Round Notched Tension Model

MatCal’s RoundNotchedTensionModel is meant to be used in calibrations requiring the simulation of a round notched tension test where higher stress triaxialities are required for parameter calibration. This model has all the MatCal standard model features as described in MatCal SIERRA Solid Mechanics Standard Models. In this section, we will provide more information about how the geometry is generated, specifics on simulation boundary conditions, and what is output from the model.

Note

Some examples and V&V studies that include these models are:

  1. Comparing iterative, staggered and adiabatic coupling solutions

Notched tension geometry and mesh generation

This model has geometry parameters similar to those in the RoundUniaxialTensionModel. The only differences are the addition of parameters regarding the notch geometry, notch_radius and notch_gauge_radius, and the removal of the inapplicable taper parameter. For the geometry to be accurately built, the model requires the following keyword arguments be provided to its constructor.

  1. total_length

  2. gauge_length

  3. extensometer_length

  4. fillet_radius

  5. grip_contact_length - distance that the grips contact the specimen in the grip section.

  6. necking_region (optional) - the fraction of the extensometer length where necking is expected to occur. This is used for output and mesh refinement for some of the mesh_methods.

  7. element_size - target element edge length

  8. mesh_method - user specified meshing method options

  9. gauge_radius

  10. grip_radius

  11. notch_radius

  12. notch_gauge_radius

The necking_region geometry input is optional for this model. It specifies the fraction of the extensometer length where necking is expected to occur and is used for output and mesh refinement for some of the mesh_methods. If the user does not provide necking_region or provides a value of zero, MatCal automatically selects a default value based on the notch geometry and the model symmetry.

For the round notched tension model, the automatic default is determined as follows:

  1. If notch_radius is less than gauge_radius, the necking-region length in the half-symmetry model is set to 1.2\,\text{notch\_radius}.

  2. Otherwise, the necking_region value is set such that it corresponds to 37.5% of the total notch height.

  3. The corresponding necking_region parameter value is then computed from that necking-region length using the model relation \text{necking\_region\_length} = \text{necking\_region}\,\text{extensometer\_length}/2.

If the user provides a valid, nonzero necking_region, that value is used directly.

These parameters provide information related to geometry, discretization sizing and output and boundary condition mesh entities such as blocks and node sets. The geometric parameters are shown in Fig. 7.

_images/round_notched_tension_bcs_and_dimensions.png

Fig. 7 The geometric dimensions and boundary conditions for the round notched tension model.

The keyword element_size is used to specify the approximate element edge length that Cubit will target in the mesh. Depending on the meshing_method chosen, this could be the entire model or just a subregion of the model. The meshing_method parameter allows the user to change how the geometry is meshed. Differences in the 5 meshing_methods available are shown in Fig. 8 and Fig. 9. In general, low meshing_method parameters are intended for coarser meshes and result in higher element counts. In contrast, high meshing_method parameters are intended for finer meshes, result in lower element counts and begin to use Cubit numsplits for meshing_method >= 4. Note that higher number mesh_methods can result in lower resolution of geometry away from the gauge section of the specimen if the target mesh size is too coarse.

_images/mesh_method_element_sizes.png

Fig. 8 The target element sizes for different mesh_method options for different regions of the round notched tension model.

_images/mesh_method_composite.png

Fig. 9 The resulting meshes for different mesh_method options for the round notched tension model.

Currently, the entire geometry is meshed in order to support thermomechanical coupling. Since conduction into the grips and load frame may be non-negligible, the entire specimen is important to model. We have found the extra computational cost associated with including the grips to be small.

Notched tension boundary conditions

This model currently only supports \frac{1}{8}^{\text{th}} symmetry geometry, and, as a result, have boundary conditions that reflect that. The boundary conditions are shown graphically in Fig. 7. Since this model can easily be coupled with thermal modeling, the boundary condition descriptions have been separated into the following two subsections associated with the solid mechanics and thermal models.

