| Abaqus Keywords Reference Guide |
|
| How to find keyword examples |
| Abaqus Keywords Reference Guide |
|
| How to find keyword examples |
Warning: Using values larger than the default values for hourglass control can produce excessively stiff response and sometimes can even lead to instability if the values are too large. Hourglassing that occurs with the default hourglass control parameters is usually an indication that the mesh is too coarse. Therefore, it is generally better to refine the mesh than to add stronger hourglass control.
This option is used to
choose a nondefault hourglass control approach for reduced-integration elements in Abaqus/Standard and Abaqus/Explicit and modified tetrahedral or triangular elements in Abaqus/Standard,
scale the default coefficients used in the hourglass control, and
activate distortion control for solid elements.
select a nondefault kinematic formulation for 8-node brick elements,
choose the second-order accurate formulation for solids and shells,
scale the drill stiffness of shell elements,
turn off the drill stiffness in small-strain shell elements S3RS and S4RS,
introduce the stresses in membrane elements from the initial configuration gradually into the model,
scale the linear and quadratic bulk viscosities,
specify the size of the particle tracking box for discrete element method (DEM) analyses and smoothed particle hydrodynamic (SPH) analyses,
specify additional control parameters for SPH analyses,
specify whether elements must be deleted when they are completely damaged, and
specify a value of the scalar degradation parameter at or above which elements are assumed to be completely damaged.
specify whether elements must be deleted when they are completely damaged,
specify a value of the scalar degradation parameter at or above which elements are assumed to be completely damaged, and,
in Abaqus/Standard, specify the viscosity coefficient that controls the viscous regularization.
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
Type: Model data
Level: Model
Abaqus/CAE: Mesh module
Set this parameter equal to a label that will be used to refer to the section control definition. All section control names in the same input file must be unique.
This parameter applies only to Abaqus/Explicit analyses involving the conversion of continuum elements to SPH particles and is valid only when ELEMENT CONVERSION=YES.
Set CONVERSION CRITERION=TIME (default) to specify the time when continuum elements are to convert to SPH particles.
Set CONVERSION CRITERION=STRAIN to specify the maximum principal strain (absolute value) when continuum elements are to convert to SPH particles.
Set CONVERSION CRITERION=STRESS to specify the maximum principal stress (absolute value) when continuum elements are to convert to SPH particles.
Set CONVERSION CRITERION=USER to specify a used-defined criterion when continuum elements are to convert to SPH particles.
This parameter applies to Abaqus/Explicit analyses and to solid sections in Abaqus/Standard analyses containing C3D10HS elements.
Set DISTORTION CONTROL=YES to activate a constraint that acts to prevent negative element volumes or other excessive distortion for crushable materials. This is the default value for elements with hyperelastic or hyperfoam materials. The DISTORTION CONTROL parameter is not relevant for linear kinematics and cannot prevent elements from being distorted due to temporal instabilities, hourglass instabilities, or physically unrealistic deformation.
Set DISTORTION CONTROL=NO to deactivate a constraint that acts to prevent negative element volumes or other excessive distortion for crushable materials. This value is the default except for elements with hyperelastic or hyperfoam materials.
This parameter applies only to the small-strain shell elements S3RS and S4RS.
Set DRILL STIFFNESS=ON (default) to activate the constraint against the drill mode in S3RS and S4RS elements.
Set DRILL STIFFNESS=OFF to deactivate the constraint against the drill mode. Deactivating the drill constraint can result in large values for the rotation degrees of freedom at the nodes of these elements.
The drill constraint is always active for finite-strain conventional shell elements such as S4R.
This parameter applies only to Abaqus/Explicit analyses involving the conversion of continuum elements to SPH particles.
Set ELEMENT CONVERSION=NO (default) to prevent continuum elements from converting to SPH particles.
Set ELEMENT CONVERSION=YES to allow continuum elements to convert to SPH particles.
Set ELEMENT CONVERSION=BACKGROUND GRID to allow continuum elements to convert to SPH particles that are uniformly distributed in an equally spaced background grid.
This parameter applies to all elements with progressive damage behavior, except connector elements in Abaqus/Explicit.
Set ELEMENT DELETION=YES to allow element deletion when the element has completely damaged. This value is the default for all elements with a damage evolution model. However, this value is not applicable to pore pressure cohesive elements.
Set ELEMENT DELETION=NO to allow fully damaged elements to remain in the computations. The element retains a residual stiffness given by the specified value of MAX DEGRADATION. In addition, elements with three-dimensional stress states (including generalized plane strain elements) can sustain hydrostatic compressive stresses, and elements with one-dimensional stress states can sustain compressive stresses. This value is the default for pore pressure cohesive elements and is not available for beam elements.
Set HOURGLASS=COMBINED to define the viscous-stiffness form of hourglass control for solid and membrane elements with reduced integration in Abaqus/Explicit.
