20. Other In-Development Capabilities
This chapter describes other miscellaneous capabilities that are still in development or have limited testing.
20.1. Element Birth (Element Activation)
BEGIN ELEMENT BIRTH <string>birth_name
BLOCK = <string list>block_names
BIRTH START TIME = <real>time
CRITERION IS ELEMENT VALUE OF
<string>var_name <|<=|=|>=|> <real>tolerance
[<integer>num_intg INTEGRATION POINTS REMAIN]
CRITERION IS AVG|MAX|MIN NODAL VALUE OF
<string>var_name <|<=|=|>=|> <real>tolerance
CRITERION IS GLOBAL VALUE OF
<string>var_name <|<=|=|>=|> <real>tolerance
END
A limited element birth/activation capability is provided for the target use cases of additive manufacturing and welds.
Elements are birthed upon an element variable, nodal variable, or global variable criterion. See Element Death section of the Sierra/SM User Manual for tips on properly setting up death/birth criteria based on a registered variable.
This capability is currently implemented for UG Hex8 elements with isotropic hypoelastic materials only.
Element birth works with thermal strains. Inactive elements do not accumulate thermal strains.
Element birth will error if a node is shared between an element birth block and a block involving: contact, force external boundary conditions, and kinetic boundary conditions.
20.2. Initial Particle Conversion
BEGIN CONVERSION TO PARTICLES AT INITIALIZATION <string>name
BLOCK = <string list>block_names
ASSEMBLY = <string list>assembly_names
SECTION = <string>section_name
END
The initial particle conversion capability is provided to facilitate the creation of particle meshes for particle based methods—such as smooth particle hydrodynamics (SPH) or reproducing kernel particle method (RKPM)—from an initial mesh of solid elements (e.g., hexes).
At the beginning of the analysis the solid element blocks listed in block_names, or assemblies of solid element blocks listed in assembly_names are converted to spherical particles of the type defined in the particle section section_name. It is important to note that the particle section will thus supersede any section specified in the original solid element block definition (consult Sierra/SM User Manual section on Element Block Parameters).
Note that elements may also be converted to particles via element death (consult Sierra/SM User Manual section on Element Death); however, conversion at initialization should offer more robust creation of particle meshes that are (a) compatible with the original mesh boundary conditions and (b) amenable to the chosen particle formulation methodology.
20.3. Shell Contact Lofting Factor
Warning
The shell contact lofting factor only works with Dash contact.
BEGIN SHELL SECTION <string>shell_section_name
# ... see the Elements chapter of Sierra/SM User Manual
CONTACT LOFTING FACTOR = <real>contact_lofting_factor
END [SHELL SECTION <string>shell_section_name]
The CONTACT LOFTING FACTOR line command is available in the SHELL SECTION command block to set a lofting factor specifically for use in contact. This contact lofting factor is used in place of the kinematic lofting factor for creation of the shell lofted geometry in contact. If no contact lofting factor is set, the kinematic lofting factor is used for contact.
The contact lofting factor has no effect on the shell element kinematics, and the LOFTING FACTOR and CONTACT LOFTING FACTOR line commands may be used in combination to independently set the kinematic and contact lofting factors, respectively.
20.4. Discrete Element Method (DEM)
The discrete element method is a particle based element formulation. This method is in early development, experimental, and currently not recommended for use.
BEGIN DEM OPTIONS
...
END
BEGIN DEM SECTION
...
END
20.5. Q1P0 Element
A selectively integrated formulation is specified with the command FORMULATION = Q1P0. This is only available for 8-node hexahedral element blocks.
BEGIN SOLID SECTION <string>solid_section_name
...
FORMULATION = Q1P0
...
