Fluid Pressure Penetration Loads

Simulating Effects of Fluid Pressure Acting on Surfaces that Consider Contact Conditions

You can model the effects of fluid pressure acting on surfaces without directly modeling the fluid volume. The extent of a surface exposed to fluid pressure can evolve as contact conditions change. Consider the example shown in Figure 1 and Figure 2. A key purpose of the simulation might be to determine if the seal is able to contain the pressurized fluid.

In this type of simulation, one or more initial steps are conducted without the effects of a fluid pressure load to compress the seal. Fluid pressure loading is introduced in a subsequent step. At the beginning of this step, a surface pressure load of magnitude $p_{f}$ acts on surface regions exposed to the fluid on the left side of Figure 1, where the contact pressure is below a specified threshold value, $σ_{c p r e s s}^{c r i t}$ . The surface pressure load might cause the contact pressure to drop below $σ_{c p r e s s}^{c r i t}$ over a greater area, leading to more of the surface being exposed to the fluid as shown in Figure 2. Various design factors influence whether fluid penetration continues until failure of the seal in these types of studies.

Abaqus provides two methods for fluid pressure penetration loading that evolves based on contact conditions:

Distributed surface pressure penetration loading used in conjunction with general contact and available in both Abaqus/Standard and Abaqus/Explicit.
Surface pairwise pressure penetration loading used in conjunction with contact pairs and available only in Abaqus/Standard.

These two methods overlap in functionality and control. Similarities include the ability to control the region initially exposed to the fluid pressure, the magnitude of the fluid pressure, and the critical contact pressure below which fluid penetration starts to occur.

Distinctions between the methods include the approach to defining the contact and loading. Usage details are discussed in Surface Fluid Pressure Penetration Loading with General Contact and Pairwise Fluid Pressure Penetration Loading with Contact Pairs in Abaqus/Standard.

Results for axisymmetric O-ring seal simulations are shown in Figure 3 and Figure 4. For additional discussion, see Fluid pressure penetration analysis of an O-ring seal of a pipe connection. The O-ring is compressed into a cavity between analytical rigid surfaces prior to the introduction of fluid pressure penetration loading. The axisymmetric model of the seal is swept circumferentially to facilitate visualization of results Figure 3 and Figure 4, although the two analytical surfaces are not swept. These simulations consider effects of fluid entering the top, left corner of the cavity to determine if the seal design successfully contains the fluid. Figure 3 shows contour plots of fluid pressure loading (PPRESS) in the top left corner of the cavity very early in the process of applying fluid pressure penetration loading for three simulation variants modeling the same physics:

An Abaqus/Standard simulation with the distributed surface pressure penetration loading capability in conjunction with general contact.
An Abaqus/Explicit simulation with the distributed surface pressure penetration loading capability in conjunction with general contact.
An Abaqus/Standard simulation with the surface pairwise pressure penetration loading capability in conjunction with contact pairs.

For this example, the two Abaqus/Standard simulations use the implicit dynamics procedure, and the Abaqus/Explicit simulation uses the explicit dynamics procedure. Contour plots of PPRESS in Figure 4 show the final extent of the region exposed to fluid pressure for these simulations. All three simulations predict similar distances of fluid penetration into the contact interface.

Input File Usage

A potential keyword interface for distributed surface pressure penetration loading in conjunction with general contact for the example shown in Figure 1 and Figure 2 is:

**Contact specification
CONTACT
CONTACT INCLUSIONS, ALL EXTERIOR
…
**Fluid pressure penetration load specification
DSLOAD
seal_leftside, PPEN, 1.E5, 1.E4, LOCAL
upperpart_leftside, PPEN, 1.E5, 1.E4, LOCAL
lowerpart_leftside, PPEN, 1.E5, 1.E4, LOCAL

A potential keyword interface for pairwise pressure penetration loading associated with contact pairs (contact) for the same example is:

