Mit der Funktion aus meiner ersten Antwort kannst du Elementen schon eine bestimmte Spannung zum Anfang der Analyse geben. Das möchtest du doch machen, oder?
Inwiefern kommst du damit nicht klar? Weißt du nicht wie du dir aus den Manuals die nötigen Informationen besorgst oder sind es andere Probleme?
Hier die wichtigen Abschnitte:
Users Manual 27.2.1:
Defining initial stresses
You can define an initial stress field. Initial stresses can be defined directly or, in ABAQUS/Standard, by user subroutine SIGINI. Stress values given directly will be applied uniformly over the element unless they are defined at each section point through the thickness in shell elements.
If a local coordinate system was defined (see “Orientations,” Section 2.2.5), stresses must be given in the local system.
In soils (porous medium) problems the initial effective stress should be given; see “Coupled pore fluid diffusion and stress analysis,” Section 6.7.1, for a discussion of defining initial conditions in porous media.
If the section properties of beam elements or shell elements are defined by a general section, the initial stress values are applied as initial section forces and moments. In the case of beams initial conditions can be specified only for the axial force, the bending moments, and the twisting moment. In the case of shells initial conditions can be specified only for the membrane forces, the bending moments, and the twisting moment. In both shells and beams initial conditions cannot be prescribed for the transverse shear forces.
Initial stress fields cannot be defined for spring elements. See “Springs,” Section 26.1.1, for a discussion of defining initial forces in spring elements.
Establishing equilibrium in ABAQUS/Standard
When initial stresses are given in ABAQUS/Standard (including prestressing in reinforced concrete or interpolation of an old solution onto a new mesh), the initial stress state may not be an exact equilibrium state for the finite element model. Therefore, an initial step should be included to allow ABAQUS/Standard to check for equilibrium and iterate, if necessary, to achieve equilibrium.
In a soils analysis (that is, for models containing elements that include pore fluid pressure as a variable) the geostatic stress field procedure (“Geostatic stress state,” Section 6.7.2) should be used for the equilibrating step. Any initial loading (such as geostatic gravity loads) that contributes to the initial equilibrium should be included in this step definition. The initial time increment and the total time specified in this step should be the same. The initial stresses are applied in full at time zero; and if equilibrium can be achieved, this step will converge in one increment. Therefore, there is no benefit to incrementing.
To achieve equilibrium for all other analyses, a first step using the static procedure (“Static stress analysis,” Section 6.2.2) should be used. It is recommended that you specify the initial time increment to be equal to the total time specified in this step so that ABAQUS/Standard will attempt to find equilibrium in one increment. By default, ABAQUS/Standard ramps down the unbalanced stress over the first step. This allows ABAQUS/Standard to use automatic incrementation if equilibrium cannot be found in one increment. This ramping is achieved in the following manner:
An additional set of artificial stresses is defined at each material point. These stresses are equal in magnitude to the initial stresses but are of opposite sign. The sum of the material point stresses and these artificial stresses creates zero internal forces at the beginning of the step.
The internal artificial stresses are ramped off linearly in time during the first step. Thus, at the end of the step the artificial stresses have been removed completely and the remaining stresses in the material will be the stress state in equilibrium.
You can force ABAQUS/Standard to achieve equilibrium in one increment by using a step variation on the initial condition to resolve the unbalanced stress instead of ramping the stress down over the entire step. If ABAQUS/Standard cannot achieve equilibrium in one increment, the analysis will terminate.
If the equilibrating step does not converge, it indicates that the initial stress state is so far from equilibrium with the applied loads that significantly large deformations would be generated. This is generally not the intention of an initial stress state; therefore, it suggests that you should recheck the specified initial stresses and loads.
Input File Usage: Use one of the following options to specify how the unbalanced stress should be resolved:
*INITIAL CONDITIONS, TYPE=STRESS,
UNBALANCED STRESS=RAMP (default)
*INITIAL CONDITIONS, TYPE=STRESS,
Keyword Reference Manual zu *Initial Conditions:
Data lines for TYPE=STRESS if the GEOSTATIC, REBAR, SECTION POINTS, and USER parameters are omitted:
Element number or element set label.
Value of first (effective) stress component, axial force when used with the *BEAM GENERAL SECTION or *FRAME SECTION options, or direct membrane force per unit width in the local 1-direction when used with the *SHELL GENERAL SECTION option.
Value of second stress component.
Etc., up to six stress components.
Give the stress components as defined for this element type in Part VI, “Elements,” of the ABAQUS Analysis User's Manual. Stress values given on data lines are applied uniformly and equally over all integration points of the element. In any element for which an *ORIENTATION option applies, the stresses must be given in the local system (“Orientations,” Section 2.2.5 of the ABAQUS Analysis User's Manual).
Repeat this data line as often as necessary to define initial stresses in various elements or element sets.
Beispiel: Die Elemente in den Element-Sets "prestress_100" und "prestress_200" sollen jeweils Anfangspannungen von 100 und 200 (Einheit je nach Eiheitensystem) in den 3 Hauptrichtungen bekommen.
*Initial Conditions, Type=Stress
prestress_100, 100, 100, 100
prestress_200, 200, 200, 200
Eine Antwort auf diesen Beitrag verfassen (mit Zitat/Zitat des Beitrags) IP