usyd_abaqus_2006

ABAQUS: Selected Topics L7.9

Automatic Stabilization and Dashpots

– When damping is applied through the automatic stabilization procedure,
ABAQUS builds a volume proportional damping matrix:

C = cM1,

where

M1 = mass matrix with unit density and
c = damping factor.
– ABAQUS automatically determines the damping factor, c, based on the

following premises:
• The model’s response in the first increment of a step to which
stabilizing damping is applied is stable.
• Under stable circumstances the amount of dissipated energy should
be very small.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.10

Automatic Stabilization and Dashpots

– This is accomplished as follows:

• During the first increment of the step, calculations are made of the
strain and dissipation energies.

• These energies are extrapolated to the time scale of the step, as if the
solution were to be scaled linearly in time.

• The damping factor, c, is determined in such a way that if the solution

were linear, the viscous dissipation energy would be a small fraction of
the model’s strain energy at the end of the step.

• This small fraction, called the dissipation intensity, a, is controlled by

the user.

– It has a default value of 2 × 10−4.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.11

Automatic Stabilization and Dashpots

– Alternatively, the user may specify the damping factor directly.

– Since c is related to the model size and material stiffness in nonobvious

ways, it may be difficult to choose a proper value.
• Initiate a run without explicit declaration of a damping factor.
• ABAQUS prints out the value of the damping factor, which can then be
used as a guideline for selecting appropriate values.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.12

Automatic Stabilization and Dashpots

– There are cases where the first increment is either unstable or singular
(e.g., due to a rigid body mode).

• In such cases it is not possible to obtain a solution in the first
increment without damping.

• ABAQUS precomputes the damping factor based on a sampling of the
average element stiffness.

• If the calculated strain energy in the first increment indicates the
solution without damping is stable, the damping factor is recalculated
as described earlier; otherwise, the initially calculated factor is
maintained.

– Warning: The damping factor may be stronger than desired;
critically review the solution.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.13
L7.14
Automatic Stabilization and Dashpots

• ABAQUS usage: Automatic stabilization
– Automatic stabilization can be added in the
following quasi-static procedures in ABAQUS:

*STATIC
*VISCO
*COUPLED TEMPERATURE-DISPLACEMENT
*SOILS, CONSOLIDATION

– It is specified by including the STABILIZE
parameter on the procedure option.

– In addition, the FACTOR parameter can also be
included on the procedure option.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Automatic Stabilization and Dashpots

– For example,

*STATIC, STABILIZE

or

*STATIC, STABILIZE=
dissipated energy fraction

or

*STATIC, STABILIZE, FACTOR=
damping factor

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.15

Automatic Stabilization and Dashpots

– Volume proportional damping can be activated during any step of an
analysis.
• The values of the damping coefficient are not carried from one step to
the next.
• They are deactivated if the STABILIZE parameter is not re-declared
and recalculated if this parameter is re-declared.

Copyright 2004 ABAQUS, Inc. L7.16

ABAQUS: Selected Topics

Automatic Stabilization and Dashpots

• Output variables: Automatic
stabilization
– The total amount of viscous energy
dissipated by volume proportional
damping is reported separately from
other viscous dissipation energies by
means of the element output variables
ELSD and ESDDEN and the global
energy variable ALLSD.
• Use the ∗ENERGY OUTPUT or
∗ENERGY PRINT option to
request this output.
• The reported energy can be
limited to a group of elements.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.17

Automatic Stabilization and Dashpots

– The nodal viscous forces and
moments are available as nodal

output variable VF (VFn and VMn).

– The damping factor calculated by
ABAQUS is reported in the
message (.msg) file.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.18

Automatic Stabilization and Dashpots

ELSD Element stabilization dissipation energy

ELSDDN Element stabilization dissipation energy
ALLSD density
Element set or model stabilization dissipation
Not output energy
by default to
VF Nodal viscous forces
.odb file!
c Damping factor (message file)

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.19

Automatic Stabilization and Dashpots

• If you want to know how much you
altered a problem by adding
stabilization, look at:
1 Energy dissipation due to stabilization
• Look at whole model energies.

Here, the total energy dissipated due
to stabilization is very small compared
to the total energies involved in
deformation.

VF

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.20

Automatic Stabilization and Dashpots 10000

2 Viscous forces during deformation 1.5

• The figures at right show the load
and viscous forces at the load
application point as functions of
displacement

• VF varies significantly in time; its
order-of-magnitude is very small
compared to the global load,
however.