**Contact specification
CONTACT PAIR
seal_top, upper_part
seal_bot, lower_part
…
**Fluid pressure penetration load specification
PRESSURE PENETRATION, SECONDARY=seal_top, MAIN=upper_part
nsetsectop_init, nsetmaintop_init, 1.E5, 1.E4
PRESSURE PENETRATION, SECONDARY=seal_bot, MAIN=lower_part
nsetsecbot_init, nsetmainbot_init, 1.E5, 1.E4

Surface Fluid Pressure Penetration Loading with General Contact

Distributed surface fluid pressure penetration loading simulates the effects of fluid pressure acting on surfaces without directly modeling the fluid. Aspects influencing this loading are discussed in Magnitude and Time Dependence of the Fluid Pressure and Initialization and Evolution of the Region Exposed to Fluid Pressure.

You specify the surface potentially exposed to fluid pressure loading, the magnitude of the fluid pressure, the critical contact pressure below which fluid penetration starts to occur, the name of the algorithm associated with evolution of the region exposed to fluid pressure, the nodes initially exposed to the fluid, and the penetration time. All surface faces potentially exposed to fluid pressure loading with this capability must be included in the general contact domain (see Defining the General Contact Domain in Abaqus/Standard and Defining the General Contact Domain in Abaqus/Explicit.

Input File Usage

DSLOAD, AMPLITUDE=name, OP=MOD (default) or NEW
surface, PPEN, fluid pressure magnitude, critical contact pressure, LOCAL or WETTING ADVANCE,
node or node set, penetration time, amplitude curve related to critical contact pressure

Abaqus/CAE Usage

Load module: Create Load: choose Mechanical for the Category and Fluid pressure penetration for the Types for Selected Step

Magnitude and Time Dependence of the Fluid Pressure

You define the reference magnitude of the fluid pressure; and, optionally, you define the variation of the fluid pressure during a step by referring to an amplitude curve. Surface-based fluid pressure penetration loading is defined in a similar method to other types of distributed surface loads, including for a surface pressure acting over a nonvarying region of a surface (see Distributed Loads). For information about specifying the reference magnitude of the fluid pressure, see Specifying Pressure Loads. For information about specifying the time dependence of the fluid pressure, see Defining Time-Dependent Distributed Loads and About Prescribed Conditions. At each new step, you can modify or completely redefine the fluid pressure penetration loading similar to the way that distributed loads are defined (see About Loads).

Initialization and Evolution of the Region Exposed to Fluid Pressure

Abaqus provides the following algorithms associated with the initialization and evolution of the region exposed to fluid pressure:

Local algorithm

A surface face is “wetted” (exposed to fluid pressure) while a measure of the local contact pressure associated with the face, $σ_{l o c a l}^{c p r e s s}$ , is less than or equal to a critical contact pressure, $σ_{c r i t}^{c p r e s s}$ , and, if cohesive behavior is locally defined, the cohesive damage measure, $d_{c s d m g}$ , is greater than 0.95. A newly wetted surface face need not be adjacent to an already wetted surface face with this algorithm.
A surface face is “unwetted” (not exposed to fluid pressure) while the measure of the local contact pressure associated with the face, $σ_{l o c a l}^{c p r e s s}$ , is greater than a critical contact pressure, $σ_{c r i t}^{c p r e s s}$ , or, if cohesive behavior is locally defined, the cohesive damage measure, $d_{c s d m g}$ , is less than or equal to 0.95.
These criteria are applicable when the fluid pressure penetration load is first introduced and thereafter. You do not specify a node or node set initially exposed to fluid pressure in this case.
There are no limits to the number of changes in wetting status for a face with this algorithm. For example, a surface face might be initially unwetted, then become wetted, and still later become unwetted again.
This algorithm is available in Abaqus/Standard and Abaqus/Explicit.

