MultiPhysicsVault/.raw/AbaqusAnalysisUserGuide5/AbaqusAnalysisUserGuide5_068.md

<!-- source-page: 671 -->

# Tracking thickness when VUINTER or VUINTERACTION is used

Computations to determine the precise distance to a master surface are avoided if a slave node can be easily determined to be separated from the master surface, accounting for all thickness effects and built-in contact property models, by more than a threshold distance called the tracking thickness. Abaqus/Explicit uses an internal default value for the tracking thickness. If a built-in contact property model is in effect, the tracking thickness is quite small to help reduce computation time. However, if user subroutine VUINTER or user subroutine VUINTERACTION is in effect, the default tracking thickness is infinite so that all slave nodes are supplied to the user subroutines as having potential interactions. Alternatively, you can specify the tracking thickness in conjunction with a user-defined surface interaction model. In this case slave nodes whose proximity to their master surfaces are within this thickness are available for user-defined interactions. Use of a user-specified tracking thickness is supported only with node-tosurface contact and not with edge-to-edge contact.

Input File Usage: \*SURFACE INTERACTION, USER=INTERACTION, TRACKING THICKNESS=tracking\_thickness

# Interfacial state

Constitutive models used to define the interfacial behavior may require the storage of solution-dependent state variables. You must allocate storage space for these variables by indicating the number of variables. There is no restriction on the number of state variables associated with a user-defined constitutive behavior for the interface.

User subroutine UINTER is called for points on the slave surface at each iteration of every increment. User subroutine VUINTER is called in every time increment for each master-slave view of each contact pair it affects, as discussed earlier. User subroutine VUINTERACTION is called in every time increment for each pair of surfaces actively interacting, as discussed earlier. Each subroutine is provided with the state of the slave node or potential contact point at the start of the increment (the state includes stress, flux, solution-dependent state variables, temperature, and any predefined field variables) and with the increments in temperature, predefined state variables, relative position, and time.

Input File Usage: Use the following option to allocate storage space for solution-dependent state variables:

\*SURFACE INTERACTION, DEPVAR=number\_of\_state\_variables

# Use with the unsymmetric equation solver in Abaqus/Standard

If the constitutive Jacobian matrix, $\partial \triangle \pmb { \sigma } / \partial \triangle \mathbf { u }$ , is not symmetric, you should invoke the unsymmetric equation solution capability in Abaqus/Standard (see “Defining an analysis,” Section 6.1.2).

Input File Usage: \*SURFACE INTERACTION, USER, UNSYMM

<!-- source-page: 672 -->

In addition to defining the constitutive behavior, in Abaqus/Standard you may also update the flags LOPENCLOSE, LSTATE, and LSDI. The flag LOPENCLOSE is useful when UINTER is used to model standard contact between two surfaces (similar to the default hard contact in Abaqus). It should be set to 0 to indicate an open status and to 1 to indicate a closed status. At the beginning of the analysis it is set to −1 before UINTER is called. A change in this flag from one iteration to the next will have two consequences. It will result in output related to the change in contact status if detailed contact output has been requested to the message file (see “The Abaqus/Standard message file” in “Output,” Section 4.1.1), and it will also trigger a severe discontinuity iteration. The flag LSTATE can be used to store the current contact status of the points on the slave surface in non-standard situations where a simple open/close status is not appropriate. An example of such a situation is debonding, where three different states can be defined—fully bonded, partially bonded or debonding, and fully debonded. You can assign an integer to each of these states and set LSTATE accordingly. At the beginning of the analysis LSTATE is set to −1 before UINTER is called. When this flag is used and it changes from one iteration to the next, you can output messages to the message file (unit 7) related to such a change in state directly from user subroutine UINTER. The flag LPRINT is provided to allow you to output messages related to change in contact status only when you request detailed contact output to the message file. In such a situation the LSDI flag may be set to 1 to trigger a severe discontinuity iteration (this issue is discussed in detail later).

An example of a situation where both the flags LOPENCLOSE and LSTATE can be used arises in the modeling of debonding between two surfaces. When the surface is in a state of transition from bonded to debonded, the flag LSTATE may be used, while the flag LOPENCLOSE may be left to its original value of −1. However, once complete debonding has taken place, the contact between the two surfaces may be modeled using standard hard contact. In that situation the LSTATE flag may be set to −1, and the LOPENCLOSE flag used. Any time one of these two flags is set to −1, Abaqus/Standard assumes that it is not being used. A change of these flags from some other value to −1 does not result in contact-status related output or severe discontinuity iterations. Similarly, a change of these flags from −1 to some other value will not result in contact-status related output or severe discontinuity iterations.

