*GEOSTATIC

Obtain a geostatic stress field.

This option is used to verify that the geostatic stress field is in equilibrium with the applied loads and boundary conditions on the model and to iterate, if needed, to obtain equilibrium.

This page discusses:

See Also
In Other Guides
Geostatic Stress State

Products Abaqus/Standard Abaqus/CAE

Type History data

LevelStep

Abaqus/CAE Step module

Optional parameters

HEAT

This parameter is relevant if there are regions in the model that use coupled temperature–pore pressure elements; it specifies whether heat transfer effects are to be modeled in these regions.

Set HEAT=YES (default) to specify that heat transfer effects are to be modeled in these regions. In this case Abaqus/Standard solves the heat transfer equation in conjunction with the mechanical equilibrium and the fluid flow continuity equations.

Set HEAT=NO to specify that heat transfer will not be modeled in these regions.

This parameter is not relevant if only coupled pore pressure–displacement elements are used in a model.

SLURRY FLOW

Set SLURRY FLOW=YES (default) to activate the solution of the slurry continuity equation in a step. In this case, the slurry concentration field will evolve with time within the step.

Set SLURRY FLOW=NO to deactivate the solution of the slurry continuity equation in a step. In this case, the slurry concentration field will not evolve with time within the step.

This parameter is relevant only when the slurry concentration degree of freedom is active.

SLURRY MAX

Set this parameter equal to the maximum allowed value of the slurry concentration at a material point. The default is 0.67.

This parameter is relevant only when the slurry concentration degree of freedom is active.

SLURRY MIN

Set this parameter equal to the minimum allowed value of the slurry concentration at a material point. The default is zero.

This parameter is relevant only when the slurry concentration degree of freedom is active.

UTOL

This parameter will invoke automatic time incrementation.

Set this parameter equal to the tolerance for the maximum change of displacements. Abaqus/Standard will ensure that the maximum absolute value of a displacement at a node is smaller than the tolerance times the characteristic element length in the model. If this parameter is used without any value specified, the default value of 10−5 is used. If this parameter is omitted, no restrictions are imposed on the displacement values.

Data line to define automatic time incrementation

First (and only) line

  1. Initial time increment. This value will be modified as required. If this entry is zero or is not specified, a default value that is equal to the total time period of the step is assumed.

  2. Time period of the step. If this entry is zero or is not specified, a default value of 1.0 is assumed.

  3. Minimum time increment allowed. If Abaqus/Standard finds it needs a smaller time increment than this value, the analysis is terminated. If this entry is zero, a default value of the smaller of the suggested initial time increment or 10−5 times the total time period is assumed.

  4. Maximum time increment allowed. If this value is zero or is not specified, no upper limit is imposed.