solution-dependent state variables, temperature, and any predefined field variables) and with the increments in temperature, predefined state variables, and time.
Required calculations
Subroutine UMATHT must perform the following functions: it must define the internal energy per unit mass and its variation with temperature and spatial gradients of temperature; it must define the heat flux vector and its variation with respect to temperature and spatial gradients of temperature; and it must update the solution-dependent state variables to their values at the end of the increment. The components of the heat flux and spatial gradients in user subroutine UMATHT are in directions that depend on the use of local orientations (see “Orientations,” Section 2.2.5).
Use with other user subroutines
User subroutine UMAT can be used in conjunction with UMATHT to define the constitutive mechanical behavior of the material. The solution-dependent variables allocated in the material definition are accessible in both UMATHT and UMAT. In addition, user subroutines FRIC, GAPCON, and GAPELECTR are available for defining mechanical, thermal, and electrical interactions between surfaces.
Use with other material models
Density, mechanical properties, and electrical properties can be included in the definition of a material whose constitutive thermal behavior is defined by user subroutine UMATHT.
Elements
User subroutine UMATHT can be used with all elements in Abaqus/Standard that include thermal behavior (elements with temperature degrees of freedom such as pure heat transfer, coupled thermal-stress, and coupled thermal-electrical elements).
About SIMULIA
Dassault Systèmes SIMULIA applications, including Abaqus, Isight, Tosca, and Simulation Lifecycle Management, enable users to leverage physics-based simulation and high-performance computing to explore real-world behavior of products, nature, and life. As an integral part of Dassault Systèmes’ 3DEXPERIENCE platform, SIMULIA applications accelerate the process of making highly informed, mission-critical design and engineering decisions before committing to costly and time-consuming physical prototypes. www.3ds.com/simulia
Our 3DEXPERIENCE Platform powers our brand applications, serving 12 industries, and provides a rich portfolio of industry solution experiences.
Dassault Systèmes, the 3DEXPERIENCE Company, provides business and people with virtual universes to imagine sustainable innovations. Its world-leading solutions transform the way products are designed, produced, and supported. Dassault Systèmes’ collaborative solutions foster social innovation, expanding possibilities for the virtual world to improve the real world. The group brings value to over 170,000 customers of all sizes in all industries in more than 140 countries. For more information, visit www.3ds.com.
flowchart
Circular diagram illustrating the integration of 3D modeling apps, information intelligence apps, and simulation apps, with associated platform icons and labels.