• Can conclude the presence of
stabilization has not changed the
problem significantly.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.21

Automatic Stabilization and Dashpots

• Automatic stabilization usage hints

– The automatic calculation of the damping factor, c, is done based on

information obtained during the first increment of a step.

• Thus, the first increment should be representative of the deformation
pattern that follows.

• If the character of the deformation changes during the step, split the
step to force a reevaluation of damping.

– If the first part of the step can be completed without stabilization, it is better
to split the step and introduce stabilization in the latter steps.

• This ensures that a stable response is the basis for computing the
damping factor.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.22

Automatic Stabilization and Dashpots

• Dashpot usage hints

– To select the damping coefficients in the dashpots, the following procedure
can be used:

• Estimate the magnitude of the displacements that will occur after
buckling.

• Divide the estimated displacement magnitude by the step time to get
an estimate for the velocity that would occur if the response were
stable.

• Determine typical nodal forces in the model prior to buckling.

• Choose the damping coefficients such that, for the estimated velocity,
the damping forces will be one to two orders of magnitude less than
the static forces.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.23

Automatic Stabilization and Dashpots

• Dashpot output variables
– The total viscous energy dissipated by dashpots is included in the global
energy variable ALLVD.
– The viscous forces in the dashpots are reported as element variable S11.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.24

Automatic Stabilization and Dashpots

• Summary

– The methods described on the previous pages will have the result that,
prior to buckling, the damping has almost no effect on the solution.

• However, as soon as instability in the structure develops, the
velocities increase rapidly and damping starts to become effective.

• For the solution procedure to converge, the time increment will usually
decrease as the velocities increase, leading to a controlled
postbuckling behavior.

– Damping in a static analysis should not be combined with the Riks
procedure.

• The Riks procedure will calculate the velocities as displacement
increments divided by the arc length; hence, these pseudo-velocities
will not increase sufficiently for the dashpots to become effective.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.25

Automatic Stabilization and Dashpots

• Example 1: Damped static
postbuckling analysis
– As an example of dynamic
postbuckling, consider this frame
structure.
• This structure can also be
analyzed with the quasi-static
method.
– The structure is expected to buckle
at a load of about 57,500 lbs.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.26

Automatic Stabilization and Dashpots

– To investigate the postbuckling behavior, we apply a load of 150,000 lbs.
– The load-displacement curve obtained with the Riks quasi-static method

and the deformed shape at approximately 250,000 lbs are shown below:

Buckling
occurs here

unstable

stable

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.27

Automatic Stabilization and Dashpots

– To analyze the problem as a damped static problem, we add DASHPOT1
elements to every single node in degree of freedom 1 and 2.

• To calculate a damping value for the dashpots, we estimate typical
nodal forces on the order of 10,000 lbs.

• Considering that the load is applied over a period of 10 sec and the
total deflection is on the order of 100 in, a typical constant velocity to
attain the total deformation would be about 10 in/sec.

– With these assumptions the damping coefficient corresponding to the
velocity would be 1000 lb sec/in.

• We choose 1% of this value as the actual damping coefficient.

– The partial input for this problem follows; the load-deflection and energy-
deflection curves are shown on the subsequent pages.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.28

Automatic Stabilization and Dashpots

• Damped static postbuckling analysis: partial input

*Heading
Frame -- damped static postbuckling analysis
:

*Imperfection, file=framEigen, step=1
1, -0.12

*Boundary
ends, 1, 2

*Element, type=dashpot1
:

*Dashpot, elset=dashpotx
:

*Dashpot, elset=dashpoty
:

*Step, nlgeom, inc=400
*Static

0.1, 10., , 0.25
*Cload

corner, 2, -200000.
*End step

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.29

Automatic Stabilization and Dashpots

• Damped static postbuckling analysis: results

Snap-through

Load-displacement curve Instability
starts here
Copyright 2004 ABAQUS, Inc.
Energy-displacement curve

ABAQUS: Selected Topics L7.30

Automatic Stabilization and Dashpots

– As can be seen from the load-displacement curve, the load increases until
the instability develops.

– When the instability develops, the load remains almost constant while the
structure snaps through to a stable state.

– The final deformed shape of the frame is in static equilibrium without
significant forces in the dashpots and agrees with the solution obtained
with the Riks method.

– The energy curves show how the strain energy stored in the structure is
released in the form of dissipated energy when the snap-through occurs.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.31

Automatic Stabilization and Dashpots

• Example 2: Stabilized static postbuckling analysis

– The same problem is repeated with the dashpots replaced by volume
proportional damping.

