Tetrahedral Elements

Tetrahedral elements are 4- or 10-node isoparametric or sub-parametric curvilinear tetrahedra. Figure 1 illustrates some typical elements. Figure 2 shows an example of a tetrahedral element.

Figure 1: A Typical Tetrahedral Element

Figure 2: A Typical Application for a Tetrahedral Element

Determination of Surface Number for Tetrahedral Elements

When applying loads to a surface number of a tetrahedral part, be aware that some models may not have all the lines on the face to be loaded on the same surface number. What happens in this situation? If the model originated from a CAD solid model, all faces coincident with the surface of the CAD model will receive the load regardless of the surface number of the lines. In hand-built models and on CAD parts that are altered so that the part is no longer associated with the CAD part, the surface number that is common in any two of the three lines that define a face determines the surface number of that face.

Tetrahedral Element Parameters

First, you must specify the material model for this part in the Material Model list box under the Element Definition dialog. The available material models are grouped in the following categories. Refer to the appropriate page under the Material Properties page for details on each of the material models.

For the tetrahedral elements in this part to have the midside nodes activated, select the Included option in the Midside Nodes drop-down box. If this option is selected, the tetrahedral elements will have additional nodes defined at the midpoints of each edge. (For meshes of CAD solid models, the midside nodes follow the original curvature of the CAD surface, depending on the option selected before creating the mesh. For hand-built models and CAD model meshes that are altered, the midside node is located at the midpoint between the corner nodes.) This will change a 4-node tetrahedral element into a 10-node tetrahedral element. An element with midside nodes will result in more accurately calculated gradients. This is especially useful when trying to model bending behavior with few elements across the bending plane. Elements with midside nodes increase processing time. If the mesh is sufficiently small, then midside nodes may not provide any significant increase in accuracy.

Use the Analysis Type drop-down to set the type of displacement that is expected. Small Displacement is appropriate for parts that experience no motion and only small strains and will ignore nonlinear geometric effects that result from large deformation. (It also sets the Analysis Formulation on the Advanced tab to Material Nonlinear Only.) Large Displacement is appropriate for parts that experience motion and/or large strains. (The Analysis Formulation on the Advanced tab should also be set as required for the analysis.)

Tip:
  • The displacement at midside nodes is always output. The stress and strain at midside nodes are output only if the user activates the option to output these results before running the analysis. The option is located under the SetupModel SetupParametersAdvanced dialog on the Output tab. (See the Control Output Files page for details.)
  • Use the Options Analysis tab and set the Use large displacement as default for nonlinear analyses option to control whether the Analysis Type defaults to small or large displacement.

DefineThermal Properties of Tetrahedral Elements

Thermal Section:

If a tetrahedral element part is using a material model that includes thermal effects, you must specify a value in the Stress free reference temperature field in the Thermal tab of the Element Definition dialog. This value is used as the reference temperature to calculate element-based loads associated with constraint of thermal growth using bilinear interpolation of the nodal temperatures.

Creep Section:

If a tetrahedral element part is using a material model that includes creep, select the option in the Creep law drop-down box. This selection will be used to calculate the creep effects during the analysis. The creep laws available are as follows:

  • No creep: When this option is chosen, no creep effects are included in the analysis.
  • Power-law: This option is also known as the uniaxial creep law. The equation is = C 1 x C2 x t C3 .
  • Garofalo: This option is also known as the hyperbolic sine creep law. The equation is = A 0 x [sinh(A 1 x )] A2 .
  • Double power-law: This option is similar to the power law but with an additional term to produce results closer to experimental results at high stress levels. The equation is = C 1 x C 2 x t C3 + C 4 x C5 x t C6 .

where is the effective creep strain rate and is the effect stress. Also refer to the Thermal Creep Viscoelastic Material Properties page for important information on entering the material properties.

For the creep calculations to be calculated on evenly sized divisions of the time step, select the Fixed substeps option in the Time integration method drop-down box. For the creep calculations to be calculated on variable sized divisions of the time step, select the Flexible substeps option. These two methods are based on time hardening and use explicit time integration methods. These methods may become unstable under some loading conditions. When using the Thermal Viscoelastic Creep material model and the Creep strain definition drop-down box is not set to Modified, an additional option will be available in the Time integration method drop-down box: the Alpha-method. This method uses an implicit time integration scheme to improve the creep behavior. This method can be unconditionally stable.

Specify the temperature at which no thermal stress exists in the Stress free reference temperature field.

If you are performing an analysis with non-cyclical loading, select the Effective option in the Creep strain definition drop-down box. If you are performing an analysis with cyclical loading, select the Modified option.

During the analysis, the creep calculations will be performed as iterations in substeps of each time step. You can control how many substeps are allowed in a single time step in the Maximum number of substeps field. You can also specify how many iterations can be performed in a single substep in the Maximum number of iterations in a substep field. After each substep iteration, the creep stress and strain will be compared to the previous iteration. If the value is not within the tolerances specified in the Creep strain calculation tolerance and Creep stress calculation tolerance fields, another iteration will be required.

