Pressure penetration loading

Pressure penetration loads simulated with contact pairs:

model the penetration of fluid between two contacting structures; and
allow the fluid to penetrate from multiple locations on the surface.

The following topics are discussed:

Defining pressure penetration loads between contacting bodies
Output

Defining pressure penetration loads between contacting bodies

Distributed pressure penetration loads allow for the simulation of fluid penetrating into the surface between two contacting bodies and application of the fluid pressure normal to the surfaces. Element-based contact surfaces are used to model the interactions between the bodies (see About contact interactions). The surfaces are modeled as slave and master contact surfaces (see Contact formulations in Abaqus/Standard).

Any contact formulation can be used.

The bodies forming the joint may both be deformable, as would be the case with threaded connectors; or one may be rigid, as would occur when a soft gasket is used as a seal between stiffer structures. You specify the nodes exposed to the fluid pressure, the magnitude of the fluid pressure, and the critical contact pressure below which fluid penetration starts to occur. See Pressure penetration loading with surface-based contact for more details.

Input File Usage

PRESSURE PENETRATION, SLAVE=slave1, MASTER=master1
slave surface node or node set, master surface node or node set, magnitude, critical contact pressure

If a node set is specified, it can contain only one node in two dimensions; in three dimensions it can contain any number of nodes.

Abaqus/CAE Usage

Interaction module:
Create Interaction: Surface-to-surface contact (Standard), Name: contact_interaction_name; select master and slave surfaces
Create Interaction: Pressure penetration; Contact interaction: contact_interaction_name, Region on Master: select face, edge, or point, Region on Slave: select face, edge, or point, Critical Contact Pressure: critical contact pressure, Fluid Pressure: magnitude

Specifying a pressure penetration criterion

A single slave-node-based penetration criterion is used. Fluid will penetrate into the surface between the contacting bodies from one or multiple locations, which are exposed to the fluid, until a point is reached where the contact pressure is greater than the specified critical value, cutting off further penetration of the fluid.

Specifying a penetration time for the fluid pressure

When the fluid pressure penetration criterion is satisfied, the fluid pressure is applied normal to the surfaces. If the full current fluid pressure is applied immediately, the resulting large changes in the strains near the contact surfaces can cause convergence difficulties. For large-strain problems severe mesh distortion can also occur. To ensure a smooth solution, the fluid pressure is ramped up linearly over a time period from zero pressure penetration load to the full current magnitude.

You can specify the time period taken for the fluid pressure penetration load to reach the full current magnitude on newly penetrated surface segments. If the accumulated increment size, measured immediately after the penetration, is greater than the penetration time, the full current fluid pressure penetration load will be applied; otherwise, the fluid pressure on the newly penetrated surface segments is ramped up linearly to the current magnitude over the penetration time period, possibly over a number of increments. When the penetration time is equal to 0, the current fluid pressure is applied immediately once the fluid pressure penetration criterion is satisfied. The default penetration time is chosen to be 0.001 of the total step time. The penetration time is ignored in a linear perturbation step.

Input File Usage

PRESSURE PENETRATION, PENETRATION TIME=n

Abaqus/CAE Usage

Interaction module: Create Interaction: Pressure penetration; Penetration time: n

Specifying the nodes exposed to the fluid pressure

The fluid can penetrate from either one or multiple locations of the surface. You must identify a node or node set on the slave surface of the contacting bodies that defines where the surface is exposed to the fluid pressure. In two dimensions if the master surface is not an analytical rigid surface (see Analytical rigid surface definition), you must also identify a node or node set on the master surface that defines where the surface is exposed to the fluid pressure. You can specify multiple nodes or node sets if multiple locations of the surface are exposed to the fluid. These nodes or node sets are always subjected to the pressure penetration load if they are on the slave surface, regardless of their contact status. The fluid then starts to penetrate into the surface between the two contacting bodies from these nodes or node sets.

Specifying the applied fluid pressure

You must define the reference magnitude of the fluid pressure. You can define the variation of the fluid pressure during a step by referring to an amplitude curve. 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 (see Defining an analysis).

The fluid pressure penetration load will be applied to the element surface based on the pressure penetration criterion at the beginning of an increment and will remain constant over that increment even if the fluid penetrates further during that increment. A nodal integration scheme is used to integrate the distributed fluid pressure penetration load over an element in two dimensions, while in three dimensions Gauss integration scheme is used; the variation of the distributed fluid pressure over an element will be determined by the load magnitudes at the element's nodes.

Input File Usage

Use the following option to define the variation of the fluid pressure during a step:

PRESSURE PENETRATION, AMPLITUDE=name

Abaqus/CAE Usage

Interaction module: Create Interaction: Pressure penetration; Amplitude: name

Removing or modifying the pressure penetration loads

After pressure penetration loads are applied to the element surfaces, they will not be removed automatically even when contact between the surfaces is reestablished. At each new step the fluid pressure penetration loading, however, can be modified or completely redefined in a manner similar to the way that distributed loads can be defined (see About loads).