Wetting advance algorithm

Wetting is irreversible with this algorithm. Once a surface face becomes wetted, it remains wetted as long as pressure penetration loading is in effect.
You must specify either a single node or a node set consisting of nodes that are initially exposed to fluid pressure. These nodes are not required to be adjacent. If all nodes of a surface face are included in this node set, the face is initially wetted.
Abaqus determines an initial wetted front, consisting of all nodes in the user-specified node or node set, except those nodes whose adjacent faces are all initially wetted. Abaqus updates the set of wetted-front nodes in subsequent increments as additional faces become wetted.
An initially unwetted face becomes wetted when any of its adjacent nodes are along the wetted front and a measure of the local contact pressure associated with the face, $σ_{l o c a l}^{c p r e s s},$ is less than or equal to a critical contact pressure, $σ_{c r i t}^{c p r e s s}$ , and, if cohesive behavior is locally defined, the cohesive damage measure, $d_{c s d m g},$ is greater than 0.95. The wetted front can advance by one face per increment in Abaqus/Explicit with this algorithm.
This algorithm is available only in Abaqus/Explicit.

Figure 5 shows contour plots of the PPRESS output variable for two Abaqus/Explicit simulations with fluid pressure penetration loading for a simple example consisting of a small block sliding along a larger block. Only two contour levels are shown in the plot: the color red indicates fluid pressure exposure, while the color blue indicates no exposure to the fluid pressure. Nodes of the bottom block at the boundary of the red and blue contour regions near the top block have significant contact forces (and contact pressure) before sliding and are at the "wetted front" before sliding. Faces exposed to fluid pressure contribute fluid pressure forces to adjacent nodes; therefore, nodes on a wetted front receive some force due to fluid pressure. The top block is omitted from some plots in Figure 5 to observe the fluid pressure exposure on the top surface of the bottom block. In this example the top side of the bottom block and all sides except the top of the top block are potentially exposed to fluid pressure. The four vertical sides of the top block are exposed to fluid pressure throughout the simulation for both types of wetting algorithms. Differences between the local and wetting advance algorithms are especially apparent on the top side of the bottom block. With the wetting advance algorithm, once a face becomes wetted it remains wetted regardless of subsequent contact conditions. However, with the local algorithm, the wetted region corresponds to the region currently without significant contact pressure.

A critical contact pressure, $σ_{c p r e s s}^{c r i t}$ , applies to both algorithms. $σ_{c p r e s s}^{c r i t}$ is zero by default, but it might be appropriate to specify a positive critical contact pressure to account for a tendency for fluid pressure to creep into an interface under low contact pressure due to surface roughness effects. Increasing the value of $σ_{c p r e s s}^{c r i t}$ tends to increase the surface area exposed to fluid pressure.

The treatment of any overlapping fluid pressure penetration loadings depends on the types of wetting algorithms involved:

Overlapping fluid pressure penetration loadings involving a mixture of the local and wetting advance algorithms: This is not allowed and triggers an error message.
Overlapping fluid pressure penetration loadings involving the local algorithm: If a face satisfies the wetting criteria for multiple loadings, the greatest fluid pressure among those loadings is applied, with consideration of current values for time varying fluid pressures.
Overlapping fluid pressure penetration loadings involving the wetting advance algorithm: Abaqus monitors nodal “fronts” with adjacent faces exposed to different fluid pressure penetration loadings. These fronts can change by one face per increment in Abaqus/Explicit, such that the surface region exposed to the greatest fluid pressure expands.

Magnitude and Time Dependence of the Critical Contact Pressure Threshold

You define the reference magnitude of the critical contact pressure threshold and can optionally define the variation of the critical contact pressure threshold during a step by referring to an amplitude curve. For more information about specifying the critical contact pressure threshold reference magnitude and the name of the amplitude curve, see *DSLOAD).

Specifying a Penetration Time for the Fluid Pressure in Abaqus/Standard

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 is 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.

Limitations with Surface-based Fluid Pressure Penetration Loads

Fluid pressure penetration loading must be used with a single-sided element-based surface.

It is often good practice, but not required, to define fluid pressure penetration loading on both surfaces of an interface. The loads are applied independently of each other because the loading is surface-based and not pairwise, and the wetted front locations are also determined independently. Thus, the fluid pressure loading can be influenced by how well the mesh densities are matched between the two surfaces along the interface because the wetted front regions along each surface might not match exactly.

