김경종
23 KiB
Accounting for frictional slip heat generation
Frictional slip heat generation is normally neglected in the steady-state case. However, it can still be accounted for if motions are used to specify translational or rotational nodal velocities in disk brake-type problems or if user subroutine FRIC provides the incremental frictional dissipation through the variable SFD. If frictional heat generation is present, the heat flux into the two contact surfaces depends on the slip rate of the surfaces. The “time” scale in this case cannot be described as arbitrary, and a transient analysis should be performed.
Transient analysis
Alternatively, you can perform a transient coupled thermal-electrical-structural analysis. As in steadystate analysis, electrical transient effects are neglected and a static displacement solution is assumed. You can control the time incrementation in a transient analysis directly, or Abaqus/Standard can control it automatically. Automatic time incrementation is generally preferred.
Automatic incrementation controlled by a maximum allowable temperature change
The time increments can be selected automatically based on a user-prescribed maximum allowable nodal temperature change in an increment, \Delta \theta _ { m a x } . Abaqus/Standard will restrict the time increments to ensure that this value is not exceeded at any node (except nodes with boundary conditions) during any increment of the analysis (see “Time integration accuracy in transient problems,” Section 7.2.4).
Input File Usage: *COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL, DELTMX=
Abaqus/CAE Usage: Step module: Create Step: General: Coupled thermal-electricalstructural: Basic: Response: Transient; Incrementation: Type: Automatic: Max. allowable temperature change per increment: \Delta \theta _ { m a x }
Fixed incrementation
If you do not specify \Delta \theta _ { m a x } , fixed time increments equal to the user-specified initial time increment, \Delta t _ { 0 } , will be used throughout the analysis.
Input File Usage: *COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL \Delta t _ { 0 }
Abaqus/CAE Usage: Step module: Create Step: General: Coupled thermal-electricalstructural: Basic: Response: Transient; Incrementation: Type: Fixed: Increment size: \Delta t _ { 0 }
Spurious oscillations due to small time increments
In transient analysis with second-order elements there is a relationship between the minimum usable time increment and the element size. A simple guideline is
\Delta t > \frac {\rho c}{6 k} \Delta \ell^ {2},
where \Delta t is the time increment, is the density, c is the specific heat, k is the thermal conductivity, and \Delta \ell is a typical element dimension (such as the length of a side of an element). If time increments smaller than this value are used in a mesh of second-order elements, spurious oscillations can appear in the solution, in particular in the vicinity of boundaries with rapid temperature changes. These oscillations are nonphysical and may cause problems if temperature-dependent material properties are present. In transient analyses using first-order elements the heat capacity terms are lumped, which eliminates such oscillations but can lead to locally inaccurate solutions for small time increments. If smaller time increments are required, a finer mesh should be used in regions where the temperature changes rapidly.
There is no upper limit on the time increment size (the integration procedure is unconditionally stable) unless nonlinearities cause convergence problems.
Automatic incrementation controlled by the creep response
The accuracy of the integration of time-dependent (creep) material behavior is governed by the user-specified accuracy tolerance parameter, . This parameter is used \geq ( \dot { \bar { \varepsilon } } _ { t + \Delta t } ^ { c r } - \dot { \bar { \varepsilon } } _ { t } ^ { c r } ) \Delta t to prescribe the maximum strain rate change allowed at any point during an increment, as described in “Rate-dependent plasticity: creep and swelling,” Section 23.2.4. The accuracy tolerance parameter can be specified together with the maximum allowable nodal temperature change in an increment, \Delta \theta _ { m a x } (described above); however, specifying the accuracy tolerance parameter activates automatic incrementation even if \Delta \theta _ { m a x } is not specified.
