A pressure penetration interaction allows you to simulate the pressure of a fluid penetrating between two surfaces involved in surface-to-surface contact. The fluid pressure is applied normal to the surfaces. The bodies forming the joint can both be deformable, as is the case with threaded connectors; or one can be rigid, as occurs when a soft gasket is used as a seal between stiffer structures.
Pressure penetration interactions can be applied in three-dimensional, planar (two-dimensional), or axisymmetric models. A pressure penetration interaction can be used only in an Abaqus/Standard analysis.
Before defining the pressure penetration interaction, you must create a surface-to-surface contact interaction to specify the master and slave surfaces for the pressure penetration; see “Defining surface-to-surface contact in an Abaqus/Standard analysis” in “Defining surface-to-surface contact,” Section 15.13.7. When you create the surface-to-surface contact interaction, any combination of Sliding formulation and Discretization method can be used (for compatibility with pressure penetration).
In the pressure penetration definition you identify the contact surfaces, the regions on the surfaces exposed to the fluid pressure, the magnitude of the fluid pressure, and the critical contact pressure acting on the regions. In a three-dimensional model points, edges, and faces can be selected as the regions exposed to the fluid pressure. In a two-dimensional model only points can be selected. In a two-dimensional model you must identify the penetration points on both the master and slave surfaces (unless the master surface is an analytical rigid surface).
The fluid can penetrate from either one or multiple regions on the surface. These regions are always subjected to the pressure penetration, regardless of their contact status. Fluid will penetrate into the region between the contacting bodies until a point is reached where the contact pressure is greater than the specified critical value, cutting off further penetration of the fluid.
For more information about pressure penetration, see “Pressure penetration loading,” Section 37.1.7 of the Abaqus Analysis User's Guide.
To define pressure penetration:
From the main menu bar, select Interaction
Create.
Tip:
You can also create a pressure penetration interaction using the 
tool in the Interaction module toolbox.
In the Create Interaction dialog box that appears, do the following:
Name the interaction. For more information about naming objects, see “Using basic dialog box components,” Section 3.2.1.
Select the step in which the interaction will be created.
Select the Pressure penetration type of interaction.
Click Continue to close the Create Interaction dialog box.
From the Contact interaction list, select the surface-to-surface contact interaction to which the pressure penetration will be applied.
The master and slave surfaces of the contact interaction are shown in the dialog box, and the surfaces are highlighted in the viewport.
For a three-dimensional model, do the following in the Penetration Regions table:
Identify the first region on the slave surface that is exposed to the fluid pressure.
Double-click the empty cell in the Region on Slave column, or select the cell and click the 
button; then use one of the following methods to select the region:
Use the mouse to select a face, edge, or point on the model in the viewport. If you are working in a mesh, you can use the mouse to select nodes.
Choose an existing set to specify the face, edge, or point. On the right side of the prompt area, click Sets. Select an existing face, edge, or vertex from the Region Selection dialog box that appears, and click Continue.
Note: The default selection method is based on the selection method you most recently employed. To revert to the other method, click Select in Viewport or Sets on the right side of the prompt area.
It is not necessary to identify the Region on Master for a three-dimensional model. However, doing so may help you resolve any problems that you encounter with the analysis. You can select the Region on Master in exactly the same way as the Region on Slave.
Note: If the selected contact interaction has an analytical rigid master surface, the Region on Master column appears dimmed, indicating that adding or editing master surface points is unavailable. Any master surface regions that have already been specified will be ignored.
Enter the Critical Contact Pressure below which fluid will start to penetrate. The higher this value, the easier the fluid penetrates. The default is zero, in which case the fluid penetrates only if contact is lost. For more information, see “Specifying a critical mechanical contact pressure” in “Pressure penetration loading,” Section 37.1.7 of the Abaqus Analysis User's Guide.
Enter the magnitude of the reference Fluid Pressure. For more information, see “Specifying the applied fluid pressure” in “Pressure penetration loading,” Section 37.1.7 of the Abaqus Analysis User's Guide.
If the analysis step is a steady-state dynamic (linear perturbation) step, you can specify both the real (in-phase) and imaginary (out-of-phase) parts of the pressure in the Fluid Pressure (Real) and Fluid Pressure (Imaginary) columns of the table. See “Use in linear perturbation analysis” in “Pressure penetration loading,” Section 37.1.7 of the Abaqus Analysis User's Guide, for more details.
To add a row to the table and to continue selecting additional penetration regions, click the 
button. This action takes you directly to the region picking step in the viewport. Repeat as needed to specify all the regions.
To edit a penetration region, select the region in the table, click the button, and reselect the region.
To delete a region, select the row in the table and click the 
button.
For a planar (two-dimensional) or axisymmetric model, do the following in the Penetration Regions table:
Identify the first pair of points exposed to the fluid pressure.
Double-click the empty cell in the Region on Master column, or select the cell and click the button; then use one of the following methods to select the point:
Use the mouse to select the point on the model in the viewport.
Choose an existing set to specify the point. On the right side of the prompt area, click Sets. Select an existing node or vertex from the Region Selection dialog box that appears, and click Continue.
Note: The default selection method is based on the selection method you most recently employed. To revert to the other method, click Select in Viewport or Sets on the right side of the prompt area.
Repeat the process to select the corresponding penetration point on the slave surface, using the Region on Slave column of the table.
Note: If the selected contact interaction has an analytical rigid master surface, the Region on Master column appears dimmed, indicating that adding or editing master surface points is unavailable. Any master surface points that have already been specified will be ignored.
Enter the Critical Contact Pressure below which fluid will start to penetrate. The higher this value, the easier the fluid penetrates. The default is zero, in which case the fluid penetrates only if contact is lost. For more information, see “Specifying a critical mechanical contact pressure” in “Pressure penetration loading,” Section 37.1.7 of the Abaqus Analysis User's Guide.
Enter the magnitude of the reference Fluid Pressure. For more information, see “Specifying the applied fluid pressure” in “Pressure penetration loading,” Section 37.1.7 of the Abaqus Analysis User's Guide.
If the analysis step is a steady-state dynamic (linear perturbation) step, you can specify both the real (in-phase) and imaginary (out-of-phase) parts of the pressure in the Fluid Pressure (Real) and Fluid Pressure (Imaginary) columns of the table. See “Use in linear perturbation analysis” in “Pressure penetration loading,” Section 37.1.7 of the Abaqus Analysis User's Guide, for more details.
To add a row to the table and to continue selecting penetration points, click the button. This action takes you directly to the point picking step in the viewport. Repeat as needed to specify all the points.
To edit a penetration point, select the point in the table, click the button, and reselect the point.
To delete a pair of penetration points, select the row in the table and click the button.
In the Penetration time field, enter the time period for the fluid pressure penetration to reach the full current magnitude on newly penetrated surface segments. The default penetration time is 0.001 of the current step time. The penetration time is not available in a linear perturbation analysis. See “Specifying a penetration time for the fluid pressure” in “Pressure penetration loading,” Section 37.1.7 of the Abaqus Analysis User's Guide, for more details.
Optionally, you can define the variation of the fluid pressure during the step by selecting an amplitude curve in the Amplitude list. By default, the reference magnitude is applied immediately at the beginning of the step or ramped up linearly over the step, depending on the amplitude variation assigned to the step. Fluid pressure amplitude curves are not available for some steps. See “Specifying the applied fluid pressure” in “Pressure penetration loading,” Section 37.1.7 of the Abaqus Analysis User's Guide, for more details.
Click OK to create the interaction and to close the editor.