– The problem is run with a dissipation intensity two orders of magnitude
smaller than the default.

• The default value is too high, because the first increment of the
analysis captures essentially axial deformation of the vertical member
of the structure.

• Later on, the snap-through behavior is dominated by bending of the
structure.

• Since the bending behavior is much less stiff than the axial behavior, a
small fraction of the axial strain energy is still relatively high when
compared with the bending strain energy.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.32

Automatic Stabilization and Dashpots

• Stabilized static postbuckling analysis: partial input

*Heading
Frame -- stabilized static postbuckling analysis
:
:

*Imperfection, file=framEigen, step=1
1, -0.12

*Boundary
ends, 1, 2

*Step, nlgeom, inc=400
*Static, stabilize=2.e-6

0.1, 10., , 0.25
*Cload

corner, 2, -200000.
*End step

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.33

Automatic Stabilization and Dashpots

• Stabilized static postbuckling analysis: results

Snap-through

Load-displacement curve Energy-displacement curve

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.34

Automatic Stabilization and Dashpots

– Both the load-displacement curves and the energy curves are very similar
to those in the static analysis damped with dashpots.
• The amount of damping was somewhat less than in the dashpot case
and can be controlled with the dissipation intensity.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Postbuckling and Loss of Contact

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.36

Postbuckling and Loss of Contact

– Often buckling and postbuckling problems are driven by moving contact
surfaces, and the structure buckles away from the contact surface.

– As discussed in Lecture 6, the Riks method is not able to analyze this kind
of problem.

– This kind of discontinuity does not present problems for damped static
analysis.

– At the load level at which contact is lost, the structure deforms without
being moved by the boundary conditions, and the inertia and viscous
forces ensure that the solution does not diverge.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.37

Postbuckling and Loss of Contact

• Example 3: Stabilization
static snap-through analysis
with contact

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.38

Postbuckling and Loss of Contact

– The contact load and the sum of reaction forces as a function of the
prescribed displacement are shown below.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Example

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.40

Example

• Local buckling of reinforced plate
– Plate with small and large reinforcements
– Spring connections to the rest of the structure
and symmetry boundary conditions
– Linear elastic material
– Axial loading

Courtesy of IRCN-France

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.41

Example – Then, buckling of a line of
sections and small
– First, localized buckling reinforcements occurs
occurs in the plate sections corresponding to the
between the small maximum load carrying
reinforcements. capacity.

– Total collapse of the plate
follows.

Contours of localized plate section buckling global buckling
(displacements normal to structure)
Buckling of a line of sections in the
Copyright 2004 ABAQUS, Inc. structure

ABAQUS: Selected Topics L7.42

Example

Buckling of line of sections
(loss of load-carrying capacity)

Local plate buckling

Axial force vs. axial displacement Energy history plots

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Summary

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.44

Summary

– Damped static postbuckling analysis is a useful technique to complement
classical eigenvalue buckling and static postbuckling analysis with the Riks
method.

– The primary advantage of this method is the reliability it offers, in particular
in conjunction with contact changes.

– Like static postbuckling analysis, the method provides an accurate
estimate of the critical load of imperfect structures, even if the structures
are imperfection sensitive.

– Unlike static postbuckling analysis, however, it does not provide detailed
insight into the nature of the postbuckling behavior.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.45

Summary

– The method is often useful for the analysis of crash and crushing
problems.

• In such problems buckling of the structure away from an indenter may
occur in the early phases of analysis, prior to large scale plastic
deformation.

• In such cases the postbuckling behavior is not the primary interest.

– The damped analysis technique regularizes this initial instability and
enables the analysis to proceed quickly to the deformation phase that is of
primary interest.

• The local contact surface damping option is provided specifically for
such applications.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Workshop 7a: Cargo Crane – Damped
Static Analysis

Workshop 7b: Cargo Crane – Dynamic
Analysis

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Lecture 8

Introduction to Contact in
ABAQUS/Standard

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.2

Overview

• Introduction • Contact Output
• Contact Examples • Solution of Contact Analyses
• Contact in Finite Element Analysis • Some Important Contact Issues
• Strict Master/Slave Contact • Workshop 8a: Hinge Model
• Overview of Defining Two-surface • Workshop 8b: Clip and Plate Model

Contact
• Surface Definition
• Adjusting Surfaces
• Local Surface Behavior
• Relative Sliding of Points in

Contact

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Introduction

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.4

Introduction

– When two solid bodies touch, contact stress is transmitted across their
common surface.
• In some cases only normal stress is transmitted.
• If friction is present, a limited amount of shear stress can also be
transmitted.
• The general objective is to determine contacting areas and stress
transmitted.

