7.2. Explicit Dynamics Material Model Descriptions

This section describes each material model in detail. Wherever “load curve ID” is mentioned as required input, you actually input a material data curve ID. Material data curves are defined using the EDCURVE command as outlined in Loading. All applicable properties for a material model appear in that model’s dialog box when you are working interactively. The corresponding commands are provided here for when you are working in batch or command mode. Be sure to define all properties that are listed for the material model; do not define extraneous properties.

7.2.1. Linear Elastic Models

7.2.1.1. Isotropic Elastic Model

Isotropic material model. Use the MP command to input the required values:

MP,DENS - density
MP,EX - elastic modulus
MP,NUXY - Poisson’s ratio

For an example input listing, see Isotropic Elastic Example: High Carbon Steel.

7.2.1.2. Orthotropic Elastic Model

Orthotropic material model. Use the MP command to input the required values.

MP,DENS - density
MP,EX - elastic moduli (also EY, EZ); one value required
MP,NUXY - Minor Poisson’s ratio (also NUYZ, NUXZ); one value required or MP,PRXY - Major Poisson’s ratio (also PRYZ, PRXZ); one value required
MP,GXY - shear moduli (also GYZ and GXZ); one value required

If only one value is specified for a given material property family (i.e., EX), the other values will be automatically defined (e.g., EY = EZ = EX). To specify a material coordinate system, use the EDLCS and EDMP,ORTHO commands. If no material coordinate system is specified, material properties are locally orthotropic with material axes defined by nodes I, J, and L of the element (see the figure below). For a multi-layer composite laminate, use the TB,COMP command instead and specify the lamina (ply) properties as SHELL163 real constants. See Composite Damage Model for more information.

For an example input listing, see Orthotropic Elastic Example: Aluminum Oxide.

7.2.1.3. Anisotropic Elastic Model

This material description requires the full elasticity matrix. Because of symmetry, only 21 constants are required. This material is only valid for SOLID164 and SOLID168 elements.

Input density with MP. The constants are input in upper triangular form by means of the TB,ANEL command. To specify a material orientation axis, use the EDLCS and EDMP,ORTHO commands. If no material coordinate system is specified, material properties are locally orthotropic with material axes defined by nodes I, J, and L of the element (see figure of element coordinate system above).

MP,DENS - density
TB,ANEL
TBDATA, 1, C11, C12, C22, C13, C23, C33
TBDATA, 7, C14, C24, C34, C44, C15, C25
TBDATA, 13, C35, C45, C55, C16, C26, C36
TBDATA, 19, C46, C56, C66

When you list out the data table information [TBLIST] for this material type, the constants will be listed in lower triangular form [D] instead of upper triangular form [C]. This discrepancy is not a computational error; the material data is correctly transferred to the LS-DYNA program.

For an example input listing, see Anisotropic Elastic Example: Cadmium.

7.2.1.4. Elastic Fluid Model

Use this option to model containers filled with fluid that undergo dynamic impact loading. You input density using the MP command (DENS). Elastic fluid is then defined as a material type using the EDMP command:

MP,DENS
EDMP,FLUID,MAT,VAL1

The fluid model requires that the bulk modulus be specified. You can input the bulk modulus in the VAL1 field of the above command. As an alternative to inputting the bulk modulus directly using EDMP, you can input the elastic modulus (EX) and Poisson’s ratio (NUXY) using the MP command, and the program will calculate the bulk modulus as shown below.

MP,EX
MP,NUXY

If VAL1 (on EDMP), EX, and NUXY are all specified, VAL1 will be used as the bulk modulus.

7.2.2. Nonlinear Elastic Models

7.2.2.1. Blatz-Ko Rubber Elastic Model

The hyperelastic continuum rubber model defined by Blatz and Ko. This model uses the second Piola-Kirchhoff stress:

G is the shear modulus, V is the relative volume, ν is the Poisson’s ratio, Cij is the right Cauchy-Green strain tensor, and δij is the Kronecker delta. Use the MP command to input density (DENS) and shear modulus (GXY).

For an example input listing, see Blatz-Ko Example: Rubber.

7.2.2.2. Mooney-Rivlin Rubber Elastic Model

Incompressible rubber material model; nearly identical to the 2-parameter existing ANSYS Mooney-Rivlin model. The strain energy density function is defined in terms of input parameters C10, C01 and ν:

I1, I2, and I3 are invariants of the right Cauchy-Green Tensor.

Input Poisson’s ratio (ν) and density with the MP command. (For Poisson's ratio, a value greater than .49 is recommended; smaller values may not work.) Input the Mooney-Rivlin constants with the TB and TBDATA commands. Data at only one temperature is permitted and must be specified in locations 1 and 2 for the data table:

TB,MOONEY,,,,0
TBDATA, 1, C10
TBDATA, 2, C01

As an alternative to inputting C10 and C01 directly, you can set these constants to zero and supply tabulated uniaxial data via a load curve. The program will calculate the constants based on the experimental data input in locations 3-6 of the TBDATA command. To use this input method, you must set the TBOPT field of the TB command to 2:

TB,MOONEY,,,,2
TBDATA, 1, C10 (set to zero to use experimental data)
TBDATA, 2, C01 (set to zero to use experimental data)
TBDATA, 3, C3 (specimen gauge length L0)
TBDATA, 4, C4 (specimen gauge width)
TBDATA, 5, C5 (specimen thickness)
TBDATA, 6, C6 (load curve ID)

The load curve definition that provides the uniaxial data should give the change in gauge length ΔL versus the corresponding force. In compression, both the force and the change in gauge length must be specified as negative values. In tension, the force and change in gauge length should be input as positive values. The principal stretch ratio in the uniaxial direction, λ1, is then given by:

where L0 is the initial length and L is the actual length.

Alternatively, you can input the stress versus strain curve by setting the gauge length, thickness, and width equal to 1.0 and defining the engineering strain in place of the change in gauge length and the nominal (engineering) stress in place of the force.

The least squares fit to the experimental data is performed during the initialization phase of the solution in ANSYS LS-DYNA.

For an example input listing, see Mooney-Rivlin Example: Rubber.

7.2.2.3. Viscoelastic Model

Linear viscoelastic material model introduced by Herrmann and Peterson. The model assumes the deviatoric behavior:

where the shear relaxation modulus is given by:

In the model, elastic bulk behavior is assumed when calculating the incrementally integrated pressure from the volume, V: p = K ln V. The parameters , G0 , K (Bulk modulus) and β are required to define the linear viscoelastic material model. Input these values with TB,EVISC and locations 46, 47, 48, and 61 of the TBDATA command:

TB,EVISC
TBDATA, 46, G0
TBDATA, 47,
TBDATA, 48, K
TBDATA, 61, 1/β

Note:  For this material option, you must specify density (DENS) with the MP command.


For an example input listing, see Viscoelastic Example: Glass.

7.2.3. Nonlinear Inelastic Models

7.2.3.1. Bilinear Isotropic Model

Classical bilinear isotropic hardening model (strain rate independent) that uses two slopes (elastic and plastic) to represent the stress-strain behavior of a material. Specify the stress-strain behavior at only one temperature. (A temperature dependent model is also available; see Temperature Dependent Bilinear Isotropic Model.) Input elastic modulus (EX), Poisson’s ratio (NUXY), and density (DENS) with the MP command. The program calculates the bulk modulus (K) using the EX and NUXY values that you input. Input the yield strength and tangent slope with TB,BISO and locations 1 and 2 of the TBDATA command:

TB,BISO
TBDATA, 1, σY (yield stress)
TBDATA, 2, Etan (tangent modulus)

For an example input listing, see Bilinear Isotropic Plasticity Example: Nickel Alloy.

7.2.3.2. Temperature Dependent Bilinear Isotropic Model

Classical bilinear isotropic hardening model that is strain rate independent and uses two slopes (elastic and plastic) to represent the stress-strain behavior of a material. The stress-strain behavior can be specified at up to six different temperatures. If the stress-strain behavior is specified at only one temperature, the Bilinear Isotropic (which is both strain rate and temperature independent) material model is assumed. You can use this model to represent a thermo-elastic material by inputting a large value for yield strength.

Input density (DENS) with the MP command. (The density is temperature independent.) Input elastic modulus (EX), Poisson’s ratio (NUXY), and thermal expansion coefficient (ALPX) with the MPTEMP and MPDATA commands. (These properties are temperature dependent.) Input the yield strength and tangent slope with the TB,BISO,,NTEMP command, TBTEMP commands, and locations 1 and 2 of the TBDATA command. The yield strength and tangent modulus must be defined relative to the same temperature data that are used on the MPTEMP command.