Input File Usage

Use the following option to modify the fluid pressure penetration loads that were applied in previous steps:

PRESSURE PENETRATION, OP=MOD (default)

In this case the slave nodes exposed to the fluid pressure must be specified on the data lines. If the master surface is not an analytical rigid surface, the master nodes exposed to the fluid pressure must also be specified on the data lines for planar or axisymmetric models.

Use the following option to remove all fluid pressure penetration loads and, optionally, to specify new fluid pressure penetration loads:

PRESSURE PENETRATION, OP=NEW

When OP=NEW is used to remove all fluid pressure penetration loads, no data line is needed. However, when OP=NEW is used to specify new fluid pressure penetration loads, the nodes exposed to the fluid pressure must be specified on the data lines. OP=NEW must be used when defining new exposed nodes. In addition, when OP=NEW is used to re-specify a previously defined pressure penetration load, the fluid pressure loading will revert to its last known configuration first, even if the contact status has subsequently changed.

Abaqus/CAE Usage

Use the following option to modify a fluid pressure penetration that was applied in a previous step:

Interaction module: Interaction Manager: select interaction, Edit

Use the following option to remove a fluid pressure penetration that was applied in a previous step:

Interaction module: Interaction Manager: select interaction, Deactivate

Specifying a critical mechanical contact pressure

To account for the asperities on the contacting surfaces, a critical contact pressure, below which fluid penetration starts to occur, is introduced. The higher this value, the easier the fluid penetrates. The default value of the critical contact pressure is zero, in which case fluid penetration occurs only if contact is lost.

Use in linear perturbation steps

Perturbation analyses can be performed from time to time during a fully nonlinear analysis by including linear perturbation steps between the general analysis steps. With the exception of the static LCP perturbation procedure, contact conditions are not allowed to change during a linear perturbation step; the fluid will not penetrate further into the surface and remains as it was defined in the base state. Even in the case of a static LCP perturbation procedure, where the contact status at the end of the perturbation analysis can be different from the base state, the portions of the contact surfaces where the fluid pressure acts remain frozen at the base state. The fluid pressure magnitude applied in the previous general analysis step, however, can be modified during a linear perturbation analysis step. In matrix generation (see Generating matrices) and steady-state dynamic analyses (direct or modal—see Direct-solution steady-state dynamic analysis and Mode-based steady-state dynamic analysis) you can specify both the real (in-phase) and imaginary (out-of-phase) parts of the loading.

Input File Usage

Use the following option to define the real (in-phase) part of the loading:

PRESSURE PENETRATION, REAL (default)

Use the following option to define the imaginary (out-of-phase) part of the loading:

PRESSURE PENETRATION, IMAGINARY

The REAL or IMAGINARY parameters are ignored in all procedures other than steady-state dynamics.

Abaqus/CAE Usage

Use the following option to define the real (in-phase) part of the loading:

Interaction module: Create Interaction: Pressure penetration; Fluid Pressure (Real)

Use the following option to define the imaginary (out-of-phase) part of the loading:

Interaction module: Create Interaction: Pressure penetration; Fluid Pressure (Imaginary)

Limitations with pressure penetration loads

Each slave surface subjected to pressure penetration loading must be continuous and cannot be a closed loop. Pressure penetration loading cannot be used with a node-based slave surface. The pressure penetration load applied at any increment is based on the contact status at the beginning of that increment. You should, therefore, be careful in interpreting the results at the end of an increment during which the contact status has changed. Small time increments are recommended to obtain accurate results.

When pressure penetrates into contacting bodies between an analytical rigid surface and a deformable surface, no pressure penetration load will be applied to the analytical rigid surface. The reference node on the analytical rigid surface should, therefore, be constrained in all directions. To account for the effect of fluid pressure penetration loads on the rigid surface, the analytical rigid surface should be replaced with an element-based rigid surface.

When fluid with different pressure loads penetrates into an element simultaneously from multiple locations on a surface, the maximum value of the fluid pressure loads is applied to the element.

In large-displacement analyses pressure penetration loads introduce unsymmetric load stiffness matrix terms. Using the unsymmetric matrix storage and solution scheme for the analysis step may improve the convergence rate of the equilibrium iterations. See Defining an analysis for more information on the unsymmetric matrix storage and solution scheme.

Only solid, shell, cylindrical, and rigid elements are supported for three-dimensional pressure penetration.

Output

You can request the fluid pressure load, PPRESS, at the nodes on the slave surface as surface output to the data, results, and output database files (see Surface output from Abaqus/Standard and Surface output in Abaqus/Standard and Abaqus/Explicit).