– Contact is a severely discontinuous form of nonlinearity.
• The contact constraint is either active or inactive—it is not smoothly
varying.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Contact Examples L8.6

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Contact Examples

– Hertz contact
• Small
displacements of
the contact
surfaces relative to
each other.
• Contact over a
distributed surface
area.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.7

Contact Examples Example: metal forming simulation

– Deformable to rigid Video Clip
body contact
• Typical examples:
– Rubber seals
– Tire on road
– Pipeline on seabed
– Forming
simulations (rigid
die/mold,
deformable
component).

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.8

Contact Examples Contact pressure
distribution due to
– Large-sliding contact interference
between deformable bodies resolution
• This is the most general
category of contact.
• Example: threaded
connector.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.9

Contact Examples SURF1
(rigid)
– Self-contact SURF2
• Self-contact is contact of a
single surface with itself. It is
available in two- and three-
dimensional models in
ABAQUS.

Contour of minimum principal stress

Example: Compression of a rubber gasket
(taken from “Self-contact in rubber/foam
components: rubber gasket,” Example
Problem 1.1.17 in the ABAQUS Example
Problems Manual)

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Contact in Finite Element Analysis

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.11

Contact in Finite Element Analysis

– Finite elements are based
on the concept of “local
support”—nodes and
elements communicate with
their nearest neighbors.

Exploded view of a mesh:
center element communicates with
its neighbors through its nodes

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.12

Contact in Finite Element Analysis The example shown here comes from
“Submodeling of a stacked sheet metal
• Why is it necessary to define contact? assembly,” Section 1.1.18 of the
ABAQUS Example Problems Manual.
– The concept of local support is not
sufficient for contact problems.

• Points and surfaces on one body
may need to recognize points and
surfaces on other bodies.

– There is currently no logic in
ABAQUS/Standard to detect contact
unless the user indicates that specified
surfaces and/or nodes might come into
contact.

• The surface of one body cannot
penetrate the surface of another
body (or itself if it folds).

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Strict Master/Slave Contact

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.14

Strict Master/Slave Contact

• Contact surfaces must be discretized because the underlying bodies are
discretized.

• With strict master/slave contact:
– Nodes on one surface (the slave surface) contact the discretized segments
on the other surface (the master surface).

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.15

Strict Master/Slave Contact

• The strict master/slave formulation used in ABAQUS/Standard has
kinematic implications.
– Slave nodes cannot penetrate master surface segments.
– Nodes on the master surface can penetrate slave surface segments.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.16

Strict Master/Slave Contact

• Approaches to master/slave contact
– Node-to-surface
• Contact is enforced between the slave node and the master surface
facets local to the slave node
• Default method for contact interactions

slave

master

These nodes are
free to penetrate

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.17

Strict Master/Slave Contact

– Surface-to-surface
• Contact is enforced in a weighted sense, between the slave node and
a larger number of master surface facets surrounding it.

slave

More master surface nodes are master
involved in contact, reducing
the likelihood of penetration.

• In effect, contact is smeared over a larger number of facets.

– Analogous to converting the slave contact force to a local surface
pressure and applying that pressure to the master surface.

• Alternative for small sliding contact; default for tie constraints.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.18

Strict Master/Slave Contact

• Choice of master and slave surfaces
– The proper choice of master and slave surfaces is critical.
• Slave surfaces allow penetration; master surfaces do not.
• With the keywords interface, the slave surface is the first surface
named under the *CONTACT PAIR option:

*CONTACT PAIR, INTERACTION=EXAMPLE

slave, master

With the GUI interface, the
slave and master surfaces
are specified explicitly.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.19

Strict Master/Slave Contact

• Mesh density considerations
– Choose slave surfaces to be the more finely meshed surface.
– If mesh densities are equal, the slave surface should be the surface with
the softer underlying material.

Incorrect Correct
Master surface placed on fine mesh⇒
Gross penetration into slave surface Master surface placed on coarse mesh⇒
Minimal penetration into slave surface
Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Overview of Defining Two-surface
Contact

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.21

Overview of Defining Two-surface Contact

– For even the simplest contact problem the user must decide:
• What constitutes each surface.
• Which pairs of surfaces will interact.
• Which surface is the master, and which is the slave.
• Which surface interaction properties are relevant: friction, softened
layers, etc.