MP,DENS
MPTEMP,1,TEMP1,TEMP2, . . . ,TEMPntemp
MPDATA,EX,,1,EX1, EX2, . . . ,EXntemp
MPDATA,NUXY,,1,NUXY1,NUXY2, . . . ,NUXYntemp
MPDATA,ALPX,,1,ALPX1,ALPX2, . . . ,ALPXntemp
TB, BISO,,NTEMP (NTEMP can be 2 to 6)
TBTEMP,TEMP1 (first temperature point)
TBDATA, 1, σY (yield stress)
TBDATA, 2, Etan (tangent modulus)
TBTEMP,TEMP2 (second temperature point)
TBDATA, 1, σY (yield stress)
TBDATA, 2, Etan (tangent modulus)
. . . (continue the pattern NTEMP times)
TBTEMP,TEMPntemp (last temperature point)
TBDATA, 1, σY (yield stress)
TBDATA, 2, Etan (tangent modulus)

Note:  For this material model, you must supply data over a temperature range wide enough to cover the actual temperatures that will occur in the analysis. Otherwise, the analysis will terminate.


7.2.3.3. Transversely Anisotropic Hardening Model

Fully iterative anisotropic plasticity model available for shell and 2–D elements only. In this model the yield function given by Hill[3] is reduced to the following for the case of plane stress:

where R is the anisotropic hardening parameter which is the ratio of the in-plane plastic strain rate, , to the out of plane plastic strain rate, :

The stress-strain behavior can be specified at only one temperature. Input the elastic modulus (EX), density (DENS), and Poisson’s ratio (NUXY) with the MP command. Input the yield stress, tangent modulus, anisotropic hardening parameter, and a load curve ID for effective yield stress versus effective plastic strain with TB,PLAW,,,,7 and locations 1 - 4 of the TBDATA command:

TB,PLAW,,,,7
TBDATA, 1, σY (yield stress)
TBDATA, 2, Etan (tangent modulus)
TBDATA, 3, R (anisotropic hardening parameter)
TBDATA, 4, LCID (load curve ID for yield stress vs. plastic strain)

For an example input listing, see Transversely Anisotropic Elastic Plastic Example: 1010 Steel.

7.2.3.4. Transversely Anisotropic FLD Hardening Model

This material model is used for simulating the sheet metal forming of anisotropic materials. Only transversely anisotropic materials can be considered. For this model, the dependence of the flow stress with the effective plastic strain can be modeled using a defined load curve (using EDCURVE). In addition, you can define a forming limit diagram (also using EDCURVE). This diagram will be used by the ANSYS LS-DYNA program to compute the maximum strain ratio that the material can experience.

This plasticity model is only available for shell and 2-D elements. The model directly follows the plasticity theory introduced in the Transversely Anisotropic Elastic Plastic model described earlier in this section. You can refer to that model for the theoretical basis.

To utilize the Transversely Anisotropic FLD model, you must input the density (DENS), elastic modulus (EX), and Poisson's ratio (NUXY) with the MP command. As shown below, the additional input parameters are specified using TB,PLAW,,,,10 and locations 1-5 of the TBDATA command.

TB,PLAW,,,,10
TBDATA,1,σy (yield stress)
TBDATA,2,Etan (tangent modulus)
TBDATA,3,R (anisotropic hardening parameter)
TBDATA,4,LCID1 (load curve for defining effective stress vs. plastic strain)
TBDATA,5,LCID2 (load curve for defining FLD)

For an example input listing, see Transversely Anisotropic FLD Example: Stainless Steel.

7.2.3.5. Bilinear Kinematic Model

(strain rate independent)

Classical bilinear kinematic hardening model that uses two slopes (elastic and plastic) to represent the stress-strain behavior of a material. The stress-strain behavior can be specified at only one temperature. Input elastic modulus (EX), density (DENS), and Poisson’s ratio (NUXY) with the MP command. Input the yield strength and tangent slope with TB,BKIN and locations 1 and 2 of the TBDATA command:

TB,BKIN
TBDATA, 1, σY (yield stress)
TBDATA, 2, Etan (tangent modulus)

For an example input listing, see Bilinear Kinematic Plasticity Example: Titanium Alloy.

7.2.3.6. Plastic Kinematic Model

Isotropic, kinematic, or a combination of isotropic and kinematic hardening models with strain rate dependency and failure. Isotropic and kinematic contributions may be varied by adjusting the hardening parameter β between 0 (kinematic hardening only) and 1 (isotropic hardening only). Strain rate is accounted for using the Cowper-Symonds model which scales the yield stress by the strain rate dependent factor as shown below:

where σ0 is the initial yield stress, is the strain rate, C and P are the Cowper-Symonds strain rate parameters, εp eff is the effective plastic strain, and Ep is the plastic hardening modulus which is given by

The stress-strain behavior can only be specified at one temperature. Input the elastic modulus (EX), density (DENS), and Poisson’s ratio (NUXY) with the MP command. Input the yield stress, tangent slope, hardening parameter, strain rate parameters C and P, and the failure strain with TB,PLAW,,,,1 and locations 1 - 6 of the TBDATA command:

TB,PLAW,,,,1
TBDATA, 1, σY (yield stress)
TBDATA, 2, Etan (tangent modulus)
TBDATA, 3, β (hardening parameter)
TBDATA, 4, C (strain rate parameter)
TBDATA, 5, P (strain rate parameter)
TBDATA, 6, εf (failure strain)

For an example input listing, see Plastic Kinematic Example: 1018 Steel.

7.2.3.7. 3-Parameter Barlat Model

Anisotropic plasticity model developed by Barlat and Lian[1] used for modeling aluminum sheets under plane stress conditions. Both exponential and linear hardening rules are available. The anisotropic yield criterion for plane stress is defined as:

where σY is the yield stress, a and c are anisotropic material constants, m is Barlat exponent, and K1 and K2 are defined by:

where h and p are additional anisotropic material constants. For the exponential hardening option, the material yield strength is given by:

where k is the strength coefficient, ε0 is the initial strain at yield, εp is the plastic strain, and n is the hardening coefficient. All of the anisotropic material constants, excluding p which is determined implicitly, are determined from Barlat and Lian width to thickness strain ratio (R) values as shown:

c = 2 – a

The width to thickness strain ratio for any angle Φ can be calculated from:

Above, σϕ is the uniaxial tension in the Φ direction. The stress-strain behavior can be specified at only one temperature. Input the elastic modulus (EX), density (DENS), and Poisson’s ratio (NUXY) with the MP command. Input the hardening rule type, HR (equal to 1 for linear or 2 for exponential), tangent modulus (for HR = 1) or strength coefficient (for HR = 2), yield stress (for HR = 1) or hardening coefficient (for HR = 2), the Barlat exponent, m, the width to thickness strain ratio values, R00, R45, and R90, and the orthotropic material axes with TB,PLAW,,,,3 and locations 1 - 8 of the TBDATA command:

TB,PLAW,,,,3
TBDATA, 1, HR (hardening rule type)
TBDATA, 2, Etan or k (tangent modulus or strength coefficient)
TBDATA, 3, σY or n (yield stress or hardening coefficient)
TBDATA, 4, m (Barlat exponent)
TBDATA, 5, R00
TBDATA, 6, R45
TBDATA, 7, R90
TBDATA,8,CSID (defines orthotropic material axes)

The last input item, CSID, has two valid values: 0 (default) and 2. If CSID = 0, the local coordinate system will be defined by nodes I, J, and L of the element:

If CSID = 2, material axes are determined by a local coordinate system specified with the EDLCS command (see the command description for the details of how the axes are oriented). Before specifying the material property, you must define the local coordinate system using EDLCS, and then issue EDMP,ORTHO,,VAL1, where VAL1 is the coordinate system ID from EDLCS.

For an example input listing, see 3 Parameter Barlat Example: Aluminum 5182.

7.2.3.8. Barlat Anisotropic Plasticity Model

Anisotropic plasticity model developed by Barlat, Lege, and Brem[2] used for modeling material behavior in forming processes. The anisotropic yield function Φ is defined as:

where m is the flow potential exponent and Si are the principal values of the symmetric matrix Sij.

where a, b, c, f, g, and h represent the anisotropic material constants. When a=b=c=f=g=h=1, isotropic material behavior is modeled and the yield surface reduces to the Tresca surface for m = 1 and the von Mises surface for m = 2 or 4. For this material option, the yield strength is given by:

where k is the strength coefficient, εP is the plastic strain, ε0 is the initial strain at yield, and n is the hardening coefficient. The stress-strain behavior can be specified at only one temperature.

Input the elastic modulus (EX), density (DENS), and Poisson’s ratio (NUXY) with the MP command. Input the strength coefficient, the initial strain at yield, the hardening coefficient, the flow potential exponent, and the Barlat anisotropic constants a-h with TB,PLAW,,,,6 and locations 1 - 10 of the TBDATAcommand.