Input File Usage: *COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL, \scriptstyle \mathrm { D E L T M X } = \Delta \theta _ { m a x } , \mathrm { C E T O L } = t o l e r a n c e
Abaqus/CAE Usage: Step module: Create Step: General: Coupled thermal-electricalstructural: Basic: Response: Transient, toggle on Include creep/swelling/viscoelastic behavior; Incrementation: Type: Automatic: Max. allowable temperature change per increment: \Delta \theta _ { m a x } , Creep/swelling/viscoelastic strain error tolerance: tolerance
Selecting explicit creep integration
Nonlinear creep problems (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4) that exhibit no other nonlinearities can be solved efficiently by forward-difference integration of the inelastic strains if the inelastic strain increments are smaller than the elastic strains. This explicit method is efficient computationally because, unlike implicit methods, iteration is not required as long as no other nonlinearities are present. Although this method is only conditionally stable, the numerical stability limit of the explicit operator is in many cases sufficiently large to allow the solution to be developed in a reasonable number of time increments.
For most coupled thermal-electrical-structural analyses, however, the unconditional stability of the backward difference operator (implicit method) is desirable. In such cases the implicit integration scheme may be invoked automatically by Abaqus/Standard.
Explicit integration can be less expensive computationally and simplifies implementation of userdefined creep laws in user subroutine CREEP; you can restrict Abaqus/Standard to using this method
for creep problems (with or without geometric nonlinearity included). See “Rate-dependent plasticity: creep and swelling,” Section 23.2.4, for further details.
Input File Usage: *COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL, CETOL=tolerance, CREEP=EXPLICIT
Abaqus/CAE Usage: Step module: Create Step: General: Coupled thermal-electricalstructural: Basic: Response: Transient, toggle on Include creep/swelling/viscoelastic behavior; Incrementation: Creep/swelling/viscoelastic strain error tolerance: tolerance, Creep/swelling/viscoelastic integration: Explicit
Excluding creep and viscoelastic response
You can specify that no creep or viscoelastic response will occur during a step even if creep or viscoelastic material properties have been defined.
Input File Usage: *COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL, DELTMX= , CREEP=NONE
Abaqus/CAE Usage: Step module: Create Step: General: Coupled thermal-electricalstructural: Basic: Response: Transient, toggle off Include creep/swelling/viscoelastic behavior
Unstable problems
Some types of analyses may develop local instabilities, such as surface wrinkling, material instability, or local buckling. In such cases it may not be possible to obtain a quasi-static solution, even with the aid of automatic incrementation. Abaqus/Standard offers a method of stabilizing this class of problems by applying damping throughout the model in such a way that the viscous forces introduced are sufficiently large to prevent instantaneous buckling or collapse but small enough not to affect the behavior significantly while the problem is stable. The available automatic stabilization schemes are described in detail in “Automatic stabilization of unstable problems” in “Solving nonlinear problems,” Section 7.1.1.
Units
In coupled problems where two or three different fields are active, take care when choosing the units of the problem. If the choice of units is such that the terms generated by the equations for each field are different by many orders of magnitude, the precision on some computers may be insufficient to resolve the numerical ill-conditioning of the coupled equations. Therefore, choose units that avoid ill-conditioned matrices. For example, consider using units of Mpascal instead of pascal for the stress equilibrium equations to reduce the disparity between the magnitudes of the stress equilibrium equations, the heat flux continuity equations, and the conservation of charge equations.
Initial conditions
By default, the initial temperature of all nodes is zero. You can specify nonzero initial temperatures. Initial stresses, field variables, etc. can also be defined; “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1, describes all of the initial conditions that are available for a fully coupled thermal-electrical-structural analysis.
Boundary conditions
Boundary conditions can be used to prescribe temperatures (degree of freedom 11), displacements/rotations (degrees of freedom 1–6), or electrical potentials (degree of freedom 9) at nodes in a fully coupled thermal-electrical-structural analysis (see “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.3.1).
Boundary conditions can be specified as functions of time by referring to amplitude curves (“Amplitude curves,” Section 34.1.2).
