整理学习subroutine VUSDFLD中的几个关键点

cys_2019

Field-Variable-Dependent Material Properties
1. Using tabular definition for built-in ABAQUS material models.
2. Using other user subroutines, such as CREEP, to define the material behavior as a function of fi (Most material properties in ABAQUS/Explicit can be defined as functions of field variables, fi).

Field Variable（fi）
1. Field variables (fi) are normally considered nodal data by ABAQUS.
2. The VUSDFLD routine is then written to define the values of fi on an integration point by integration point basis:
    1) The *USER DEFINED FIELD option is included in the material definition to indicate that the VUSDFLD subroutine will be called for those elements using that material definition.
    2) The fi can be defined as functions of solution data, such as stress or strain, available at the integration points (ABAQUS/Explicit allows the fi to be defined as functions of solution data, such as stress or strain, at the material points).
Before user subroutine VUSDFLD is called, the values of the field variables at the material point are calculated by interpolation from the values defined at the nodes. Any changes to the field variables in the user subroutine are local to the material point: the nodal field variables retain the values defined as initial conditions or predefined field variables or the values defined in user subroutine VUFIELD. The values of the field variables defined in this routine are used to calculate values of material properties that are defined to depend on field variables and are passed into other user subroutines that are called at the material point.
    3) ABAQUS/Explicit does not store the values of calculated in VUSDFLD. If you need access to previous values of fi, you must save them as solution-dependent variables (SDVs) inside VUSDFLD.
    4) Solution-dependent state variables (SDVs) must be used in VUSDFLD if fi have any history dependence.
    5) field(nblock,nfieldv): An array containing the field variables at the material points; stateNew(nblock,nstatev): An array containing the solution-dependent state variables at the material points.

Solution data
1. ABAQUS/Explicit allows the fi to be defined as functions of solution data, such as stress or strain, at the material points.
2. The values of the solution data provided are from the beginning of the current increment.
3. Subroutine VUSDFLD must use the ABAQUS utility routine VGETVRM to access this material point data (The variables provided to VGETVRM are the output variable key, VAR, for the desired solution data).

State Variable
1. Solution-dependent state variables (SDVs) must be used in VUSDFLD if have any history dependence (ABAQUS/Explicit does not store the values of calculated in VUSDFLD).
2. These are passed in as the values at the beginning of the increment.
    1) The SDVs updated in VUSDFLD are then passed into other user subroutines that can be called at this material point.
    2) The number of state variables associated with this material point is defined with the ∗DEPVAR option.

VUSDFLD
1. It allows the redefinition of field variables at a material point as functions of time or of any of the available material point quantities listed in “Available output variable keys” in “Obtaining material point information in an Abaqus/Explicit analysis,” Section 2.1.7;
2. It can be used to introduce solution-dependent material properties since such properties can be easily defined as functions of field variables;
3. It will be called at all material points of elements for which the material definition includes user-defined field variables;
4. It can call utility routine VGETVRM to access material point data; and
5. It can use and update solution-dependent state variables.

备注：
          1. 学习材料来自ABAQUS Documentation（http://ivt-abaqusdoc.ivt.ntnu.no ... sub-rtn-uexpusdfld;[/url]等）和编写用户子程序USDFLD的讲义（http://forum.simwe.com/forum.php ... 35&highlight=USDFLD）等；
          2. 分享此个人理解的几个关键点与大家，希望与大家一起进步，整理的过程中有不足或者不对的地方请大家批评指正补充；
          3. 如有需要增加的部分，后续将更新。