While pressure penetration loading acts on a single-sided surface of a shell, the contact pressure field used to compare with the critical contact pressure does not distinguish between contact on either side of the shell. As such, fluid evolution might be inhibited due to contact on the shell side in which the fluid pressure penetration load is not potentially applied.

The fluid pressure penetration load applied at any increment is based on the contact status at the beginning of that increment. Therefore, in Abaqus/Standard, you should 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. This behavior should have minimal effect with Abaqus/Explicit.

In large-displacement Abaqus/Standard analyses, pressure penetration loads introduce unsymmetric load stiffness matrix terms. Using the unsymmetric matrix storage and solution scheme for the analysis step might improve the convergence rate of the equilibrium iterations. For more information on the unsymmetric matrix storage and solution scheme, see Defining an Analysis.

The contact pressure field from contact pairs does not have any influence on the evolution of the fluid.

Fluid pressure penetration loading is not available within the following Abaqus/Standard procedures: frequency, complex frequency, buckling, RIKS, substructure generation, and beam section generation. For general procedure types, this loading is not available for steady state transport. However, fluid pressure penetration loads from prior steps can be propagated from the base state of these steps if the steps are linear or remain fixed in the case of a steady state transport step. Fluid pressure penetration loads are not available when you specify a cyclic symmetry mode number because this type of loading does not guarantee cyclic symmetry.

Only solid, shell, axisymmetric, cylindrical, and rigid elements are supported for fluid pressure penetration.

Pairwise Fluid Pressure Penetration Loading with Contact Pairs in Abaqus/Standard

Pairwise fluid pressure penetration loading with contact pairs in Abaqus/Standard is an alternative to surface fluid pressure penetration loading with general contact (see About Contact Pairs in Abaqus/Standard). Similarities and differences between these two methods are discussed in Simulating Effects of Fluid Pressure Acting on Surfaces that Consider Contact Conditions.

A pairwise fluid pressure penetration loading specification must refer to surfaces of a contact pair. These surface might both be deformable, as is the case with threaded connectors; or one body might be rigid, as occurs when a soft gasket is used as a seal between stiffer structures. Any contact formulation can be used. Other aspects influencing pairwise fluid pressure penetration loading are discussed in Magnitude and Time Dependence of the Fluid Pressure and Initialization and Evolution of the Region Exposed to Fluid Pressure.

You specify the main and secondary surfaces of the contact pair, nodes exposed to the fluid pressure, the magnitude of the fluid pressure, the critical contact pressure below which fluid penetration starts to occur, and the penetration time.

Input File Usage

PRESSURE PENETRATION, SECONDARY=secondary1, MAIN=main1, PENETRATION TIME
secondary surface node or node set, main 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 main and secondary surfaces
Create Interaction: Pressure penetration; Contact interaction: contact_interaction_name, Region on Main: select face, edge, or point, Region on Secondary: select face, edge, or point, Critical Contact Pressure: critical contact pressure, Fluid Pressure: magnitude

Magnitude and Time Dependence of the 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 pairwise fluid pressure penetration load is applied to the element surface based on the pressure penetration criterion at the beginning of an increment and remains 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 is 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 pairwise fluid pressure penetration loads are applied to the element surfaces, they are not 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 secondary nodes exposed to the fluid pressure must be specified on the data lines. If the main surface is not an analytical rigid surface, the main 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 respecify a previously defined pressure penetration load, the fluid pressure loading reverts 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

Initialization and Evolution of the Region Exposed to Fluid Pressure

The algorithm associated with initialization and evolution of the region exposed to the fluid pressure for pairwise fluid pressure penetration loading with contact pairs in Abaqus/Standard is similar to the WETTING ADVANCE algorithm of surface fluid pressure penetration loading with general contact in that the wetting is irreversible and the wetting region incrementally grows along a wetted front.