TB,PLAW,,,,6
TBDATA, 1, k (strength coefficient)
TBDATA, 2, ε0 (initial strain)
TBDATA, 3, n (hardening coefficient)
TBDATA, 4, m (flow potential (Barlat) exponent)
TBDATA, 5, a
TBDATA, 6, b
TBDATA, 7, c
TBDATA, 8, f
TBDATA, 9, g
TBDATA, 10, h

For an example input listing, see Barlat Anisotropic Plasticity Example: 2008-T4 Aluminum.

7.2.3.9. Rate Sensitive Power Law Plasticity Model

Strain rate dependent plasticity model typically used for superplastic forming analyses. The material model follows a Ramburgh-Osgood constitutive relationship of the form:

where ε is the strain, is the strain rate, k is the material constant, m is the hardening coefficient, and n is the strain rate sensitivity coefficient. The stress-strain behavior can be specified at only one temperature. Input the elastic modulus (EX), density (DENS), and Poisson’s ratio (NUXY) with the MP command. Input the material constant, hardening coefficient, strain rate sensitivity coefficient, and initial strain rate with TB,PLAW,,,,4 and locations 1 - 4 of the TBDATA command:

TB,PLAW,,,,4
TBDATA, 1, k (material constant)
TBDATA, 2, m (hardening coefficient)
TBDATA, 3, n (strain rate sensitivity coefficient)
TBDATA, 4, 0 (initial strain rate)

For an example input listing, see Rate Sensitive Powerlaw Plasticity Example: A356 Aluminum.

7.2.3.10. Strain Rate Dependent Plasticity Model

Strain rate dependent isotropic plasticity model used mainly for metal and plastic forming analyses.

In this model, a load curve is used to describe the initial yield strength, σ0, as a function of effective strain rate. The yield stress for this material model is defined as:

where σ0 is the initial yield strength, is the effective strain rate, (εp)eff is the effective plastic strain, and Eh is given by:

The stress-strain behavior can be specified at only one temperature. Input the elastic modulus (EX), density (DENS), and Poisson’s ratio (NUXY) using the MP command. Input the load curve ID for defining the initial yield stress vs. effective strain rate, the tangent modulus, the load curve ID for defining the elastic modulus vs. effective strain rate (optional), the load curve ID for defining the tangent modulus vs. effective strain rate (optional), and the load curve ID for defining the von Mises stress at failure vs. effective strain rate using TB,PLAW,,,,5 and locations 1 - 5 of the TBDATA command. For shell elements, you have the option of specifying Mn Time in location 6, instead of LCID4 in location 5, to define failure of the material. Mn Time is the minimum time step size for automatic element deletion.

TB,PLAW,,,,5
TBDATA, 1, LCID1 (load curve ID for defining the initial yield stress vs. effective strain rate)
TBDATA, 2, Etan (tangent (plastic hardening) modulus)
TBDATA, 3, LCID2 (the load curve ID for defining the elastic modulus vs. effective strain rate)
TBDATA, 4, LCID3 (the load curve ID for defining the tangent modulus vs. effective strain rate)
TBDATA, 5, LCID4 (the load curve ID for defining von Mises stress at failure vs. effective strain rate)
TBDATA, 6, Mn Time (minimum time step size for automatic element deletion, for shell elements only)

For an example input listing, see Strain Rate Dependent Plasticity Example: 4140 Steel.

7.2.3.11. Piecewise Linear Plasticity Model

This model provides a multilinear elastic-plastic material option that allows stress vs. strain curve input and strain rate dependency. This is a very commonly used plasticity law, especially for steel. Failure based on plastic strain can also be modeled with this material.

The piecewise linear plasticity model provides three different methods to account for the strain rate. The first method utilizes the Cowper-Symonds model, which scales the yield stress as shown:

where is the effective plastic strain rate, C and P are strain rate parameters, and is the yield stress without considering strain rate. This yield stress quantity can be input as either σy and Etan (TBDATA entries 1 and 2) or as a total true stress vs. effective plastic strain curve, LCID1 (TBDATA entry 6).

The second method uses the LCID2 curve (TBDATA entry 7) to scale the yield stress with respect to strain rate. If LCID2 is input, it is used instead of the Cowper-Symonds scaling term defined by the strain rate parameters C and P.

The third method used to account for the strain rate dependency requires that you define separate stress vs. effective plastic strain curves at specific strain rates. Using TBDATA entries 8 - 27, you may input stress vs. effective plastic strain behavior for up to ten different strain rates (Rate1 and LCID3, Rate2 and LCID4, etc.). It is important that you input all strain rate definitions in ascending order. Note that if Rate1 and LCID3 are specified, TBDATA entries 4-7 (C, P, LCID1, and LCID2) are automatically ignored.

Input the elastic modulus (EX), density (DENS), and Poisson’s ratio (NUXY) with the MP command. Input the yield stress, the tangent modulus, the effective plastic strain at failure, and the remaining parameters (listed below) with TB,PLAW,,,,8 and locations 1 - 27 of the TBDATA command:

TB, PLAW,,,,8
TBDATA,1, σY (yield stress)
TBDATA,2, Etan (tangent modulus)
TBDATA,3, εF (effective plastic strain at failure)
TBDATA,4, C (strain rate parameter)
TBDATA,5, P (strain rate parameter)
TBDATA,6, LCID1 (load curve defining total true stress vs. effective plastic strain)
TBDATA,7, LCID2 (load curve that scales LCID1 with respect to strain rate)
TBDATA,8, Rate1 (strain rate value 1)
TBDATA,9, LCID3 (stress vs. effective plastic strain curve for Rate1)
TBDATA,10, Rate2 (strain rate value 2)
TBDATA,11, LCID4 (stress vs. effective plastic strain curve for Rate2)
TBDATA,12, Rate3 (strain rate value 3)
TBDATA,13, LCID5 (stress vs. effective plastic strain curve for Rate3)
TBDATA,14, Rate4 (strain rate value 4)
TBDATA,15, LCID6 (stress vs. effective plastic strain curve for Rate4)
TBDATA,16, Rate5 (strain rate value 5)
TBDATA,17, LCID7 (stress vs. effective plastic strain curve for Rate5)
TBDATA,18, Rate6 (strain rate value 6)
TBDATA,19, LCID8 (stress vs. effective plastic strain curve for Rate6)
TBDATA,20, Rate7 (strain rate value 7)
TBDATA,21, LCID9 (stress vs. effective plastic strain curve for Rate7)
TBDATA,22, Rate8 (strain rate value 8)
TBDATA,23, LCID10 (stress vs. effective plastic strain curve for Rate8)
TBDATA,24, Rate9 (strain rate value 9)
TBDATA,25, LCID11 (stress vs. effective plastic strain curve for Rate9)
TBDATA,26, Rate10 (strain rate value 10)
TBDATA,27, LCID12 (stress vs. effective plastic strain curve for Rate10)

If load curve LCID1 (total true stress vs. effective plastic strain) is input, the yield stress (σY) and tangent modulus (Etan) values will be overwritten. If LCID2 (the scaling curve) is input, strain rate parameters C and P will be overwritten. If C and P, LCID2, and Rate1 (first strain rate value) are all set to zero, strain rate dependency is ignored.

For an example input listing, see Piecewise Linear Plasticity Example: High Carbon Steel. See also Using Data Curves with Material Models for an example of how to input a true stress vs. effective plastic strain curve for this material model.

7.2.3.12. Modified Piecewise Linear Plasticity Model

This model provides a multilinear elastic-plastic material option that allows stress vs. strain curve input and strain rate dependency. This model is similar to piecewise linear plasticity (TB,PLAW,,,,8), but has an enhanced failure criteria. Failure is based on effective plastic strain, plastic thinning, or the major principal in-plane strain component (see TBDATA entries 8 - 10: EPSTHIN, EPSMAJ, and NUMINT).

The modified piecewise linear plasticity model uses the same three methods to account for the strain rate as the piecewise linear plasticity model (see Piecewise Linear Plasticity Model for details). To account for strain rate, do one of the following:

  • Input the strain rate parameters C and P (TBDATA entries 4 and 5) to use the Cowper-Symonds model.

  • Input the LCID2 curve (TBDATA entry 7) to scale the yield stress with respect to strain.

  • Define separate stress vs. strain curves for different strain rates (TBDATA entries 11 - 30).

