Defining a pressure load

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

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

• To edit an existing 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.

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 pressure that is uniformly distributed over the surface. For this option, the magnitude you provide must be the force per unit area.

• Select Total Force to define a pressure that is uniformly distributed over the surface. For this option, the magnitude you provide must be the total magnitude of the force applied to the surface (instead of force per unit area).

• Select Hydrostatic to define a hydrostatic pressure applied to the surface. (This option is valid only for Abaqus/Standard analyses.)

• Select Stagnation to define a stagnation pressure applied to the surface. (This option is valid only for Abaqus/Explicit analyses.)

• Select Viscous to define a viscous pressure applied to the surface. (This option is valid only for Abaqus/Explicit analyses.)

• Select User-defined to define the magnitude of the load in user subroutine DLOAD (for Abaqus/Standard) or VDLOAD (for Abaqus/Explicit). See the following sections for more information:

  • Specifying general job settings

  • DLOAD

  • VDLOAD

• Select an analytical field, labeled with an (A), or a discrete field, labeled with a (D), to define a spatially varying pressure. Only analytical fields and discrete 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, Total Force, analytical field, or discrete field distribution option, perform the following steps:

1. In the Magnitude text field, enter the pressure magnitude.

   For a Uniform distribution, enter the total force magnitude divided by the surface area over which the force is applied (units FL⁻²).

   For a Total Force distribution, enter the total magnitude of the force (units F). Based on the undeformed model geometry, Abaqus/CAE calculates a constant uniform surface pressure from the force magnitude entered. In a large-displacement analysis, however, the actual total force may change during the analysis due to the deformation of the loaded surface.

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 (if you are working in three-dimensional or axisymmetric space) or the Y-coordinate (if you are working in two-dimensional space) of the height at which the pressure is zero.
3. In the Reference pressure height field, enter the Z-coordinate (if you are working in three-dimensional or axisymmetric space) or the Y-coordinate (if you are working in two-dimensional space) 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 Stagnation or Viscous 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. If desired, toggle on Determine velocity from reference point to subtract the velocity of a reference node from the velocity of the surface where the pressure is applied.
4. Click to select a reference point using one of the following methods:

   • Select a point from the viewport.

   • Click Points in the prompt area, and select a named set.

     Note:

     The set that you select must contain a single node or vertex.

5. Click OK to save your data and to exit the editor.

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 in an Abaqus/Standard analysis but are ignored in an Abaqus/Explicit analysis.
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 that defines the load magnitude. 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.