Loads
The following types of thermal loads can be prescribed in a fully coupled thermal-electrical-structural analysis, as described in “Thermal loads,” Section 34.4.4:
• Concentrated heat fluxes.
• Body fluxes and distributed surface fluxes.
• Node-based film and radiation conditions.
• Average-temperature radiation conditions.
• Element and surface-based film and radiation conditions.
The following types of mechanical loads can be prescribed:
• Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see “Concentrated loads,” Section 34.4.2.
• Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 34.4.3.
The following types of electrical loads can be prescribed, as described in “Electromagnetic loads,” Section 34.4.5:
• Concentrated current.
• Distributed surface current densities and body current densities.
Predefined fields
Predefined temperature fields are not allowed in a fully coupled thermal-electrical-structural analysis. Boundary conditions should be used instead to prescribe temperature degree of freedom 11, as described earlier.
Other predefined field variables can be specified in a fully coupled thermal-electrical-structural analysis. These values will affect only field-variable-dependent material properties, if any. See “Predefined fields,” Section 34.6.1.
Material options
The materials in a fully coupled thermal-electrical-structural analysis must have thermal properties (such as conductivity), mechanical properties (such as elasticity), and electrical properties (such as electrical conductivity) defined. See Part V, “Materials,” for details on the material models available in Abaqus.
Internal heat generation can be specified; see “Uncoupled heat transfer analysis,” Section 6.5.2.
Thermal strain will arise if thermal expansion (“Thermal expansion,” Section 26.1.2) is included in the material property definition.
A fully coupled thermal-electrical-structural analysis can be used to analyze static creep and swelling problems, which generally occur over fairly long time periods (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4); viscoelastic materials (“Time domain viscoelasticity,” Section 22.7.1); or viscoplastic materials (“Rate-dependent yield,” Section 23.2.3).
Inelastic energy dissipation as a heat source
You can specify an inelastic heat fraction in a fully coupled thermal-electrical-structural analysis to provide for inelastic energy dissipation as a heat source. The heat flux per unit volume, r ^ { p l } , that is added into the thermal energy balance is computed using the equation
r ^ {p l} = \eta \pmb {\sigma}: \dot {\pmb {\varepsilon}} ^ {p l},
or, in the case when the nonlinear isotropic/kinematic hardening model is used, from the following equation:
r ^ {p l} = \eta (\pmb {\sigma} - \pmb {\alpha}): \dot {\pmb {\varepsilon}} ^ {p l},
where is a user-defined factor (assumed constant), is the stress, is the backstress, and \dot { \varepsilon } ^ { p l } is the rate of plastic straining.
Inelastic heat fractions are typically used in the simulation of high-speed manufacturing processes involving large amounts of inelastic strain, where the heating of the material caused by its deformation significantly influences temperature-dependent material properties. The generated heat is treated as a volumetric heat flux source term in the heat balance equation.
An inelastic heat fraction can be specified for materials with plastic behavior that use the Mises or Hill yield surface (“Inelastic behavior,” Section 23.1.1). It cannot be used with the combined isotropic/kinematic hardening model. The inelastic heat fraction can be specified for user-defined material behavior in Abaqus/Explicit and will be multiplied by the inelastic energy dissipation coded in the user subroutine to obtain the heat flux. In Abaqus/Standard the inelastic heat fraction cannot be used with user-defined material behavior; in this case the heat flux that must be added to the thermal energy balance is computed directly in the user subroutine.
In Abaqus/Standard an inelastic heat fraction can also be specified for hyperelastic material definitions that include time-domain viscoelasticity (“Time domain viscoelasticity,” Section 22.7.1).
The default value of the inelastic heat fraction is 0.9. If you do not include the inelastic heat fraction behavior in the material definition, the heat generated by inelastic deformation is not included in the analysis.