Input the elastic modulus (EX), density (DENS), and Poisson’s ratio (NUXY) with the MP command. Input the remaining parameters with TB,PLAW,,,,11 and locations 1 - 30 of the TBDATA command:

TB, PLAW,,,,11
TBDATA,1, σY (yield stress)
TBDATA,2, Etan (tangent modulus)
TBDATA,3, εF (effective plastic strain at failure)
TBDATA,4, C (strain rate parameter)
TBDATA,5, P (strain rate parameter)
TBDATA,6, LCID1 (load curve defining total true stress vs. effective plastic strain)
TBDATA,7, LCID2 (load curve that scales LCID1 with respect to strain rate)
TBDATA,8, EPSTHIN (thinning plastic strain at failure)
TBDATA,9, EPSMAJ (major in-plane strain at failure)
TBDATA,10, NUMINT (number of through-thickness integration points that must fail for element failure)
TBDATA,11, Rate1 (strain rate value 1)
TBDATA,12, LCID3 (stress vs. effective plastic strain curve for Rate1)
TBDATA,13, Rate2 (strain rate value 2)
TBDATA,14, LCID4 (stress vs. effective plastic strain curve for Rate2)
TBDATA,15, Rate3 (strain rate value 3)
TBDATA,16, LCID5 (stress vs. effective plastic strain curve for Rate3)
TBDATA,17, Rate4 (strain rate value 4)
TBDATA,18, LCID6 (stress vs. effective plastic strain curve for Rate4)
TBDATA,19, Rate5 (strain rate value 5)
TBDATA,20, LCID7 (stress vs. effective plastic strain curve for Rate5)
TBDATA,21, Rate6 (strain rate value 6)
TBDATA,22, LCID8 (stress vs. effective plastic strain curve for Rate6)
TBDATA,23, Rate7 (strain rate value 7)
TBDATA,24, LCID9 (stress vs. effective plastic strain curve for Rate7)
TBDATA,25, Rate8 (strain rate value 8)
TBDATA,26, LCID10 (stress vs. effective plastic strain curve for Rate8)
TBDATA,27, Rate9 (strain rate value 9)
TBDATA,28, LCID11 (stress vs. effective plastic strain curve for Rate9)
TBDATA,29, Rate10 (strain rate value 10)
TBDATA,30, LCID12 (stress vs. effective plastic strain curve for Rate10)

If load curve LCID1 (total true stress vs. effective plastic strain) is input, the yield stress (σY) and tangent modulus (Etan) values will be overwritten. If LCID2 (the scaling curve) is input, strain rate parameters C and P will be overwritten. If C and P, LCID2, and Rate1 (first strain rate value) are all set to zero, strain rate dependency is ignored.

For an example input listing, see Modified Piecewise Linear Plasticity Example: PVC.

7.2.3.13. Composite Damage Model

Material model developed by Chang & Chang[4] for the failure of composite materials. The following five parameters are used in the model:

S1 = longitudinal tensile strength
S2 = transverse tensile strength
S12 = shear strength
C2 = transverse compressive strength
α = nonlinear shear stress parameter

All parameters are determined experimentally. Input the elastic moduli (EX, EY, EZ), shear moduli (GXY, GYZ, GXZ), density (DENS), and Poisson’s ratios (NUXY, NUYZ, NUXZ) with the MP command. Input the bulk modulus at compressive failure, the shear strength, the longitudinal tensile strength, transverse tensile strength, transverse compressive strength, and nonlinear shear stress parameter with TB,COMP and locations 1 - 6 of the TBDATA command:

TB, COMP
TBDATA, 1, KFAIL (bulk modulus of material in compressive failure)
TBDATA, 2, S12 (shear strength)
TBDATA, 3, S1 (longitudinal tensile strength)
TBDATA, 4, S2 (transverse tensile strength)
TBDATA, 5, C2 (transverse compressive strength)
TBDATA, 6, α (nonlinear shear stress parameter)

Note:  Please refer to the LS-DYNA Theoretical Manual for more details about LS-DYNA Material model #22 (Composite Damage). This material model is required for multi-layer composite laminates, even if the failure capabilities are not used. The lamina (ply) properties are specified as SHELL163 real constants.


7.2.3.14. Concrete Damage Model

The Concrete Damage model is used to analyze buried steel reinforced concrete subject to impact loadings. This model requires constants for the concrete and reinforced materials, and also requires tabulated equation of state constants. (Refer to Equation of State Models for a detailed description of the tabulated equation of state.) Input the density (DENS) and Poisson’s ratio (NUXY) with the MP command. Input all values shown below with the TB,CONCR,,,,2 command and locations 1 – 78 of the TBDATA command:

TB,CONCR,,,,2
TBDATA,1,σf (maximum principal stress for failure)
TBDATA,2,A0 (cohesion constant)
TBDATA,3,A1 (pressure hardening coefficient)
TBDATA,4,A2 (pressure hardening coefficient)
TBDATA,5,A0Y (cohesion for yield)
TBDATA,6,A1Y (pressure hardening coefficient for yield limit)
TBDATA,7,A2Y (pressure hardening coefficient for yield limit)
TBDATA,8,A1F (pressure hardening coefficient for failed material)
TBDATA,9,A2F (pressure hardening coefficient for failed material)
TBDATA,10,B1 (damage scale factor)
TBDATA,11,B2 (damage scale factor for uniaxial tension)
TBDATA,12,B3 (damage scale factor for triaxial tension)
TBDATA,13,PER (percent reinforcement)
TBDATA,14,Er (elastic moduli of reinforcement)
TBDATA,15,NUXYr (Poisson’s ratio of reinforcement)
TBDATA,16,σy (initial yield stress)
TBDATA,17,Etan (tangent modulus)
TBDATA,18,LCP (load curve ID giving rate sensitivity for principal material)
TBDATA,19,LCR (load curve ID giving rate sensitivity for reinforcement)
TBDATA,20-32,λ1-λ13 (tabulated damage functions 1-13)
TBDATA,33-45,η1-η13 (tabulated scale factors 1-13)
TBDATA,46,GAMA (temperature constant)
TBDATA,47,E0 (initial internal energy)
TBDATA,48,V0 (initial relative volume)
TBDATA,49-58,εv1-εv10 (volumetric strain data values 1-10; natural log of the relative volume)
TBDATA,59-68,C1-C10 (volumetric pressure values at εvi)
TBDATA,69-78,T1-T10 (temperature values at εvi)

7.2.3.15. Power Law Plasticity Model

Strain rate dependent plasticity model typically used for metal and plastic forming analyses. Elastoplastic behavior with isotropic hardening is provided with this model. The material model has a Power Law constitutive relationship which includes the Cowper-Symonds multiplier to account for strain rate:

where is the strain rate, C and P are the Cowper-Symonds strain rate parameters, εe is the elastic strain to yield, is the effective plastic strain, k is the strength coefficient, and n is the hardening coefficient. The stress-strain behavior can be specified at only one temperature. Input the elastic modulus (EX), density (DENS), and Poisson’s ratio (NUXY) with the MP command. Input the strength coefficient, hardening coefficient, and strain rate parameters C and P with TB,PLAW,,,,2 and locations 1 - 4 of the TBDATA command:

TB, PLAW,,,,2
TBDATA, 1, k (strength coefficient)
TBDATA, 2, n (hardening coefficient)
TBDATA, 3, C (strain rate parameter)
TBDATA, 4, P (strain rate parameter)

For an example input listing, see Powerlaw Plasticity Example: Aluminum 1100.

7.2.3.16. Elastic Viscoplastic Thermal Model

This material allows an elastic viscoplastic material definition with thermal effects. The uniaxial stress-stress-strain curve has the form:

where σ0 is the initial yield stress, εp eff is the effective plastic strain, and the other parameters are as described in the TBDATA input shown below.

Strain rate is accounted for using the Cowper and Symonds model (where C and P are the Cowper-Symonds strain rate parameters), which scales the yield stress with the factor:

To convert from these constants, set the viscoelastic constants, Vk and Vm, to the following values:

You must input density (DENS) using the MP command. You must also input the elastic modulus (EX), Poisson's ratio (NUXY), and the coefficient of thermal expansion (ALPX) by either using the MP command or by inputting load curves in locations 13, 14, and 18 of the TBDATA command. You can use the load curve input to represent each quantity as a function of temperature. Input the remaining parameters (described below) with the TB,PLAW,,,,12 command and locations 1 - 18 of the TBDATA command.

TB,PLAW,,,,12
TBDATA,1, σ0 (initial yield stress)
TBDATA,2, QR1 (isotropic hardening parameter)
TBDATA,3, CR1 (isotropic hardening parameter)
TBDATA,4, QR2 (isotropic hardening parameter)
TBDATA,5, CR2 (isotropic hardening parameter)
TBDATA,6, QX1 (kinematic hardening parameter)
TBDATA,7, CX1 (kinematic hardening parameter)
TBDATA,8, QX2 (kinematic hardening parameter)
TBDATA,9, CX2 (kinematic hardening parameter)
TBDATA,10, C (viscous parameter)
TBDATA,11, p (viscous parameter)
TBDATA,12, LCID1 (load curve ID for total true stress vs. effective plastic strain (if specified, TBDATA 2-9 are ignored))
TBDATA,13, LCID2 (load curve ID for elastic modulus vs. temperature)
TBDATA,14, LCID3 (load curve ID for Poisson's ratio vs. temperature)
TBDATA,15, LCID4 (load curve ID for initial yield stress vs. temperature; if input, σ0 is ignored)
TBDATA,16, LCID5 (load curve ID for scaling factor on isotropic hardening parameters (QR1 and QR2) vs. temperature)
TBDATA,17, LCID6 (load curve ID for scaling factor on kinematic hardening parameters (QX1 and QX2) vs. temperature)
TBDATA,18, LCID7 (load curve ID for thermal coefficient of expansion vs. temperature)

Note:  If the total true stress vs. effective plastic strain is input (LCID1 in location 12 of TBDATA), then TBDATA locations 2-9 are ignored. Also, if LCID2, LCID3, or LCID7 is specified, then the corresponding MP command is ignored. (For example, LCID2 overrides the command MP,EX.)