When using a Time integration method of Alpha-method, the Time integration parameter needs to be specified. To use a fully explicit method for the time-integration scheme (but different than the fixed/flexible substeps' explicit method), type 0.0 in the Time integration parameter field. To use a fully implicit method, type 1.0 in the Time integration parameter field. When the Time integration parameter is greater than 0.5, this method is unconditionally stable.

Control Orientation of Tetrahedral Elements

If this part of tetrahedral elements is using an orthotropic material model, you will need to define the orientation of material axes 1, 2 and 3 in the Orthotropic tab of the Element Definition dialog. There are two basic methods to accomplish this.

Method 1:

The first method is to select one of the global axes as material axis 1. If you select the Global X-direction option in the Material axis direction specified using drop-down box, the orthogonal material axes follow the X, Y and Z axes as follows:

If you select the Global Y-direction option in the Material axis direction specified using drop-down box, the orthogonal material axes follow the X, Y and Z axes as follows:

If you select the Global Z-direction option in the Material axis direction specified using drop-down box, the orthogonal material axes follow the X, Y and Z axes as follows:

With the first method, the axes can be rotated about the chosen global direction by entering an angle in the Material Axis Rotation Angle field. This angle follows the right-hand rule.

Method 2:

The second method is to select the Spatial Points option in the Material axis direction specified using drop-down menu. Next you must define the coordinates for three spatial points in the Spatial point coordinates table. Next, select the appropriate index for the spatial points in the Index of spatial point 1, Index of spatial point 2, and Index of spatial point 3 drop-down menus.

Figure 3: Orientation of Material Axes

Attention: The spatial point coordinates are shared by all of the parts in the model. Changing any of the coordinates in one part affects all other parts that use the same spatial point. However, since more than three points can be defined in the Spatial point coordinates table, and any point can be chosen for each of the indices (in any order), the orientation can vary for different parts.

Advanced Tetrahedral Element Parameters

Analysis Formulation: Select the formulation method that you want to use for the tetrahedral elements in the Analysis Formulation drop-down box in the Advanced tab.

Stress Update Method:

The Stress Update Method is used when the material model (on the General tab) is set to one of the following plastic material models:

  • von Mises with Isotropic Hardening
  • von Mises with Kinematic Hardening
  • von Mises curve with Isotropic Hardening
  • von Mises curve with Isotropic Hardening

This controls the numerical algorithm for integrating the constitutive equations (stress/strain law) when the material goes plastic. The options available for the Stress Update Method are as follows:

  • Explicit: (Original method). This option uses the explicit sub-incremental forward-Euler method for integrating the constitutive equations. The Explicit option is best used for simple problems, such as simple tension, because the method runs faster. However, it is more sensitive to the loading, time step size, and complexity of the material stress-strain curve.
  • Generalized Mid-Point: This option uses an implicit method for integrating the constitutive equations. It reduces the error accumulation and can ensure that the stress updating process is unconditionally stable. Thus, this option is better suited for complicated analyses, such as contact problems, severe plasticity, or complex material stress-strain curves.

Stress Update Method Guidelines:

  • Verify that the analysis results make sense (that is, that they follow the expected behavior). For example, if there is symmetry in the geometry, loads, and boundary conditions, symmetrical results are expected (except for anisotropic materials). If the results are counterintuitive or if there are discontinuities or instability in the solution, change the Stress Update Method or increase the updating rate of the variables, as discussed in the next guideline.
  • Whether you choose Explicit or Generalized Mid-Point, more frequent updating of the stress and strain variables improves the solution for plastic material models. Use one of the following methods to increase the updating rate:
    1. Reduce the time step size (increase capture rate) in the Analysis Parameters.
    2. Instead of Automatic or Combined Newton, choose the Full Newton option for the Nonlinear iterative solution method in the Equilibrium tab of the Analysis Parameters - Advanced dialog box.
  • The Generalized Mid-Point method is typically able to tolerate larger time steps than the Explicit method – while obtaining more accurate results – but it is computationally more expensive.
  • Background: Integrating the constitutive relations to obtain unknown stress increments is crucial to mechanical event simulation (MES). These relations define a set of ordinary differential equations, and methods for integrating them are usually classified as explicit or implicit. The explicit method only looks forward. That is, the slope of the material stress-strain curve is chosen at the beginning of an increment, and this slope is used to calculate stress at the end of the increment. For the implicit method, the solver looks forwards and backwards, and the slope has to be calculated using multiple iterations. The strain increment is multiplied by the slope of the stress-strain curve to determine the stress.

    In the Explicit integration scheme, the yield surface, plastic potential gradients, and hardening law are all evaluated at known stress states. No particular iteration is strictly necessary to predict the final stresses.

    In the Generalized Mid-Point scheme (which is a type of implicit method), simple iterative adjustment restores the next increment's stresses and hardening parameters to the yield surface, since this condition is not enforced by the integration. This correction requires additional effort for solving the nonlinear equations iteratively. Conversely, explicit methods do not require the solution of a system of nonlinear equations to compute the stresses at each Gauss point.