Set HOURGLASS=ENHANCED (default for elements with hyperelastic and hyperfoam materials in Abaqus/Standard and Abaqus/Explicit; default in Abaqus/Standard and only option in Abaqus/Explicit for modified tetrahedral or triangular elements) to define hourglass control that is based on the assumed enhanced strain method for solid, membrane, finite-strain shell elements with reduced integration and modified tetrahedral or triangular elements in Abaqus/Standard and Abaqus/Explicit. Any data given on the data line will be ignored for this case.
Set HOURGLASS=RELAX STIFFNESS (default for Abaqus/Explicit, except for elements with hyperelastic and hyperfoam materials) to use the integral viscoelastic form of hourglass control for all elements with reduced integration in Abaqus/Explicit. This value is not supported for Eulerian EC3D8R elements.
Set HOURGLASS=STIFFNESS (default for Abaqus/Standard, except for elements with hyperelastic and hyperfoam materials and modified tetrahedral or triangular elements) to define hourglass control that is strictly elastic for all elements with reduced integration in Abaqus/Standard and Abaqus/Explicit and modified tetrahedral or triangular elements in Abaqus/Standard.
Set HOURGLASS=VISCOUS (default for Eulerian EC3D8R elements) to define the hourglass damping used to control the hourglass modes for solid and membrane elements with reduced integration in Abaqus/Explicit.
This parameter applies only to Abaqus/Standard analyses using pore pressure cohesive elements.
Set this parameter equal to the value of the initial gap opening used in the tangential flow continuity equation for pore pressure cohesive elements. The default value is 0.002.
This parameter applies only to Abaqus/Explicit analyses involving smoothed particle hydrodynamics (SPH).
Set KERNEL=CUBIC (default) to use a cubic spline interpolator for the SPH formalism.
Set KERNEL=QUADRATIC to use a quadratic interpolator for the SPH formalism.
Set KERNEL=QUINTIC to use a quintic interpolator for the SPH formalism.
Include this parameter to change the kinematic formulation for 8-node brick elements only.
Set KINEMATIC SPLIT=AVERAGE STRAIN (default in Abaqus/Explicit) to use the uniform strain formulation and the hourglass shape vectors in the hourglass control. This is the only option available for Abaqus/Standard.
Set KINEMATIC SPLIT=CENTROID to use the centroid strain formulation and the hourglass base vectors in the hourglass control in Abaqus/Explicit.
Set KINEMATIC SPLIT=ORTHOGONAL to use the centroid strain formulation and the hourglass shape vectors in the hourglass control in Abaqus/Explicit.
If SECOND ORDER ACCURACY=YES, the KINEMATIC SPLIT parameter will be reset to AVERAGE STRAIN in Abaqus/Explicit.
This parameter applies only to Abaqus/Explicit analyses and is valid only when the DISTORTION CONTROL parameter is used.
Set this parameter equal to 
(
) to define the length ratio when using distortion control for crushable materials. The default value is 
.
This parameter applies to all elements with progressive damage behavior, except connector elements in Abaqus/Explicit.
Set this parameter equal to the value of the damage variable at or above which a material point will be assumed to be completely damaged. This parameter also determines the amount of residual stiffness that will be retained by elements for which the ELEMENT DELETION parameter is set to NO. For elements other than cohesive elements, connector elements, and elements with plane stress formulations the default value is 1.0 if the element is deleted from the mesh and 0.99 otherwise. For cohesive elements, connector elements, and elements with plane stress formulations the default value is always 1.0.
This parameter applies only to Abaqus/Explicit analyses and is valid only when ELEMENT CONVERSION=BACKGROUND GRID.
Set PARTICLE THICKNESS=VARIABLE (default) to define the nonuniform thickness of the particles.
Set PARTICLE THICKNESS=UNIFORM to define the uniform thickness of the particles.
This parameter applies only to Abaqus/Standard analyses.
Set this parameter equal to a small perturbation to be applied to the second orientation for the FLEXION-TORSION connectors.
This parameter applies to membrane elements in Abaqus/Explicit analyses.
Set this parameter equal to the name of a total time-based amplitude defined to go from an initial value of zero to a final value of one. When this parameter is specified, the element stiffness is controlled until the amplitude value reaches its final value of one, so that the initial stresses are introduced gradually and not abruptly.
This parameter applies only to Abaqus/Explicit analyses; the element formulation is always second-order accurate in Abaqus/Standard.
Set SECOND ORDER ACCURACY=YES to use a second-order accurate formulation for solid or shell elements suitable for problems undergoing a large number of revolutions (> 5).
Set SECOND ORDER ACCURACY=NO (default) to use the first-order accurate solid or shell elements.
The SECOND ORDER ACCURACY parameter is not relevant for linear kinematics.
This parameter applies only to Abaqus/Explicit analyses involving smoothed particle hydrodynamics (SPH).