Input File Usage: *INELASTIC HEAT FRACTION
Abaqus/CAE Usage: Property module: material editor: Thermal: Inelastic Heat Fraction: Fraction:
Specifying the amount of thermal energy generated due to electrical current
Joule’s law describes the rate of electrical energy, P _ { e c } , dissipated by current flowing through a conductor as
P _ {e c} = \mathbf {J} \cdot \mathbf {E} = \frac {\partial \varphi}{\partial \mathbf {x}} \cdot \pmb {\sigma} ^ {E} \cdot \frac {\partial \varphi}{\partial \mathbf {x}}.
The amount of this energy released as internal heat within the body is \eta _ { v } P _ { e c } , , where \eta _ { v } is an energy conversion factor. You specify \eta _ { v } in the material definition. It is assumed that all the electrical energy is converted into heat ( \eta _ { v } = 1 . 0 ) if you do not include the joule heat fraction in the material description. The fraction given can include a unit conversion factor, if required.
Input File Usage: *JOULE HEAT FRACTION
Abaqus/CAE Usage: Property module: material editor: Thermal→Joule Heat Fraction
Elements
Coupled thermal-electrical-structural elements that have displacements, temperatures, and electrical potentials as nodal variables are available. Simultaneous temperature/electrical potential/displacement solution requires the use of such elements; pure displacement and temperature-displacement elements can be used in part of the model in a fully coupled thermal-electrical-structural analysis, but pure heat transfer elements cannot be used.
The first-order coupled thermal-electrical-structural elements in Abaqus use a constant temperature over the element to calculate thermal expansion. The second-order coupled thermal-electrical-structural elements in Abaqus use a lower-order interpolation for temperature than for displacement (parabolic variation of displacements and linear variation of temperature) to obtain a compatible variation of thermal and mechanical strain.
Output
See “Abaqus/Standard output variable identifiers,” Section 4.2.1, for a complete list of output variables. The types of output available are described in “Output,” Section 4.1.1.
Considerations for steady-state coupled thermal-electrical-structural analysis
In a steady-state coupled thermal-electrical-structural analysis the electrical energy dissipated due to flow of electrical current at an integration point (output variable JENER) is computed using the following relationship:
E _ {e c} = P _ {e c} t _ {s t e p},
where E _ { e c } denotes the electrical energy dissipated due to flow of electrical current and t _ { s t e p } is the current step time. In the above relationship it is assumed that the rate of the electrical energy dissipation, P _ { e c } , has a constant value in the step that is equal to the value currently computed.
The output variable JENER and the derived output variables ELJD and ALLJD contain the values of electrical energies dissipated in the current step only. Similarly, the contribution from the electrical current flow to the output variable ALLWK includes only the external work performed in the current step.
Input file template ```txt *HEADING ... ** Specify the coupled thermal-electrical-structural element type *ELEMENT, TYPE=Q3D8 ... ** *STEP *COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL Data line to define incrementation *BOUNDARY Data lines to define nonzero boundary conditions on displacement, temperature or electrical potential degrees of freedom *CFLUX and/or *CFILM and/or *CRADIATE and/or *DFLUX and/or *DSFLUX and/or *FILM and/or *SFILM and/or *RADIATE and/or *SRADIATE Data lines to define thermal loads *CLOAD and/or *DLOAD and/or *DSLOAD Data lines to define mechanical loads *CECURRENT Data lines to define concentrated currents *DECURRENT and/or *DSECURRENT Data lines to define distributed current densities *FIELD Data lines to define field variable values *END STEP
<!-- source-page: 448 -->
<!-- source-page: 449 -->
# 6.7.5 EDDY CURRENT ANALYSIS
Products: Abaqus/Standard Abaqus/CAE
# References
• “Mapping thermal and magnetic loads,” Section 3.2.27
• “Electromagnetic analysis procedures,” Section 6.7.1
• “Electrical conductivity,” Section 26.5.1
• “Magnetic permeability,” Section 26.5.3
• “Electromagnetic loads,” Section 34.4.5
• “Predefined loads for sequential coupling,” Section 16.1.3
• \*ELECTROMAGNETIC
• \*D EM POTENTIAL
• \*DECURRENT
• \*DSECURRENT
• \*MOTION
• “UDECURRENT,” Section 1.1.24 of the Abaqus User Subroutines Reference Guide
• “UDEMPOTENTIAL,” Section 1.1.25 of the Abaqus User Subroutines Reference Guide