– ABAQUS automatically creates internal contact elements based on these
decisions.

– These internal elements are almost completely transparent to the user.
• The only time a user will typically want to review these elements is
when something goes wrong.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.22

Overview of Defining Two-surface Contact

• Defining a contact interaction
in ABAQUS/CAE
1 Create an interaction, and
select the steps in which it
will be active.

Create Interaction dialog box

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.23

Overview of Defining Two-surface Contact

2 Select the application surfaces
from geometric surfaces,
element faces, surface sets, or
node sets.
Surfaces on orphan meshes
can be selected by picking one
element face and a feature
angle. Individual edits make it
easy to clean up anomalies.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.24

Overview of Defining Two-surface Contact

3 In the Edit Interaction dialog
box, complete the interaction
definition (for example, for
contact interactions define the
friction model).

Create Interaction Property dialog box Edit Interaction dialog box

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.25

Overview of Defining Two-surface Contact

4 Use the Interaction Manager to manage multiple contact
interactions as necessary.

Interaction Manager

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Surface Definition

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.27

Surface Definition

• User-specified contact faces: GUI
interface
Solid bodies
– The surface on a solid is defined
by selecting the appropriate
region of the exterior of the part.
– Regions may be selected
individually or based on face
angles.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.28

Surface Definition

• User-specified contact faces: GUI interface (cont'd)

Shells and beams
The surface on a
shell/membrane or
beam/truss is defined by
choosing the
appropriate side of the
part.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Adjusting Surfaces

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.30

Adjusting Surfaces

– The slave nodes of any contact pair can be “adjusted” automatically so that
they are initially in contact with the master surface.
• This process is useful when preprocessors do not place nodes in
“exact” positions.
• ABAQUS modifies coordinates of slave nodes before the analysis
starts.
• The adjustment does not generate any strain.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.31

Adjusting Surfaces

– The initial positions of the nodes on the contact surfaces can be adjusted
without stress or strain prior to the analysis.
• ABAQUS/Standard allows the user to adjust the nodes by specifying
either
– an absolute distance or
– a node set.

– Warning: With either method only surface nodes are relocated.
• Gross (large) adjustments can severely distort initial element shapes.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.32

Adjusting Surfaces

1.0
CONNODE

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Local Surface Behavior L8.34

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Local Surface Behavior

– General contact modeling
includes contact interactions in
directions:
• Normal to the master
surface
• Tangent to the surfaces

– Other contact interactions
include contact damping.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.35

Local Surface Behavior Pressure-clearance relationship

• Behavior in the contact
normal direction

• Hard contact
– “Hard” contact is the default
local behavior in all contact
problems.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.36

Local Surface Behavior

– Alternatives to hard contact
• Contact without separation.
• Softened contact
(exponential or tabular
pressure-clearance
relationship)

Contact with separation “Soft” contact

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.37

Local Surface Behavior

– Behavior in the contact
tangential direction
• Frictional shear

stresses, τ, may develop

at the interface between
contacting bodies.
• If the magnitude reaches
a critical value, the
bodies will slip;
otherwise they will stick.

– Friction is a highly nonlinear effect.
• Solutions are more difficult to obtain.
• Do not use unless physically important.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.38

Local Surface Behavior

– Four friction models are available in ABAQUS:
• Isotropic Coulomb friction (with shear stress cap)
• Anisotropic Coulomb friction (with shear stress cap)

• Exponential form where µs decays to µk exponentially

• User-defined (through user subroutine FRIC or UINTER)
– Two friction algorithms are implemented:

• Penalty method
• Lagrange multiplier method
– The most common (and default) combination is isotropic Coulomb friction
using the penalty method.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.39

Local Surface Behavior

– Default Coulomb friction model

• The critical frictional stress depends on

contact pressure: τ = µp.
cr

• The friction coefficient, µ, can be a

function of the relative slip velocity,
pressure, temperature,

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.40

Local Surface Behavior τcrit

– By default, ABAQUS uses an ideal
adaptive penalty method.
• It approximates stick with penalty
stiff elastic behavior.

• Small elastic slip, γcrit, is
permitted before τeq = τcrit.

G γcrit

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.41

Local Surface Behavior

Copyright 2005 ABAQUS, Inc.
ABAQUS: Selected Topics

Relative Sliding of Points in Contact

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.43

Relative Sliding of Points in Contact

• Two slide distance options:

– Finite sliding Finite sliding is the most general—used by default.
– Small-sliding
Arbitrarily large sliding between surfaces
and large rotations are allowed.