For an example input listing, see Elastic Viscoplastic Thermal Example.

7.2.4. Pressure Dependent Plasticity Models

7.2.4.1. Elastic-Plastic Hydrodynamic Model

This model is used for modeling materials undergoing large amounts of strain, where the plastic behavior can either be defined from a set of data points or from the yield stress and tangent modulus. If the effective true plastic strain and effective true stress data values are not specified, the yield strength will be calculated as shown below (based on isotropic hardening):

You can calculate the plastic hardening modulus, Eh, in terms of the Young’s modulus and tangent modulus:

If the effective true plastic strain and stress values are specified, the stress-strain behavior is defined by the data points along the effective true stress vs. true plastic strain curve. Up to 16 data points may be specified. Linear extrapolation will be used if the strain values exceed the maximum input values; therefore, you should input values to cover the full range of strains expected in the analysis. Input the density (DENS), elastic modulus (EX), and shear modulus (GXY) with the MP command. Input the parameters described below with TB,PLAW,,,,9 and locations 1-45 of the TBDATA command:

TB,PLAW,,,,9
TBDATA,1, σ0 (initial yield stress)
TBDATA,2,Eh (hardening modulus)
TBDATA,3,PC (pressure cutoff value)
TBDATA,4, εf (failure strain)
TBDATA,5-20,ε1-ε1 6 (effective strain data curve values)
TBDATA,21-36,σ1-σ1 6 (effective stress data curve values)
TBDATA,37,Co (linear polynomial equation of state constant)
TBDATA,38,C1 (linear polynomial equation of state constant)
TBDATA,39,C2 (linear polynomial equation of state constant)
TBDATA,40,C3 (linear polynomial equation of state constant)
TBDATA,41,C4 (linear polynomial equation of state constant)
TBDATA,42,C5 (linear polynomial equation of state constant)
TBDATA,43,C6 (linear polynomial equation of state constant)
TBDATA,44,Eo (initial internal energy)
TBDATA,45,Vo (initial relative volume)

Note that constants 37 through 45 specified on the TBDATA command are the same as the linear polynomial equation of state model. Please refer to Equation of State Models later in this chapter for more details.

7.2.4.2. Geological Cap Model

This model is an inviscid, two invariant geologic cap model which can be used for geomechanical problems or for materials such as concrete. In this model, the two invariant cap theory is extended to include nonlinear kinematic hardening. A discussion of the extended cap model and its parameters is given below.

The cap model is formulated in terms of the invariants of the stress tensor. The square root of the second invariant of the deviatoric stress tensor, , is found from the deviatoric stresses (s) as

and is the objective scalar measure of the distortional or shearing stress. The first invariant of the stress, J1, is the trace of the stress tensor.

Figure 7.1:  Surface of the Two-invariant Cap Model

Surface of the Two-invariant Cap Model

The cap model consists of three surfaces in pressure space, as shown in Figure 7.1: Surface of the Two-invariant Cap Model. Surface f1 is the failure envelope, f2 is the cap surface, and f3 is the tension cutoff. The functional form of f1 is

where Fe is given by

and

This failure envelope surface is fixed in space, and therefore does not harden unless kinematic hardening is present. Next, there is a cap surface f2 in the figure, with f2 given by

where Fc is defined by

X(κ) is the intersection of the cap surface with the J1 axis

and L(κ) is defined by

The hardening parameter κ is related to the plastic volume change through the hardening law

Geometrically, κ is seen in the figure as the J1 coordinate of the intersection of the cap surface and the failure surface. Finally, there is the tension cutoff surface, denoted f3 in the figure. The function f3 is given by

where T is the input material parameter which specifies the maximum hydrostatic tension sustainable by the material. The elastic domain in space is then bounded by the failure envelope surface above, the tension cutoff surface on the left, and the cap surface on the right.

Input the density (DENS) and shear modulus (GXY) with the MP command. Input the parameters described below with the TB,GCAP command and locations 1–13 of the TBDATA command.

TB,GCAP
TBDATA,1,K (bulk modulus)
TBDATA,2,α (failure envelope parameter)
TBDATA,3,θ (failure envelope linear coefficient)
TBDATA,4,γ (failure envelope exponential coefficient)
TBDATA,5,β (failure envelope exponent)
TBDATA,6,R (cap surface axis ratio)
TBDATA,7,D (hardening law exponent)
TBDATA,8,W (hardening law coefficient)
TBDATA,9,X0 (hardening law exponent)
TBDATA,10,C (kinematic hardening coefficient)
TBDATA,11,N (kinematic hardening parameter)
TBDATA,12,Ftype (formulation flag: use 1 for soil or concrete, 2 for rock )
TBDATA,13,Toff (tension cutoff value; Toff < 0, positive in compression)

Please refer to Material Model 25 in the LS-DYNA Theoretical Manual for more information about this material model.

For an example input listing, see Geological Cap Example: SRI Dynamic Concrete.

7.2.5. Foam Models

7.2.5.1. Closed Cell Foam Model

Rigid, closed cell, low density polyurethane foam material model often used for modeling impact limiters in automobile designs. This material model is very similar to the honeycomb model in that the components of the stress tensor are uncoupled until volumetric compaction is achieved. Unlike honeycomb, however, the closed cell foam model is isotropic in nature and includes the effects of confined air pressure. The material model defines stress to be:

where (σij)sk is the skeletal stress, po is the initial foam pressure, φ is the ratio of foam to polymer density, δij is the Kronecker delta, and γ is the volumetric strain which is defined by:

where V is the relative volume and γo is the initial volumetric strain. The yield condition is applied to the principal trial stresses and is defined by:

where a, b, and c are user defined input constants. The stress-strain behavior can be specified at only one temperature. Input the elastic modulus (EX) and density (DENS) with the MP command. Poisson’s ratio for this model is assumed to be zero. Input the yield stress constants a, b, and c, the initial foam pressure, the ratio of foam to polymer density, and the initial volumetric strain with TB,FOAM,,,,1 and locations 1 - 6 of the TBDATA command:

TB, FOAM,,,,1
TBDATA, 1, a
TBDATA, 2, b
TBDATA, 3, c
TBDATA, 4, po (initial foam pressure)
TBDATA, 5, φ (ratio of foam to polymer density)
TBDATA, 6, γo (initial volumetric strain)

7.2.5.2. Viscous Foam Model

Energy absorbing foam material used in crash-simulation models. The model consists of a nonlinear elastic stiffness in parallel with a viscous damper. The elastic stiffness is intended to limit total crush while the viscosity absorbs energy. The elastic stiffness, , and initial viscous coefficient, , are both nonlinear functions of the relative volume, V:

where E1 is the initial elastic stiffness, V2 is the initial viscous coefficient, and n1 and n2 are the Power Laws for the elastic stiffness and viscous coefficient, respectively. The stress-strain behavior can be specified at only one temperature. Input the initial elastic stiffness (EX), Poisson’s ratio (NUXY), and density (DENS) with the MP command. Input the Power Law for the elastic stiffness, the initial viscous coefficient, the elastic stiffness for viscosity (required to prevent time step problems), and the pearly for viscosity with TB,FOAM,,,,3 and locations 1 - 4 of the TBDATA command:

TB, FOAM,,,,3
TBDATA, 1, n1 (Power Law for the elastic stiffness)
TBDATA, 2, V2 (initial viscous coefficient)
TBDATA, 3, E1 (elastic stiffness for viscosity)
TBDATA, 4, n2 (Power Law for the viscous coefficient)

7.2.5.3. Low Density Foam Model

Highly compressible (urethane) foam material model often used for padded materials such as seat cushions. In compression, the model assumes hysteresis unloading behavior with possible energy dissipation. In tension the material model behaves linearly until tearing occurs. For uniaxial loading, the model assumes that there is no coupling in transverse directions. By using input shape factor controls (a hysteresis unloading factor (HU), a decay constant (β), and a shape factor for unloading) the observed unloading behavior of foams can be closely approximated. The stress-strain behavior can be specified at only one temperature. Input the elastic modulus (EX) and density (DENS) with the MP command. Input the load curve ID for nominal stress vs. strain, the tension cutoff (tearing) stress, the hysteresis unloading factor, the decay constant, the viscous coefficient, the shape factor for unloading, the failure option when the cutoff stress is reached, and the bulk viscosity action flag with TB,FOAM,,,,2 and locations 1 - 8 of the TBDATA command:

TB, FOAM,,,,2
TBDATA, 1, LCID (load curve ID for stress-strain behavior)
TBDATA, 2, TC (tension cutoff stress, default=1E20)
TBDATA, 3, HU (hysteretic unloading factor: between 1.0 - no energy dissipation (default) and 0.0 - full energy dissipation)
TBDATA, 4, β (decay constant)
TBDATA, 5, DAMP (viscous coefficient, values between 0.05 and 0.5 are recommended)
TBDATA, 6, SHAPE (shape unloading factor, default = 1)
TBDATA, 7, FAIL (failure option when cutoff stress is reached: 0.0 - tensile stress remains at cutoff value, 1.0 - tensile stress reset to zero)
TBDATA, 8, BVFLAG (bulk viscosity action flag: 0.0 - no bulk viscosity (recommended) and 1.0 - bulk viscosity active)

7.2.5.4. Crushable Foam Model

Material model used for crushable foams in side impact and other applications where cyclic behavior is unimportant. The foam model is strain rate dependent and crushes one-dimensionally with a Poisson’s ratio that is essentially zero. In the formulation, the elastic modulus is considered constant and the stress is updated assuming elastic behavior:

where ij is the strain rate, E is the elastic modulus, and t is time. The model includes a tensile stress cutoff value which defines failure under tensile loads. For stresses below the tensile cutoff value, the model predicts similar response between tensile and compressive loading. It is important to have a nonzero value for the cutoff stress to prevent deterioration of the material under small tensile loads. Input the elastic modulus (EX), density (DENS), and Poisson’s ratio (NUXY) with the MP command. Input the load curve ID for defining stress vs. volumetric strain, the tension cutoff value, and the viscous damping coefficient with TB,FOAM,,,,4 and locations 1 - 3 of the TBDATA command:

TB, FOAM,,,,4
TBDATA, 1, LCID (load curve ID for defining yield stress vs. volumetric strain)
TBDATA, 2, TC (tension cutoff value)
TBDATA, 3, DAMP (viscous damping coefficient, values between 0.05 and 0.5 are recommended)

7.2.5.5. Honeycomb Foam Model

Orthotropic material model used for honeycomb materials. The behavior of the model before compaction is orthotropic where the components of the stress tensor are uncoupled. The elastic moduli are considered to vary linearly with relative volume as shown below:

where

and

V = the relative volume (defined as ratio of current to original volume)
Vf = relative volume of the fully compacted honeycomb

To specify a material coordinate system, use the EDLCS and EDMP,ORTHO commands. If no material coordinate system is specified, material properties are locally orthotropic with material axes defined by nodes I, J, and L of the element (see Orthotropic Elastic Model for a graphic depiction).

Load curves can be used to input the magnitude of the average stress as the relative volume changes. Each curve must have the same abscissa values. Curves can be defined either as a function of relative volume (V) or volumetric strain (1 - V). Input the elastic modulus (EX), density (DENS), and Poisson’s ratio (NUXY) with the MP command. Input all values shown below with TB,HONEY and locations 1 - 17 of the TBDATA command:

TB, HONEY
TBDATA, 1, σY (yield stress for fully compacted honeycomb)
TBDATA, 2, Vf (relative volume of fully compacted honeycomb)
TBDATA, 3, μ (material viscosity coefficient, default = 0.05)
TBDATA, 4, Eaau (Elastic modulus in aa direction for uncompressed configuration)
TBDATA, 5, Ebbu (Elastic modulus in bb direction for uncompressed configuration)
TBDATA, 6, Eccu (Elastic modulus in cc direction for uncompressed configuration)
TBDATA, 7, Gabu (Shear modulus in ab direction for uncompressed configuration)
TBDATA, 8, Gbcu (Shear modulus in bc direction for uncompressed configuration)
TBDATA, 9, Gcau (Shear modulus in ca direction for uncompressed configuration)
TBDATA, 10, LCA (Load curve ID for aa direction stress vs. relative volume or volumetric strain)
TBDATA, 11, LCB (Load curve ID for bb direction stress vs. relative volume or volumetric strain)
TBDATA, 12, LCC (Load curve ID for cc direction stress vs. relative volume or volumetric strain)
TBDATA, 13, LCS (Load curve ID for shear yield vs. relative volume or volumetric strain)
TBDATA, 14, LCAB (Load curve ID for ab direction stress vs. relative volume or volumetric strain)
TBDATA, 15, LCBC (Load curve ID for bc direction stress vs. relative volume or volumetric strain)
TBDATA, 16, LCCA (Load curve ID for ca direction stress vs. relative volume or volumetric strain)
TBDATA, 17, LCRS (Load curve ID for strain rate effects. This input is optional. The curves defined above are scaled using this curve)

7.2.6. Equation of State Models

There are 3 different equation of state models available in ANSYS LS-DYNA:

Linear polynomial
Gruneisen
Tabulated

These equation of state models are used in conjunction with certain material models, such as the Johnson-Cook Plasticity and Zerilli-Armstrong models. You identify the equation of state to be used by inputting the appropriate number in the EOSOPT field of the TB command.

7.2.6.1. Linear Polynomial Equation of State

(EOSOPT = 1)

This equation of state is linear in internal energy. The pressure is given by:

where terms C2μ2 and C6μ2 are set to zero if and is the ratio of current density to initial density.

Input the required constants using the TBDATA command. The starting location (LOC) for the constants depends on which material model you are using. (See the description for the specific material model to find out what starting location value should be used.)

TBDATA,LOC,C0
TBDATA,LOC+1,C1
TBDATA,LOC+2,C2
TBDATA,LOC+3,C3
TBDATA,LOC+4,C4
TBDATA,LOC+5,C5
TBDATA,LOC+6,C6
TBDATA,LOC+7,E0 (initial internal energy)
TBDATA,LOC+8,V0 (initial relative volume)

7.2.6.2. Gruneisen Equation of State

(EOSOPT = 2)

This equation of state defines the pressure volume relationship in one of two ways, depending on whether the material is compressed or expanded.

The Gruneisen equation of state with cubic shock velocity-particle velocity defines pressure for compressed materials as:

and for expanded materials as:

where C is the intercept of the vs-vp curve; S1, S2, and S3 are the coefficients of the slope of the vs-vp curve, γ0 is the Gruneisen gamma, a is the first order volume correction to γ0, and

Input the required constants using the TBDATA command. The starting location (LOC) for the constants depends on which material model you are using. (See the description for the specific material model to find out what starting location value should be used.)

TBDATA,LOC,C
TBDATA,LOC+1,S1
TBDATA,LOC+2,S2
TBDATA,LOC+3,S3
TBDATA,LOC+4,γ0
TBDATA,LOC+5,A
TBDATA,LOC+6,E0 (initial internal energy)
TBDATA,LOC+7,V0 (initial relative volume)

7.2.6.3. Tabulated Equation of State

(EOSOPT = 3)

The tabulated equation of state model is linear in internal energy. Pressure is defined by:

Input the required constants using the TBDATA command. The starting location (LOC) for the constants depends on which material model you are using. (See the description for the specific material model to find out what starting location value should be used.)

TBDATA,LOC,GAMA (temperature constant)
TBDATA,LOC+1,E0 (initial internal energy)
TBDATA,LOC+2,V0 (initial relative volume)
TBDATA,LOC+3 to LOC+12,εv1-εv10 (volumetric strain data values 1-10, natural log of the relative volume)
TBDATA,LOC+13 to LOC+22,C1-C10 (volumetric pressure values at εvi)
TBDATA,LOC+23 to LOC+32,T1-T10 (temperature values at εvi)

7.2.6.4. Bamman Plasticity Model

This is a fairly complex material model used in metal forming processes with strain rate and temperature dependent plasticity. The Bamman model does not require an additional equation of state model (EOSOPT is not used) because internal equation of state variables are specified in fields 21 through 26 of the TBDATA command (as shown below).

Input the density (DENS), elastic modulus (EX) and Poisson's ratio (NUXY) with the MP command. Input the parameters described below with TB,EOS and locations 1-26 of the TBDATA command:

TB,EOS,,,,4
TBDATA,1,TI (initial temperature)
TBDATA,2,HC (heat generation coefficient)
TBDATA,3-20,C1-C18 (constants for flow stress)
TBDATA,21-26,A1-A6 (internal equation of state variables)

For a complete discussion of the kinematics associated with this model, as well as a more detailed description of the required input constants, refer to the description of Material Model 51 in Chapter 16 of the LS-DYNA Theoretical Manual.

7.2.6.5. Johnson-Cook Plasticity Model

This model, also called the viscoplastic model, is a strain-rate and adiabatic (heat conduction is neglected) temperature-dependent plasticity model. This model is suitable for problems where strain rates vary over a large range, and temperature changes due to plastic dissipation cause material softening. The model may be used for shell and solid elements. For solid elements, you need an equation of state (discussed later in this section).