If these flags are not used, there will be no output related to change in contact status unless you decide to output messages that are not based on these flags directly from UINTER.

# Severe discontinuity iterations in Abaqus/Standard

Abaqus/Standard classifies iterations in which the contact state at the end of the iteration is different from the state assumed for that iteration as severe discontinuity iterations. The treatment of severe discontinuity iterations by Abaqus/Standard is discussed in “Severe discontinuities in Abaqus/Standard” in “Defining an analysis,” Section 6.1.2. When you define the interfacial constitutive behavior through user subroutine UINTER and do not use the LOPENCLOSE flag, it is your responsibility to provide Abaqus/Standard with input on how an iteration should be treated. The flag LSDI is provided in user subroutine UINTER for this purpose. It is set to 0 before each call to UINTER; you should set it to 1 to treat the current iteration as a severe discontinuity iteration. If the LOPENCLOSE flag is used, the value

<!-- source-page: 673 -->

of this flag alone determines whether a severe discontinuity iteration is necessary or not, and the LSDI flag is ignored.

# Use with contact in Abaqus/Explicit

The penalty contact algorithm must be used with user subroutines VUINTER and VUINTERACTION; see “Penalty contact algorithm” in “Contact constraint enforcement methods in Abaqus/Explicit,” Section 38.2.3.

When VUINTER is used and balanced master-slave contact is specified (i.e., the contact pair weighting factor is not equal to 0.0 or 1.0), VUINTER will be called for each surface in the contact pair that can act as a slave surface. The forces and fluxes defined in VUINTER will be multiplied by the weight value for the master-slave view before they are applied.

# Effects on solution time in Abaqus/Explicit

Abaqus/Explicit accounts for the contact stiffness and conductance in the stable time increment calculation. Specifying stresses and fluxes in the user subroutine that correspond to large contact stiffness (e.g., large slope of contact pressure versus penetration) and large contact conductance will cause a significant drop in the stable time increment and, therefore, an increase in the solution time. Tangent stiffnesses and conductances are determined by Abaqus/Explicit using a finite difference method. User subroutine VUINTER is called three times per increment for each master-slave view of each two-dimensional contact pair that references it and four times per increment for each three-dimensional contact pair that references it. User subroutine VUINTERACTION is called four times per increment for each active surface interaction that references it. The user subroutines are called once with the actual configuration and subsequently with perturbed configurations based on displacement perturbations in the normal direction, the $\mathbf { t } _ { 1 }$ tangential direction, and, in three-dimensional cases, the $\mathbf { t } _ { 2 }$ tangential direction, respectively (see the local coordinate system discussion in “VUINTER,” Section 1.2.20 of the Abaqus User Subroutines Reference Guide, and “VUINTERACTION,” Section 1.2.21 of the Abaqus User Subroutines Reference Guide, for an explanation of how the $\mathbf { t } _ { 1 }$ and $\mathbf { t } _ { 2 }$ directions are defined). For example, each component of contact stiffness is computed as a difference in contact stress divided by a difference in relative position. You do not have access to the computed values of contact stiffness and conductance, but you can control the constitutive behavior of the model. Estimated default penalty stiffness (and conductance) values are provided to the user subroutines for comparison purposes. Contact stiffnesses or conductances that exceed the default penalty values can significantly reduce the time increment size. The default penalty stiffnesses and conductances are based on an assumption that all slave nodes are in contact. In the case of VUINTER, if only a fraction of the slave nodes are in contact, higher penalties than are reported in VUINTER would be assigned in some cases with the default penalty algorithm.

Any changes to state variables are ignored for the perturbation calls.

In the case of VUINTER there can be significant additional CPU expense associated with contact tracking. Since the contact state is unknown on entry to VUINTER, all nodes on the slave surface must be tracked in every increment. This can increase the cost of an analysis significantly compared to the contact models in Abaqus/Explicit if a large proportion of the slave nodes are not involved in contact.

<!-- source-page: 674 -->

In the case of VUINTERACTION there can be significant additional CPU expense associated with contact tracking only if the tracking thickness is large compared to the element facet size on contacting surfaces.

# Use with other subroutines

Any other user subroutine that does not deal with constitutive behavior across an interface can be used in conjunction with UINTER, VUINTER, or VUINTERACTION.