Small relative sliding between surfaces.

Allows large rotations of the surfaces, as long as
the surfaces do not move significantly relative to
each other.

Computationally less expensive than finite sliding.

• While small-sliding is less expensive, take care to use it only in cases
where small tangential motions are expected

– Non-physical behaviour can result if it is used inappropriately

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.44

Relative Sliding of Points in Contact

Edit Interaction dialog box

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Contact Output

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.46

Contact Output

• Contact information is available for all surfaces.
– Contact stresses: CSTRESS (contact pressure CPRESS and frictional
shear stresses CSHEAR1 and CSHEAR2)
– Contact displacements: CDISP (contact opening COPEN, relative
tangential motions CSLIP1 and CSLIP2)

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.47

Contact Output

• Field output requests

CPRESS,
CSHEAR1, and
CSHEAR2

COPEN,
CSLIP1, and
CSLIP2

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.48

Contact Output

– Solver contact output
• Controls output to the message file during the analysis phase.
• Gives details of the iteration process.
• Use to understand where difficulties are occurring during contact.

Activate in the Edit Diagnostic Print dialog box of the Step module

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Solution of Contact Analyses

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.50

Solution of Contact Analyses

• Contact requires the imposition of constraints between the points that are
in contact.
– Different ways of imposing constraints.
– ABAQUS/Standard uses the Lagrange multiplier method.
– For each potential contact point the contact condition is described by a
single, often nonlinear, inequality constraint:

h(u1, u2, u3, ...) ≤ 0,
where h is the “penetration” and uN are degrees of freedom.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.51

Solution of Contact Analyses

• Contact algorithm determine closed h>0

begin increment 1

h≤0 contact state
open

do not apply apply
2 constraint 2 constraint

point opens; perform point closes;
severe severe
3
5 discontinuity 5 discontinuity
iteration iteration iteration

p<0 check for h>0
4 changes in

contact

no changes

end increment 6 check
equilibrium
8 convergence 7 no convergence

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.52

Solution of Contact Analyses

– The algorithm distinguishes between “severe discontinuity iterations” and
“equilibrium iterations” and can be described as follows:
1 Determine current contact state at each point (closed or
open).

2 Impose contact constraints, calculate stiffness.

3 Perform iteration ⇒ pass through the solver once.

4 Contact pressures and clearances consistent with contact
state? If yes, go to 6. If no, go to 5.

– Point was closed; confirm that p > 0.
– Point was open; confirm that h < 0.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.53

Solution of Contact Analyses

5 Contact state changed: the start of the iteration was
based on the wrong state.
– Flag the point as having an incorrect contact estimate.
– Label and count this iteration as an SDI (severe discontinuity
iteration).
– Reset equilibrium iteration counter to zero. Go back to 1.

6 After all SDIs, check force residuals to determine
equilibrium.
– Label and count this iteration as an equilibrium iteration.

7 If equilibrium is not satisfied, iterate again with the same
contact state. Go to 3.

8 If equilibrium is satisfied, the increment ends.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.54

Solution of Contact Analyses

• Contact diagnostics example
– Reference: Example Problem 1.3.4, Deep drawing of a cylindrical cup

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.55

Solution of Contact Analyses

– Visual diagnostics are available in the Visualization module of
ABAQUS/CAE.

Step 3, Increment 6: 4 SDIs +
2 equilibrium iterations

Visualization module: Tools Job Diagnostics

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.56

Solution of Contact Analyses Slave nodes
that close: h > 0

Toggle on to see the locations
in the model where the contact
state is changing.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.57

Solution of Contact Analyses Slave nodes
that open: p < 0

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.58

Solution of Contact Analyses Slave nodes that slip;
stick/slip messages cause
SDIs only if the Lagrange
multiplier method is used.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.59

Solution of Contact Analyses

There are no residual checks in
this iteration since the contact
consistency checks did not pass.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.60

Solution of Contact Analyses

3 additional SDIs are required
before the contact state is
established; once the contact
checks pass, the residuals
checks are performed.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Some Important Contact Issues

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L8.62

Some Important Contact Issues

• Contact is an extremely discontinuous form of nonlinearity
– During solution of contact problems, ABAQUS has to perform iterations to
resolve the correct contact state, ie
• which nodes are in contact and what the contact pressures are
• which nodes are not in contact
– This adds another level of complexity to the solution process
• Contact problems in general require more CPU time to solve

Copyright 2005 ABAQUS, Inc.