Defining a pore pressure field in a porous medium

For Abaqus/Standard analyses you can define the initial pore pressure field, uw, for nodes in a coupled pore fluid diffusion/stress analysis (see Coupled pore fluid diffusion and stress analysis). The initial pore pressure can be defined directly as an elevation-dependent function, by interpolation from the output database file of a previous Abaqus analysis, or by user subroutine UPOREP. You can create or modify a pore pressure field only during the initial step. For more information, see Initial conditions in Abaqus/Standard and Abaqus/Explicit.

Related Topics
Understanding symbols that represent prescribed conditions
Creating predefined fields
Using analytical expression fields
Creating expression fields
In Other Guides
Coupled pore fluid diffusion and stress analysis

  1. Display the pore pressure field editor using one of the following methods:

    • To create a new pore pressure field, follow the procedure outlined in Creating predefined fields (Category: Other; Types for Selected Step: Pore pressure). You can create a pore pressure field only during the initial step.

    • To edit an existing pore pressure field using menus or managers, see Editing step-dependent objects. You can modify a pore pressure field only during the initial step.

  2. Click the arrow to the right of the Point 1 distribution field, and select the option of your choice from the list that appears:

    • Select Uniform to define a pore pressure that is uniform for the selected region.

    • Select From output database file to read pore pressure values from the output database file of a previous Abaqus analysis with pore pressure components.

    • Select User-defined to specify pore pressure output using options in user subroutine UPOREP. See the following sections for more information:

    • Select an analytical field to define a spatially varying initial pore pressure. Alternatively, you can click to create a new analytical field. (See The Analytical Field toolset,” for more information.)

  3. For uniform distributions, do the following:

    1. From the Elevation distribution options, select either Linear or Constant.
    2. In the Pore pressure 1 field, specify the initial pore pressure in the first region in your model.
    3. If you selected an elevation distribution that varies linearly, specify the following options:

      • In the Vertical coordinate 1 field, specify the vertical position of the first location in your model for which you are specifying initial pore pressure.

      • In the Point 2 distribution field, specify either a Uniform distribution for pore pressure at the second elevation or select an analytical field to define a spatially varying initial pore pressure at the second elevation. If you select Uniform, specify the pore pressure and vertical position of the second location in your model.

  4. If you are specifying pore pressure output from an output database file, do the following:

    1. Specify the file name from which you want to import pore pressure values.
    2. From the Step options, either select Last to read pore pressure output from the last step of the output database or select Specify and enter the number of the step from which you want to read pore pressure data
    3. From the Increment options, either select Last to read pore pressure output from the last increment of the selected step or select Specify and enter the number of the increment from which you want to read pore pressure data.
    4. Toggle on Interpolate midside nodes to interpolate pore pressure values between dissimilar meshes.

  5. For user-defined pore pressure distributions, do the following:

    1. Enter the Job module, and display the job editor for the analysis job of interest. (For more information, see Creating, editing, and manipulating jobs.)
    2. In the job editor, click the General tab, and specify the file containing the user subroutine that defines the predefined field. For more information, see Specifying general job settings.

      Note:

      You can specify only one user subroutine file in the job editor; if your analysis involves more than one user subroutine, you must combine the user subroutines into one file and then specify that file.

  6. Click OK to create the pore pressure field and to close the dialog box.

    Magenta squares appear on the model representing the initial pore pressure field that you just created.