• “UDSECURRENT,” Section 1.1.27 of the Abaqus User Subroutines Reference Guide
• “Configuring a time-harmonic electromagnetic analysis” in “Configuring linear perturbation analysis procedures,” Section 14.11.2 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
• “Defining a magnetic vector potential boundary condition,” Section 16.10.17 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
# Overview
Eddy current problems:
• involve coupling between electric and magnetic fields, which are solved for simultaneously;
• solve Maxwell’s equations describing electromagnetic phenomena under the low-frequency assumption that neglects the effects of displacement currents;
• require the use of electromagnetic elements in the whole domain;
• require that magnetic permeability is specified in the whole domain and electrical conductivity is specified in the conducting regions;
• allow for both time-harmonic and transient electromagnetic solutions;
• allow predefined conductor translation and rotation;
<!-- source-page: 450 -->
• calculate as output variables, rate of Joule heating and intensity of magnetic body forces associated with eddy currents, and these output variables can be transferred from a time-harmonic electromagnetic solution to drive a subsequent heat transfer, coupled temperature-displacement, or stress/displacement analysis, thereby allowing for the coupling of electromagnetic fields with thermal and/or mechanical fields in a sequentially coupled manner; and
• can be solved using continuum elements in two- and three-dimensional space.
# Eddy current analysis
Eddy currents are generated in a metal workpiece when it is placed within a time-varying magnetic field. Joule heating arises when the energy dissipated by the eddy currents flowing through the workpiece is converted into thermal energy. This heating mechanism is usually referred to as induction heating; the induction cooker is an example of a device that uses this mechanism. The time-varying magnetic field is usually generated by a coil that is placed close to the workpiece. The coil carries either a known amount of total current or an unknown amount of current under a known potential (voltage) difference. The current in the coil is assumed to be alternating at a known frequency for a time-harmonic eddy current analysis but may have an arbitrary variation in time for a transient eddy current analysis.
The time-harmonic eddy current analysis procedure is based on the assumption that a time-harmonic excitation with a certain frequency results in a time-harmonic electromagnetic response with the same frequency everywhere in the domain. In other words, both the electric and the magnetic fields oscillate at the same frequency as that of the alternating current in the coil. The transient eddy current analysis does not make any assumption regarding the time-variation of the current in the coil; in fact any arbitrary time variation can be specified, and the electric and magnetic fields follow from the solution to Maxwell’s equations in the time domain.
The eddy current analysis provides output, such as Joule heat dissipation or magnetic body force intensity, that can be transferred, from a time-harmonic eddy current analysis only, to drive a subsequent heat transfer, coupled temperature-displacement, or stress/displacement analysis. This allows for modeling the interactions of the electromagnetic fields with thermal and/or mechanical fields in a sequentially coupled manner. See “Mapping thermal and magnetic loads,” Section 3.2.27, and “Predefined loads for sequential coupling,” Section 16.1.3, for details.
Electromagnetic elements must be used to model the response of all the regions in an eddy current analysis including the coil, the workpiece, and the space in between and surrounding them. To obtain accurate solutions, the outer boundary of the space (surrounding the coil and the workpiece) being modeled must be at least a few characteristic length scales away from the device on all sides.
The electromagnetic elements use an element edge-based interpolation of the fields instead of the standard node-based interpolation. The user-defined nodes only define the geometry of the elements; and the degrees of freedom of the element are not associated with these nodes, which has implications for applying boundary conditions (see “Boundary conditions” below).
# Governing field equations
The electric and magnetic fields are governed by Maxwell’s equations describing electromagnetic phenomena. The formulation is based on the low-frequency assumption, which neglects the