Q1P0 STABILIZATION THRESHOLD = <real>threshold(0.0)
Q1P0 TIMESTEP SCALE FACTOR = <real>scale_factor(0.95)
Q1P0 TIMESTEP WAVE SPEED = <string>VOLUMETRIC|SHEAR|
AUTOMATIC(AUTOMATIC)
Q1P0 TIMESTEP LENGTH SCALE = <string>DEFORMED_NODAL_DISTANCE|
MINIMUM_MAPPING_STRETCH|INSCRIBED_SPHERE_DIAMETER
(MINIMUM_MAPPING_STRETCH)
END [SOLID SECTION <string>solid_section_name]
In the Q1P0 element formulation, the internal forces arising from material stress are selectively integrated. Forces arising from the pressure component of the stress are integrated using a single integration point while forces arising from the deviatoric stress are integrated using a \(2\times 2\times 2\) Gauss rule.
The only STRAIN INCREMENTATION option available for this element is STRONGLY_OBJECTIVE.
When post-processing information such as the plastic strain with this element, information at the first integration point should typically be used as it is more accurate than at any other point. The first integration point corresponds to the location at the center of the element where the pressure response is evaluated.
Warning
Material model evaluations at the Q1P0 element’s deviatoric integration points can result in spurious high and low locked pressures for incompressible (or nearly incompressible) material models. The Q1P0 element avoids the pressure locking when calculating the internal forces (for the balance of linear momentum) by discarding the pressures calculated at the deviatoric integration points and replacing them with the pressure from the central integration point. Note that the locked pressures are replaced during element calculations, not inside the constitutive model. This means that material models and element death criteria that fail or accumulate damage based on pressure may be adversely affected by this deviatoric pressure locking. For this reason, the selective-deviatoric (SD) element is generally preferred for material failure analyses. The SD element calculates a single average element volumetric strain and passes that average volumetric strain to all material integration points. The volume averaging of strain in the SD element prevents pressure locking in the material constitutive equations and in the overall element response.
Stress-based values such as stress and values derived from it such as von_mises are evaluated using a stress tensor taken from a volumetric average of the 8 deviatoric Gauss points for the deviatoric response combined with a pressure response at the central integration point.
The Q1P0 STABILIZATION THRESHOLD command modifies the formulation to provide additional stabilization as elements become distorted at the cost of accuracy. If a simulation produces inverted elements, these may be able to be mitigated by providing a value of 0.25. One may look at the stabilization_factor element variable to determine if this option is being activated in the analysis. A value of 0 in this variable corresponds to a fully q1p0 formulation while a value of 1 corresponds to a fully integrated formulation. Keep in mind that if this is changed from the default value of 0, the formulation is no longer truly Q1P0.
Explicit only
Three additional parameters are available to select how the critical time step is evaluated, Q1P0 TIMESTEP SCALE FACTOR, Q1P0 TIMESTEP WAVE SPEED, and Q1P0 TIMESTEP LENGTH SCALE. The critical time step is evaluated using the following formula:
The Q1P0 TIMESTEP SCALE FACTOR = scale_factor command scales the calculated time step for elements with this section. The default of 0.95 should be sufficient for almost all analyses. Lowering this slightly may provide better results in certain circumstances. If another time step scale factor is specified within the PARAMETERS FOR PRESTO REGION block, they are effectively multiplied together for elements using this section.
The Q1P0 TIMESTEP WAVE SPEED command chooses the wave speed used by the time step calculation. The default, AUTOMATIC, should be sufficient for all analyses. The VOLUMETRIC option calculates wave speed using the bulk modulus while the SHEAR option uses the shear modulus. The AUTOMATIC option uses the maximum of the other two options.
The Q1P0 TIMESTEP LENGTH SCALE selects the method used to calculate the length scale of the element. The default MINIMUM_MAPPING_STRETCH option calculates this as the minimum stretch from the mapping between a unit cube and the current configuration of the element. While this option is relatively slow, it is robust. The DEFORMED_NODAL_DISTANCE option calculates this as the minimum non-zero node to node distance within the element. This is the fastest option and a potential increase in speed is achieved by selecting it at the cost of robustness. The INSCRIBED_SPHERE_DIAMETER option calculates this as the diameter of the largest sphere which can fit inside the element.