Defining a pipe pressure load

Display the pipe pressure load editor using one of the following methods:

• To create a new pipe pressure load, follow the procedure outlined in Creating loads (Category: Mechanical; Types for Selected Step: Pipe pressure).

• To edit an existing pipe pressure load using menus or managers, see Editing step-dependent objects. To edit the region to which the load is applied, see Editing the region to which a prescribed condition is applied.

Select the Side option of your choice:

• Select Internal to prescribe an internal pressure within the pipe.

• Select External to prescribe an external pressure on the pipe.

In the Effective diameter field, enter the appropriate pipe diameter:

• Enter the inner diameter of the pipe if you selected Internal in the previous step.

• Enter the outer diameter of the pipe if you selected External in the previous step.

Note:

The effective diameter that you enter remains constant throughout the analysis. It is not scaled as the pipe expands or contracts under the pressure, even when the Nlgeom setting is turned on. (For more information on the Nlgeom setting, see Accounting for geometric nonlinearity.)

Click the arrow to the right of the Distribution field, and select the option of your choice from the list that appears:

• Select Uniform to define a load that is uniform over the pipe surface.

• Select Hydrostatic to define a hydrostatic pressure on or within the pipe.

• Select User-defined to define the magnitude of the load in user subroutine DLOAD. See the following sections for more information:

  • Specifying general job settings

  • DLOAD

• Select an analytical field to define a spatially varying load. Only analytical fields that are valid for this load type are displayed in the selection list. Alternatively, you can click to create a new analytical field. (See The Analytical Field toolset,” for more information.)

If you selected the Uniform or analytical field distribution option, perform the following steps:

1. In the Magnitude text field, enter the pressure magnitude (units FL⁻²).
2. If desired, click the arrow to the right of the Amplitude field, and select the amplitude of your choice from the list that appears. Alternatively, you can click to create a new amplitude. (See The Amplitude toolset,” for more information.)
3. Click OK to save your data and to exit the editor.

If you selected the Hydrostatic distribution option, perform the following steps:

1. In the Magnitude text field, enter the pressure magnitude (units FL⁻²).
2. In the Zero pressure height field, enter the Z-coordinate of the height at which the pressure is zero.
3. In the Reference pressure height field, enter the Z-coordinate of the height at which the pressure is the magnitude specified in the Magnitude field.

   (For more information, see Hydrostatic pressure loads on two-dimensional, three-dimensional, and axisymmetric elements in Abaqus/Standard.)

4. If desired, click the arrow to the right of the Amplitude field, and select the amplitude of your choice from the list that appears. Alternatively, you can click to create a new amplitude. (See The Amplitude toolset,” for more information.)

If you selected the User-defined distribution option, perform the following steps:

1. If desired, enter the pressure magnitude in the Magnitude field (units FL⁻²). Magnitude data that you enter in the editor are passed into the user subroutine.
2. Click OK to save your data and to exit the editor.
3. Enter the Job module and display the job editor for the analysis job of interest. (For more information, see Creating, editing, and manipulating jobs.)
4. In the job editor, click the General tab, and specify the file containing the user subroutine DLOAD. 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.