The fluid can penetrate from either one or multiple locations of the surface. You must identify a node or node set on the secondary surface of the contacting bodies that defines where the surface is exposed to the fluid pressure. In two dimensions if the main surface is not an analytical rigid surface (see Analytical Rigid Surface Definition), you must also identify a node or node set on the main surface that defines where the surface is exposed to fluid pressure. These nodes or node sets are always subjected to the pairwise fluid pressure penetration load if they are on the secondary surface, regardless of their contact status. The wetted surface region expands as fluid effectively penetrates into the interface of the contacting bodies from these nodes or nodes sets until a point is reached where the contact pressure is greater than the specified critical value, $σ_{c p r e s s}^{c r i t}$ , cutting off further penetration of the fluid.

$σ_{c p r e s s}^{c r i t}$ is zero by default, but it might be appropriate to specify a positive critical contact pressure to account for a tendency for fluid pressure to creep into an interface under low contact pressure due to surface roughness effects. Increasing the value of $σ_{c p r e s s}^{c r i t}$ tends to increase surface areas exposed to fluid pressure.

Figure 6 shows results for two Abaqus/Standard simulations with fluid pressure penetration loading for a small block sliding along a larger block. Figure 5 shows Abaqus/Explicit results for the same example with the LOCAL and WETTING ADVANCE algorithms using general contact. The color red indicates fluid pressure exposure, while the color blue indicates no exposure to the fluid pressure. With pairwise pressure penetration loading, output indicating fluid pressure exposure is available only on the secondary surface. All sides except the top of the smaller, top block and just the top side of the larger, bottom block are potentially exposed to fluid pressure. The four vertical sides of the top block are exposed to fluid pressure throughout the simulation for both pairwise fluid pressure penetration loading and surface-based fluid pressure penetration loading.

Results on the top surface of the bottom block:

are similar for the pairwise method in Abaqus/Standard (see middle row of plots in Figure 6) and the surface-based method with the WETTING ADVANCE algorithm in Abaqus/Explicit (see bottom row of plots in Figure 5); although, for example, the region under fluid pressure extends into the active contact region due to the ramp-down characteristic described in Fluid Pressure Ramp Versus Sharp Cutoff at the Wetted Front; and
are similar for the LOCAL algorithm in Abaqus/Standard (see bottom row of plots in Figure 6) and Abaqus/Explicit (see middle row of plots in Figure 5).
the wetted front in Abaqus/Standard is at a location between elements (Figure 6) compared to nodal locations in Abaqus/Explicit (Figure 5).

Fluid Pressure Ramp Versus Sharp Cutoff at the Wetted Front

In three dimensions the surfaces of the elements at the front of the penetrated nodes can have only ramped-down pressure loadings. In two dimensions the surfaces of the elements at the front of the penetrated nodes can have either zero or ramped-down pressure loadings.

Input File Usage

Use the following option to apply zero pressure loading to the unwetted surface at the front of the penetration node:

PRESSURE PENETRATION, WETTED FRONT=NODE (default)

Use the following option to apply ramped down pressure loading to the unwetted surface at the front of the penetration node:

PRESSURE PENETRATION, WETTED FRONT=MID ELEMENT

Abaqus/CAE Usage

Specifying pressure loading on the front unwetted elements is not supported in Abaqus/CAE.

Specifying a Penetration Time for the Fluid Pressure

When the pairwise 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 pairwise 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 is 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

Limitations with Pairwise Fluid Pressure Penetration Loads

Each secondary 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 secondary 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 are 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 might 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.

Behavior in Linear Perturbation Steps

Perturbation analyses can be performed 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 penetrates no 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 as a Linear Analysis Step) 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 surface-based fluid pressure penetration loading:

DSLOAD, REAL (default)

Use the following option to define the imaginary (out-of-phase) part of the surface-based fluid pressure penetration loading:

DSLOAD, IMAGINARY

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

PRESSURE PENETRATION, REAL (default)

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

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

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

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

Output

You can request output of the currently active pressure (PPRESS) and force (PFORCE) associated with nodes of a wetted region due to fluid pressure penetration loading as surface output to the data, results, and output database files (see Surface Output from Abaqus/Standard and Writing Surface Output to the Output Database). With pairwise fluid pressure loading, you can define this output on nodes along the secondary surface.

You can also request the total force (PFN) associated with a whole surface due to fluid pressure penetration loading.