Pressure loads represent uniform scalar pressure fields applied to surface geometries. The force direction for a pressure load is always normal to the surface and remains normal even as the surface rotates, provided that geometric nonlinearity is considered in the step.
Pressure loads can be applied only in mechanical steps.
The magnitude of a pressure load can vary with time during a step according to an amplitude definition (see Amplitudes for more information on defining amplitudes).
You can prescribe the time variation of the magnitude of a pressure load in a user subroutine, which is sometimes preferable when the time history of the magnitude is complex. You can also apply knowledgeware techniques to control the value of a pressure load (for more information, see Applying Knowledgeware).
Pressure loads can be applied to surface or face supports or to a surface group. When you select the support, you can also select an existing pressure load that was created from a different analysis case that was created in the Generative Structural Analysis workbench. The new pressure load has the same magnitude and is applied to the same region as the pressure load created in the Generative Structural Analysis workbench. You can modify the magnitude or the region only by modifying the original pressure feature in the Generative Structural Analysis workbench. The original pressure feature in the Generative Structural Analysis workbench can include Data Mapping using values imported from a Microsoft Excel spreadsheet (.xls*) or a text file (.txt). The imported pressure data must satisfy the following criteria:
The data must be arranged in four columns in the following order: X-coordinate, Y-coordinate, Z-coordinate, and pressure value.
The data must include a header row in which the dimensional data are provided in parentheses. Pressure data can be provided without dimensions. The following sample header row provides one example of proper header row syntax:
X(mm) Y(mm) Z(mm) Pressure()
The actual pressure values created from imported data will be the product of the dimensionless pressure values multiplied by the value you provide for the Magnitude of the pressure. For example, if your imported data specify a dimensionless value of 10 at the location (0, 0, 0) and you specify a value of 20N_m2 for the pressure history object, the pressure at that location will be 200N/m2 for the analysis.
This task shows you how to create a pressure load on geometry.
Click the Pressure Load icon .
The Pressure dialog box appears, and a Pressure object appears in the specification tree under the Loads objects set for the current step.
You can change the identifier of the load by editing the Name field.
Select the geometry support (a surface or a pressure load that you created in the Generative Structural Analysis workbench). Any selectable geometry is highlighted when you pass the cursor over it. You can select several supports to apply the load to all supports simultaneously. You can also select a surface group.
The Supports field is updated to reflect your selection. A temporary symbol will appear at the supports to indicate zero values until you apply a nonzero load.
Enter a value for the pressure magnitude.
Right-click on the Magnitude field to add knowledgeware controls (for more information, see Applying Knowledgeware).
To import and incorporate a pressure history into the pressure load, perform the following steps:
Toggle on Data mapping, then click the ... button.
The Data Mapping dialog box appears.
Click Browse, then select the spreadsheet or text file from which you want to import temperature data.
Once you select a file, you can display the imported data in tabular form in the Imported Table dialog box by clicking Show.
If desired, toggle on Display Bounding Box to display a three-dimensional box incorporating the minimum and maximum values from the imported table. The bounding box enables you to confirm that the support you select lies completely within the space dictated by the imported data; if a portion of the support is outside this box, an error will be returned during the analysis.
Click OK to close the Data Mapping dialog box.
Click More to access additional pressure load options.
Toggle on Selected amplitude, and select an amplitude from the specification tree to define a nondefault time variation for the pressure load.
If you do not specify an amplitude in a Nonlinear Structural case, Abaqus applies the reference magnitude based on the Default load variation with time option that you selected when you created the step. Abaqus either applies the reference magnitude linearly over the step (Ramp) or applies it immediately at the beginning of the step and subsequently holds it constant (Instantaneous).
If you do not specify an amplitude in an Explicit Dynamics case, Abaqus applies the reference magnitude immediately at the beginning of the step and subsequently holds it constant (Instantaneous).
See About Prescribed Conditions in the Abaqus Prescribed Conditions Guide for more information.
Toggle on Apply user subroutine to define a nonuniform variation of the pressure load magnitude throughout the step in user subroutine DLOAD (in a Nonlinear Structural case) or VDLOAD (in an Explicit Dynamics case). For more information, see Using User Subroutines; DLOAD in the Abaqus User Subroutines Guide; and VDLOAD in the Abaqus User Subroutines Guide.
Click OK in the Pressure dialog box.
Symbols representing the applied pressure are displayed on the geometry.