Notched tension solid mechanics boundary conditions

The tensile loading is caused by a displacement function applied to the outer surface of the grip section block in the axial direction away from the specimen center. This function acts on the surface of the specimen where the grips would contact it, and includes nodes from the top of the specimen down by the grip_contact_length dimension. This includes all nodes on the outside radius of the grip section. These node sets are shown for the two tension specimens in Fig. 7.

The applied function is determined using the add_boundary_condition_data(). This method must be supplied a Data or DataCollection class that contains either a “displacement” field or an “engineering_strain” field for the states of interest for the model. They can also optionally include a “time” field. The add_boundary_condition_data() method determines the boundary condition function to be applied to the specimen according to the following algorithm:

  1. Determine the boundary condition by state since maximum deformation, material behavior and experiment setup can vary significantly over different states.

  2. For each state, determine the driving field for boundary condition generation:

    • If “displacement” is present, use displacement.

    • Else if “engineering_strain” is present, convert to an equivalent displacement using

      \text{displacement} = \varepsilon_{\text{eng}} \cdot \text{extensometer\_length}

  3. For each state, find the data set with the largest resulting displacement (either the provided displacement directly, or the displacement converted from engineering strain as described above) and use it for boundary condition generation.

  4. Perform no scaling on this displacement or derived displacement. This assumes that the strain is primarily localized to the notched region of the specimen.

  5. If the data does not contain a “time” field and there is not a State parameter named “displacement_rate”, then apply a linear displacement function from zero to the maximum displacement found in the data over one second.

  6. If the data does not contain a “time” field and there is a State parameter named “displacement_rate”, then apply a linear displacement function from zero to the maximum displacement found in the data. This is done over a time period beginning at zero seconds and ending at a time calculated by dividing the maximum displacement at the extensometer by the “displacement_rate” State parameter.

  7. If the data does contain a “time” field, use the displacement function directly as provided.

Note

This algorithm assumes that negligible deformation occurs in the regions outside of the notched region of the geometry. If this is known or suspected to be an invalid assumption, an additional scale factor can be applied to increase the displacement applied to the grips. Use the set_boundary_condition_scale_factor() method to add a scale factor to scale the displacement function. It must be between 1 and 10 and it directly multiplies the displacement determined from the boundary condition generation algorithm.

The remaining solid mechanics boundary conditions only include the symmetry boundary conditions where displacements normal to the symmetry surfaces are set to zero.

Notched tension thermal model boundary conditions

Since MatCal SIERRA/SM standard models only allow heat flux out of the specimen through the grips, only the grip boundary condition is described here. As discussed in the previous section, the boundary condition for the grip-to-specimen interface includes the nodes between the ends of the model geometry and grip_contact_length away from the ends of the specimen. As described in Staggered and iterative coupling, the temperature at the nodes is fixed to the value of the State parameter “temperature”. The entire body of the model is prescribed an initial temperate of State parameter “temperature” for all simulations regardless of coupling specification (uncoupled, staggered coupling, iterative coupling or adiabatic). For uncoupled simulations, this is only done if a temperature state variable is provided.

Notched tension model specific output

By default, the round notched tension model includes the following global output fields:

  1. time

  2. displacement - measured across extensometer length in the loading direction

  3. load - measured at the applied boundary condition node set in the loading direction.

  4. engineering_strain - computed as

    \varepsilon_{\text{eng}} = \frac{\text{displacement}}{\text{extensometer\_length}}

  5. engineering_stress - computed as

    \sigma_{\text{eng}} = \frac{\text{load}}{A_0}, \qquad A_0 = \pi\,(\text{notch\_gauge\_radius})^2

If coupling is activated, the following global temperature output is provided:

  1. low_temperature

  2. med_temperature

  3. high_temperature

and how they are calculated is dependent on the type of coupling. For adiabatic simulations, they are the minimum, average and maximum element temperatures in the gauge section of the model. For coupled simulations, the same quantities are provided by acting on the nodal temperatures instead of the element temperatures.