The Parameter for Generalized Mid-point input is used when the Stress Update Method is set to Generalized Mid-Point. Acceptable ranges for this input are 0 to 1, inclusive. When the Parameter is set equal to 0, the resulting algorithm would be a fully explicit member of the algorithm family (similar to the Explicit option for the Stress Update Method); however, the solution is not unconditionally stable. When the Parameter is 0.5 or larger, the method is unconditionally stable. When the Parameter is set to 0.5, the solution is known as a mid-point algorithm; when it is 1, the solution is known as the fully backward Euler or closest point algorithm and is fully implicit. A value of 1 is more accurate than other values, especially for large time steps.

Strain Measurements:

The Strain Measurements is used when the Material Model (on the General tab) is set to Isotropic and the Analysis Formulation is set to Updated Lagrangian. The options are used to improve the convergence of the updated Lagrangian method. The options available for the Strain Measurements are as follows:

  • Almansi Strain: (Original method). This option uses the Cauchy stress and Almansi strain for the constitutive relation. It is limited to cases of small strain.
  • Log-strain: This option uses the Cauchy stress and virtual log-strain (incremental strain) for the constitutive relation. It is acceptable for all cases, including large strain. This is a hypoelastic model, and one drawback is that it works better for incompressible material (Poisson ratio = 0.5) than compressible materials. This is because the shear modulus is assumed to be a constant where as it changes with the varying volume in reality.

Overlapping Elements:

If the Allow for overlapping elements check box is activated, overlapping elements will be allowed to be created when the lines are decoded into elements. Overlapping may be necessary when modeling elements. This is especially true for problems confined to planar motion.

Output Options:

For the stress results for each element to be written to the text log file at each time step during the analysis, activate the Detailed force and moment output check box. This may result in large amounts of output data.

If one of the von Mises material models has been selected, you can choose to have the current material state (elastic or plastic), current yield stress limit, current equivalent stress limit and equivalent plastic strain output at corner nodes and/or integration points at every time step. This is done by selecting the appropriate option in the Additional output drop-down box.

Selective Reduced Integration (Mean-dilatation):

Many physical problems involve motions that essentially preserve volumes. Materials that behave in this fashion are termed incompressible. For example, rubber and metals with rigid-plastic flow are nearly incompressible. Activating the Selective Reduced Integration (Mean-dilatation) check box will add a modification to the usual compressible FEA formulations that represents the incompressible limit and high-compressible volume change. This method (B-Bar) helps avoid the volumetric locking.

When not activated (unchecked), the dilatational components of deformations (volume related) are integrated at the same order with the deviatoric components. When activated (checked), the mean value is used to compute the dilatational contribution.

Two examples in which this option will benefit the analysis are as follows:

  1. Material Properties: In isotropic linear elasticity, the condition of incompressibility may be expressed in terms of Poisson’s ratio. As the Poisson ratio approaches 0.5, resistance to volume change is greatly increased - assuming resistance to shearing remains constant. In another word, the bulk modulus approaches infinity.
  2. Material Models and Deformation: In elasto-plastic material models, the plastic deformation is much larger than the elastic deformation, and mechanical theory assumes there is no volume change in plastic deformation. Thus, the material is practically constant volume. Similar assumptions also exist in other nonlinear material models.

To activate the Selective Reduced Integration (Mean-dilatation) check box, the Compatibility must be set to Enforced.

Piezoelectric Material Options:

When one of the piezoelectric material models has been chosen for a part, two additional options will become available within the Advanced tab of the Element Definition dialog box...

  • Use the Nodal voltage load curve input field to specify the number of the load curve that will be used to control all nodal voltages throughout the analysis event.
  • Voltage differentials applied across piezoelectric materials produce an electrical field that causes the piezoelectric part to deform slightly. The amount of strain is typically small. The deformation of the part has a small effect on the electrical field, which in turn has a slight effect on the resultant piezoelectric deformation. To take this effect into account, activate the Update electric field checkbox. Otherwise, the electrical field will be based on the initial (undisplaced) condition of the part.

Define Soil Conditions

If the Duncan-Chang material model is chosen, the Soil tab is enabled. Enter the following input as appropriate for the analysis. This input is related to the initial state of the soil; also see the page Setting Up and Performing the Analysis: Nonlinear: Material Properties: Duncan-Chang Material Properties: Duncan-Chang Theoretical Description for information.

Basic Steps for Use of Tetrahedral Elements

  1. Be sure that a unit system is defined.
  2. Be sure that the model is using a nonlinear analysis type.
  3. Right-click the Element Type heading for the par that you want to be brick elements.
  4. Select the Tetrahedral command.
  5. Right-click the Element Definition heading.
  6. Select the Edit Element Definition command.
  7. In the General tab, select the appropriate material model in the Material Model drop-down box.
  8. If you selected the Temperature Dependent Plasticity, Temperature Dependent Isotropic, Viscoplastic, or Viscoelastic option in the Material Model drop-down box, specify the necessary information in the Thermal tab.
  9. Press the OK button.

Parent topic: Solid Elements