Set SPH FORMULATION=CLASSICAL (default) to use the classical SPH method.
Set SPH FORMULATION=NSPH to use the normalized SPH method.
Set SPH FORMULATION=XSPH to use the XSPH method.
This parameter applies only to Abaqus/Explicit analyses involving smoothed particle hydrodynamics (SPH).
Set SPH SMOOTHING LENGTH=CONSTANT (default) to use the constant smoothing length.
Set SPH SMOOTHING LENGTH=VARIABLE to use the variable smoothing length.
This parameter applies to cohesive elements, connector elements, and elements with plane stress formulations (plane stress, shell, continuum shell, and membrane elements) in Abaqus/Standard analyses.
Set this parameter equal to the value of the viscosity coefficient used in the viscous regularization scheme for cohesive elements or connector elements or equal to the value of the damping coefficient used in connector failure modeling. When this parameter is used to specify the viscosity coefficients for the damage model for fiber-reinforced materials, the specified value is applied to all the damage modes. The default value is 0.0.
This parameter applies only to Abaqus/Explicit analyses.
Set this parameter equal to 
(
) to scale the contributions from the constant hourglass stiffness term and the hourglass damping term to the hourglass control formulation. Setting 
or 
corresponds to pure constant stiffness hourglass control and pure damping hourglass control, respectively. The default is 
. This option is used only for solid and membrane elements when the HOURGLASS parameter is set equal to COMBINED.
First line:
Scaling factor, 
, for the hourglass stiffness, for use with displacement degrees of freedom. If this value is left blank, Abaqus will use the default value of 1.0. The suggested range for the value of is between 0.2 and 3.0.
Scaling factor, 
, for the hourglass stiffness, for use with rotational degrees of freedom in shell elements. If this value is left blank, Abaqus will use the default value of 1.0. The suggested range for the value of is between 0.2 and 3.0.
Scaling factor, 
, for the hourglass stiffness for use with the out-of-plane displacement degree of freedom in small-strain shell elements in Abaqus/Explicit. If this value is left blank, Abaqus/Explicit will use the default value of 1.0. The suggested range for the value of is between 0.2 and 3.0. This scaling factor is not relevant for Abaqus/Standard.
Scaling factor for the linear bulk viscosity in Abaqus/Explicit. If this value is left blank, Abaqus/Explicit will use the default value of 1.0. The suggested range for the value is between 0.0 and 1.0. This scaling factor is not relevant for Abaqus/Standard.
Scaling factor for the quadratic bulk viscosity in Abaqus/Explicit. If this value is left blank, Abaqus/Explicit will use the default value of 1.0. The suggested range for the value is between 0.0 and 1.0. This scaling factor is not relevant for Abaqus/Standard.
Scaling factor, 
, for the hourglass stiffness for use with pressure Lagrange multiplier degrees of freedom for element type C3D4H in Abaqus/Standard. If this value is left blank, Abaqus/Standard will use the default value of 1.0. The suggested range for the value of is between 0.2 and 3.0. This scaling factor is not relevant for Abaqus/Explicit.
Not used.
Scaling factor for the drill stiffness of shell elements in Abaqus/Explicit. This scaling factor is not relevant for Abaqus/Standard.
Second line (optional, to be used only in conjunction with smoothed particle hydrodynamics):
User-specified smoothing length.
User-specified smoothing length factor to scale the smoothing length.
Minimum number of particles within the sphere of influence for a given particle (default is 5).
Not used.
Mean velocity filtering coefficient for modified coordinate updates for particles used in the XSPH method. If this value is left blank, Abaqus/Explicit uses the default value of 0.5. The suggested range for the value is between 0.0 and 1.0.
Third line (optional, to be used only in conjunction with smoothed particle hydrodynamics and the discrete element method to control the size of the particle tracking box):
X-coordinate of the lower box corner.
Y-coordinate of the lower box corner.
Z-coordinate of the lower box corner.
X-coordinate of the opposite box corner.
Y-coordinate of the opposite box corner.
Z-coordinate of the opposite box corner.
Enter a value of 1 (default) to track all of the particles as the analysis progresses. Enter a value of 0 to define a particle tracking box using the coordinates given on this data line. This data item is ignored for discrete element method analyses.
Fourth line (optional, to be used only in conjunction with the conversion of continuum elements to smoothed particle hydrodynamic particles for ELEMENT CONVERSION=YES):
Number of particles to be generated per isoparametric direction.
Threshold value for the conversion criterion.
Fourth line (optional, to be used only in conjunction with the conversion of continuum elements to smoothed particle hydrodynamic particles for ELEMENT CONVERSION=BACKGROUND GRID):
Spacing of the background grid.
Name of an orientation definition (“Orientations,” Section 2.2.5 of the Abaqus Analysis User's Guide) to be used to define a local coordinate system for the background grid.