Johnson and Cook express the flow stress as

where:

A, B, C, n, and m = material constant
p = effective plastic strain

The strain at fracture is given by:

Where σ* is the ratio of pressure divided by effective stress:

Fracture occurs when the damage parameter

reaches the value of 1.

Input the Young’s modulus (EX), density (DENS), and Poisson’s ratio (NUXY) with the MP command. Input the parameters described in the above equations with TB,EOS and locations 1 - 15 of the TBDATA command:

TB,EOS,,,,1,EOSOPT
TBDATA,1,A
TBDATA,2,B
TBDATA,3,n
TBDATA,4,C
TBDATA,5,m
TBDATA,6,Tmelt
TBDATA,7,Troom
TBDATA,8, * (effective plastic strain rate)
TBDATA,9,CP (specific heat)
TBDATA,10,pressure cutoff
TBDATA,11,D1
TBDATA,12,D2
TBDATA,13,D3
TBDATA,14,D4
TBDATA,15,D5

When using the Johnson-Cook Plasticity Model, you can define one of three types of equations of state: Linear Polynomial (EOSOPT = 1), Gruneisen (EOSOPT = 2), and Tabulated (EOSOPT = 3). Each has its own set of required constants that are input starting with position (LOC) 16 of the TBDATA command. See the descriptions of the three equation of state models in Equation of State Models.

For an example input listing using the Linear Polynomial EOS, see Johnson-Cook Linear Polynomial EOS Example: 1006 Steel.

For an example input listing using the Gruneisen EOS, see Johnson-Cook Gruneisen EOS Example: OFHC Copper.

7.2.6.6. Null Material Model

This material allows equations of state to be considered without computing deviatoric stresses. Optionally, you can define a viscosity. Erosion in tension and compression is possible. The Young’s modulus and Poisson’s ratio are used only for setting the contact interface stiffness, so you should use reasonable values.

Input the Young’s modulus (EX), density (DENS), and Poisson’s ratio (NUXY) with the MP command. Input the parameters listed below with TB,EOS and locations 1 - 4 of the TBDATA command:

TB, EOS,,,,2, EOSOPT
TBDATA, 1, Pressure Cutoff (  0.0)
TBDATA, 2, Viscosity Coefficient (optional)
TBDATA, 3, Relative volume for erosion in tension (V/Vo)
TBDATA, 4, Relative volume for erosion in compression (V/Vo)

When using the Null Model, you can define one of three types of equations of state: Linear Polynomial (EOSOPT = 1), Gruneisen (EOSOPT = 2), and Tabulated (EOSOPT = 3). Each has its own set of required constants that are input starting with position (LOC) 16 of the TBDATA command. See the descriptions of the three equation of state models in Equation of State Models.

For an example input listing using the Linear Polynomial EOS, see Null Material Linear Polynomial EOS Example: Brass.

For an example input listing using the Gruneisen EOS, see Null Material Gruneisen EOS Example: Aluminum.

7.2.6.7. Zerilli-Armstrong Model

This model is used in metal forming processes and high speed impact applications where the stress depends on strain, strain rate, and temperature. The Zerilli-Armstrong model expresses the yield stress as follows.

For FCC Metals:

and for BCC Metals:

where:

and the relationship between heat capacity and temperature is given by:

Cp = G1 + G2T + G3T2 + G4T3

An equation of state must also be defined with the Zerilli-Armstrong model.

Input the density (DENS), elastic modulus (EX) and Poisson’s ratio (NUXY) with the MP command. Input the parameters described below with TB,EOS and locations 1-19 of the TBDATA command:

TB,EOS,,,,3,EOSOPT
TBDATA,1,εo (initial strain)
TBDATA,2,N (strain exponent for BCC metals)
TBDATA,3,Troom (room temperature)
TBDATA,4,PC (pressure cutoff value)
TBDATA,5,SPALL (Spall type. Set SPALL = 1.0 to use minimum pressure limit; SPALL = 2.0 to use maximum principal stress; SPALL = 3.0 to use minimum pressure cutoff.)
TBDATA,6,C1 (flow stress coefficient)
TBDATA,7,C2 (flow stress coefficient)
TBDATA,8,C3 (flow stress coefficient)
TBDATA,9,C4 (flow stress coefficient)
TBDATA,10,C5 (flow stress coefficient)
TBDATA,11,C6 (flow stress coefficient)
TBDATA,12,εFAIL (failure strain)
TBDATA,13,B1 (temperature coefficient)
TBDATA,14,B2 (temperature coefficient)
TBDATA,15,B3 (temperature coefficient)
TBDATA,16,G1 (heat capacity coefficient)
TBDATA,17,G2 (heat capacity coefficient)
TBDATA,18,G3 (heat capacity coefficient)
TBDATA,19,G4 (heat capacity coefficient)

When using the Zerilli-Armstrong Model, you can define one of three types of equations of state: Linear Polynomial (EOSOPT = 1), Gruneisen (EOSOPT = 2), and Tabulated (EOSOPT = 3). Each has its own set of required constants that are input starting with position (LOC) 20 of the TBDATA command. See the descriptions of the three equation of state models in Equation of State Models.

7.2.6.8. Steinberg Model

This material model is used for modeling high strain rate effects in solid elements with failure. The yield strength is a function of both temperature and pressure. The model must be defined with an equation of state.

The Steinberg material model was originally developed for treating plasticity at very high strain rates (105 s-1) where the influence of strain rate variation on the material's yield stress begins to saturate out. In this model, the shear modulus (G) and the yield strength (σy) both increase with pressure but decrease with temperature. Both G and σy approach zero as the melting temperature of the material is reached.

In this model, the shear modulus before the material melts is defined by:

where Go, b, h, and f are experimentally determined material constants, p is the pressure, V is the relative volume, and Ec is the cold compression energy:

and Em is the melting energy:

which is in terms of the melting temperature Tm(x):

and the melting temperature at ρ = ρo, Tmo.

In the above equations,   is defined by

where R is the gas constant and A is the atomic weight. If   is not defined, LS-DYNA computes it with R in the cm-gram-microsecond system of units.

The yield strength is given by:

if Em exceeds Ei. Here, is given by:

where εi is the initial plastic strain. Whenever exceeds σm, is set equal to σm. After the material melts, σy and G are set to one half their initial values.

If the coefficients EC0-EC9 are not defined in the input, LS-DYNA will fit the cold compression energy to a ten term polynomial expansion either as a function of μ or η, depending on the input variable FLAG:

where ECi is the ith coefficient, and:

A linear least squares method is used to perform the fit.

A choice of three spall models is offered to represent material splitting, cracking, and failure under tensile loads. The pressure limit model, SPALL = 1, limits the hydrostatic tension to the specified value, pcut. If pressures more tensile than this limit are calculated, the pressure is reset to pcut. This option is not strictly a spall model, since the deviatoric stresses are unaffected by the pressure reaching the tensile cutoff, and the pressure cutoff value, pcut, remains unchanged throughout the analysis. The maximum principal stress spall model, SPALL = 2, detects spall if the maximum principal stress, σmax, exceeds the limiting value -pcut. Note that the negative sign is required because pcut is measured positive in compression, while σmax is positive in tension. Once spall is detected with this model, the deviatoric stresses are reset to zero, and no hydrostatic tension (p < 0) is permitted. If tensile pressures are calculated, they are reset to 0 in the spalled material. Thus, the spalled material behaves as a rubble or incohesive material. The hydrostatic tension spall model, SPALL = 3, detects spall if the pressure becomes more tensile than the specified limit, pcut. Once spall is detected the deviatoric stresses are reset to zero, and nonzero values of pressure are required to be compressive (positive). If hydrostatic tension (p < 0) is subsequently calculated, the pressure is reset to 0 for that element.

Input the shear modulus (GXY) and density (DENS) with the MP command. Input the parameters described in the above equations with TB,EOS and locations 1–28 of the TBDATA command.

TB,EOS,,,5,EOSOPT
TBDATA,1,σo (initial yield stress)
TBDATA,2,β (hardening coefficient)
TBDATA,3,n (hardening parameter)
TBDATA,4,εi (initial plastic strain)
TBDATA,5,σm (maximum yield stress)
TBDATA,6,b (shear modulus parameter)
TBDATA,7,b' (Steinberg yield strength parameter)
TBDATA,8,h (Steinberg yield strength parameter)
TBDATA,9,f (Steinberg exponential coefficient)
TBDATA,10,A (atomic weight)
TBDATA,11,Tmo (absolute melting temperature)
TBDATA,12,γo (melting temperature parameter)
TBDATA,13,a (melting temperature parameter)
TBDATA,14,PC (pressure cutoff, pcut)
TBDATA,15,SPALL (Spall type. Set SPALL = 1 to use the pressure limit spall model; set SPALL = 2 to use the maximum principal stress spall model; set SPALL = 3 to use the hydrostatic tension spall model.)
TBDATA,16,FLAG (cold compression energy flag)
TBDATA,17,MMN (minimum bulk modulus)
TBDATA,18,MMX (maximum bulk modulus)
TBDATA,19-28,EC0-EC9 (cold compression energy constants)

When using the Steinberg Model, you can define one of three types of equations of state: Linear Polynomial (EOSOPT = 1), Gruneisen (EOSOPT = 2), and Tabulated (EOSOPT = 3). Each has its own set of required constants that are input starting with position (LOC) 29 of the TBDATA command. See the descriptions of the three equation of state models in Equation of State Models.