For example, user subroutines UMAT and UMATHT can be used in conjunction with UINTER to define the constitutive mechanical and thermal behaviors of the material underlying the contact surfaces. User subroutine VUMAT can be used in conjunction with VUINTER to define the mechanical constitutive behavior of the material underlying the contact surfaces. However, user subroutines FRIC, GAPCON, and GAPELECTR—available in Abaqus/Standard for defining mechanical, thermal, and electrical interactions between surfaces—can be used in conjunction with UINTER only if they are referenced on separate surface interactions. The same restriction applies to user subroutine VFRIC used in conjunction with VUINTER and to user subroutines VFRICTION or VFRIC\_COEF used in conjunction with VUINTERACTION.

# Use with contact controls

In Abaqus/Standard contact controls will not have any effect when used at an interface whose constitutive behavior is defined through user subroutine UINTER.

In Abaqus/Explicit contact controls can be specified for a contact pair referencing a user-defined surface interaction. In the case of user subroutine VUINTERACTION the default penalty stiffness argument includes any scale factor specified; whereas with user subroutine VUINTER the scale factor is ignored.

# Output

Most of the standard output variables that are normally available in an analysis involving contact are available with this capability.

# Output for UINTER

The variables COPEN and CSLIP represent the relative positions normal and tangential to the interface, respectively. The surface-based thermal interaction variable, SFDR, contains the heat flux due to the total energy dissipated due to friction, and not some fraction of it. This is unlike using the built-in capability in Abaqus/Standard, where SFDR may contain the heat flux due to only a fraction of the total frictional dissipation, depending on the specified fraction of the dissipated energy that is converted into heat. In addition, the surface-based thermal interaction variable WEIGHT, which represents the weighting factor for heat flux (generated by frictional sliding) distribution between the surfaces, is not available with this capability.

Additional user-defined output variables can be defined for UINTER by using the solutiondependent state variables (SDV).

<!-- source-page: 675 -->

# Output for VUINTER and VUINTERACTION

All contact output variables in Abaqus/Explicit will be available except output for spot welds (BONDSTAT and BONDLOAD).

The following user subroutine variables will contribute to the associated total energy variables: the variable sed will contribute to the energy output variable ALLSE; sfd will contribute to ALLFD; scd will contribute to ALLCD; spd will contribute to ALLPD; and svd will contribute to ALLVD.

If SFDR is requested, sfd, scd, spd, and svd will also be used to calculate the heat generated at the interface (for output purposes only; the generated heat will not be applied to the model). The default values of the fraction of mechanical energy converted into heat and the weighting factor for the distribution of heat between the two surfaces (1.0 and 0.5, respectively) are used.

User-defined, solution-dependent state variables associated with the user subroutine cannot be output to the output database (.odb) file or results (.fil) file.

<!-- source-page: 676 -->

<!-- source-page: 677 -->

# 37.1.7 PRESSURE PENETRATION LOADING

Products: Abaqus/Standard Abaqus/CAE

# References

• \*PRESSURE PENETRATION   
• \*SURFACE   
• \*CONTACT PAIR   
• “Defining pressure penetration,” Section 15.13.16 of the Abaqus/CAE User’s Guide, in the HTML version of this guide

# Overview

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.

# 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 “Contact interaction analysis: overview,” Section 36.1.1). The surfaces are modeled as slave and master contact surfaces (see “Contact formulations in Abaqus/Standard,” Section 38.1.1).

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,” Section 6.4.1 of the Abaqus Theory Guide, 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,

<!-- source-page: 678 -->

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 analysis.

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,” Section 2.3.4), 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

<!-- source-page: 679 -->

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,” Section 6.1.2).

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 “Applying loads: overview,” Section 34.4.1).

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

<!-- source-page: 680 -->

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 analysis

Linear perturbation analyses can be performed from time to time during a fully nonlinear analysis by including linear perturbation steps between the general analysis steps. Because contact conditions cannot change during a linear perturbation analysis, the fluid will not penetrate further into the surface and it remains as it was defined in 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,” Section 10.3.1) and steady-state dynamic analyses (direct or modal—see “Direct-solution steady-state dynamic analysis,” Section 6.3.4, and “Mode-based steady-state dynamic analysis,” Section 6.3.8) you can specify both the real (in-phase) and imaginary (out-of-phase) parts of the loading.

<table><tr><td>Input File Usage:</td><td>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, IMAGINARYThe REAL or IMAGINARY parameters are ignored in all procedures other than steady-state dynamics.</td></tr><tr><td>Abaqus/CAE Usage:</td><td>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)</td></tr></table>

# 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