For an example input listing using the Gruneisen EOS, see Steinberg Gruneisen EOS Example: Stainless Steel.

7.2.7. Discrete Element Models

7.2.7.1. Linear Elastic Spring Model

This model provides a translational or rotational elastic spring located between two nodes. Input the spring elastic stiffness with the TB,DISCRETE,,,,0 and location 1 of the TBDATA command:

TB,DISCRETE,,,,0
TBDATA,1,KE (Elastic stiffness (force/displacement) or (moment/rotation))

7.2.7.2. General Nonlinear Spring Model

This model provides general nonlinear translational or rotational spring with arbitrary loading and unloading definitions located between two nodes. Hardening and softening can be defined. Input the model parameters with the TB,DISCRETE,,,,5 and locations 1 to 5 of the TBDATA command:

TB,DISCRETE,,,,5
TBDATA,1,LCDL (Load curve ID describing force vs. displacement or moment vs. rotation relationship for loading)
TBDATA,2,LCDU (Load curve ID describing force vs. displacement or moment vs. rotation relationship for unloading)
TBDATA,3,BETA (Hardening parameter)
TBDATA,4,TYI (Initial yield force in tension (= 0: Tensile and compressive yield with strain softening; ≠ 0: Kinematic hardening without strain softening; = 1: Isotropic hardening without strain softening.))
TBDATA,5,CYI (Initial yield force in compression (< 0))

7.2.7.3. Nonlinear Elastic Spring Model

This model provides nonlinear elastic translational or rotational spring with arbitrary force/displacement or moment/rotation dependency. Input the model parameters with the TB,DISCRETE,,,,3 and locations 1 and 2 of the TBDATA command:

TB,DISCRETE,,,,3
TBDATA,1,LCID (Load curve ID (force/displacement or moment/rotation))
TBDATA,2,LCR (Optional load curve ID describing scale factor on force or moment as a function of relative velocity or rotational velocity, respectively.)

7.2.7.4. Elastoplastic Spring Model

This model provides elastoplastic translational or rotational spring with isotropic hardening located between two nodes. Input the spring elastic stiffness, tangent stiffness and yield force with the TB,DISCRETE,,,,2 and locations 1 to 3 of the TBDATA command:

TB,DISCRETE,,,,2
TBDATA,1,KP (Elastic stiffness (force/displacement) or (moment/rotation))
TBDATA,2,KT (Tangent Stiffness (force/displacement or moment/rotation))
TBDATA,3,FY (Yield (force) or (moment))

7.2.7.5. Inelastic Tension- or Compression-Only Spring Model

This model provides an inelastic tension or compression only, translational or rotational spring located between two nodes. Optionally, the user can define unloading stiffness instead of the maximum loading stiffness. Input the model parameters with the TB,DISCRETE,,,,7 and locations 1 to 3 of the TBDATA command:

TB,DISCRETE,,,,7
TBDATA,1,LCFD (Load curve ID describing arbitrary force/torque vs. displacement/twist relationship. Must be defined in the positive force-displacement quadrant, regardless of whether the spring acts in tension or compression.)
TBDATA,2,KU (Unloading stiffness. The maximum of KU and the maximum loading stiffness in the force/displacement or the moment/twist curve is used for unloading.)
TBDATA,3,CTF (Compression or tension indicator: – 1.0 is tension only, 0.0 is compression only (default), 1.0 is compression only.)

7.2.7.6. Maxwell Viscosity Spring Model

This model provides a three parameter Maxwell viscoelastic translational or rotational spring located between two nodes. Optionally, a cutoff time with a remaining force/moment can be defined. Input the model parameters with the TB,DISCRETE,,,,6 and locations 1 to 6 of the TBDATA command:

TB,DISCRETE,,,,6
TBDATA,1,Ko (Short time stiffness)
TBDATA,2,KI (Long time stiffness)
TBDATA,3,BETA (Decay parameter)
TBDATA,4,TC (Cutoff time, after which a constant force/moment is transmitted)
TBDATA,5,FC (Force/moment after cutoff time)
TBDATA,6,COPT (Time implementation option)

7.2.7.7. Linear Viscosity Damper Model

This model provides linear translational or rotational damper located between two nodes. Input the damping constant with the TB,DISCRETE,,,,1 and location 1 of the TBDATA command:

TB,DISCRETE,,,,1
TBDATA,1,DC (Damping constant (force/displacement rate) or (moment/rotation rate))

7.2.7.8. Nonlinear Viscosity Damper Model

This model provides a nonlinear damping spring with arbitrary force/velocity or moment/rotational velocity dependency located between two nodes. The load curve must define the response in the negative and positive quadrants and pass through point (0, 0). Input load curve ID with the TB,DISCRETE,,,,4 and location 1 of the TBDATA command:

TB,DISCRETE,,,,4
TBDATA,1,LCID (Load curve ID describing force vs. rate-of-displacement relationship or moment vs. rate-of-rotation relationship. The load curve must define the response in the negative and positive quadrants and pass through point (0, 0). )

7.2.7.9. Cable Model

Use this model to realistically model elastic cables. No force will develop in compression. The force, F, generated by the cable is nonzero if and only if the cable is in tension. The force is given by:

F = K x max(ΔL,0.)

where ΔL is the change in length

ΔL = current length - (initial length - offset)

and the stiffness is defined as:

The area and offset are defined by means of the real constants for LINK167. For a slack cable, the offset should be a negative length. For an initial tensile force, the offset should be positive. If a load curve is specified, Young’s modulus is ignored and the load curve is used instead. The points on the load curve are defined as engineering stress versus engineering strain, i.e., the change in length over the initial length.

Use the MP and EDMP commands to input the required values:

MP,DENS
MP,EX
EDMP,CABLE,MAT,Load Curve ID

For an example input listing, see Cable Material Example: Steel.

7.2.8. Other Models

7.2.8.1. Rigid Model

Rigid bodies are defined for a material type using the command EDMP. For example, to define a rigid body for material 2, issue: EDMP,RIGID,2. All elements defined with the specified material number are then considered to be part of that rigid body. This material number, along with the element type and real constant type numbers of the elements, will define the PART ID of the rigid body. This PART ID can then be used to define loads and constraints to the rigid body (as described in Loading). Elements within a rigid body do not have to be linked by mesh connectivity. Therefore, to represent more than one independent rigid body in a model, multiple rigid material types must be specified. Two independent rigid bodies, however, cannot share a common node.

Along with the EDMP command, you must use the MP command to specify Young's modulus (Ex), Poisson’s ratio (NUXY), and density (DENS) for the rigid body’s material type. Realistic material property values are required so that the stiffness of the contact surfaces can be calculated by the program. For this reason, never use unrealistically high values of Young’s modulus or density for a rigid body in an explicit dynamic analysis. A rigid body cannot be stiffened because it is perfectly rigid.

Because the motion of the mass center of a rigid body is transferred to its nodes, constraints should not be applied to rigid bodies using the D command. The constraints and initial velocities of one node of a rigid body will be transferred to the center of mass of the body. However, if more than one node is constrained, it is hard to determine which constraints will be used. To properly apply constraints to a rigid body, the translational (VAL1) and rotational (VAL2) constraint parameter fields of the EDMP command are used as shown below:

VAL1 - Translational constraint parameter (relative to global Cartesian coordinates)

0No constraints (default)
1Constrained X displacement
2Constrained Y displacement
3Constrained Z displacement
4Constrained X and Y displacements
5Constrained Y and Z displacements
6Constrained Z and X displacements
7Constrained X, Y, and Z displacements

VAL2 - Rotational constraint parameter (relative to global Cartesian coordinates)

0No constraints (default)
1Constrained X rotation
2Constrained Y rotation
3Constrained Z rotation
4Constrained X and Y rotations
5Constrained Y and Z rotations
6Constrained Z and X rotations
7Constrained X, Y, and Z rotations

For example, the command EDMP,RIGID,2,7,7 would constrain the rigid body elements of material 2 in all degrees of freedom.

After defining a rigid body, you can assign inertia properties, mass, and an initial velocity vector to that body using the EDIPART command. If you do not specifically define the inertia properties for a rigid body, the program will calculate them based on the finite element model.

For an example input listing, see Rigid Material Example: Steel.


Release 18.2 - © ANSYS, Inc. All rights reserved.