Reviewing the Adjustments of Initially Overclosed Surfaces
Initial strain-free adjustments of nodal positions are performed by
Abaqus/Standard
under various circumstances to remove contact overclosures (see
Contact Initialization for General Contact in Abaqus/Standard
and
Contact Initialization for Contact Pairs in Abaqus/Standard)
or to remove overclosures or gaps between surfaces of surface-based tie
constraints (see
Mesh Tie Constraints).
The initial configuration of the model is determined after these strain-free
adjustments are applied. There are two sources of information on the
adjustments of overclosed surfaces: the data (.dat) file
and the output database (.odb) file.
Output of Information on Strain-Free Adjustments to the Data File
By default, information about a limited number of strain-free nodal
adjustments is provided in the data (.dat) file.
Requesting more detailed output concerning contact constraints provides
information for all strain-free adjustments, regardless of the number of nodes
adjusted.
Visualizing Strain-Free Adjustments
Output variable STRAINFREE (see
Abaqus/Standard Output Variable Identifiers)
contains nodal vectors representing initial strain-free adjustments. By
default, this output variable is written to the output database
(.odb) file for the original field output frame at zero
time if any strain-free adjustments are made by
Abaqus/Standard.
Initial nodal positions written to
the output database file by
Abaqus/Standard
include the effects of strain-free adjustments, so plots of the initial
configuration show the adjusted nodal positions.
Reviewing Initial Contact Conditions
Before conducting an analysis, perform a data check on the model to review the initial contact
conditions (see Abaqus/Standard and Abaqus/Explicit Execution). The data check
creates an output database and calculates the variable
COPEN (contact opening) on each secondary
surface based on the initial configuration of the model.
In addition, you can instruct Abaqus to print detailed information about the initial contact conditions to the data file
during the data check (this information is not printed by default). The data file lists the
status (open or closed) and clearance distance for each constraint point on a secondary
surface, the internally generated contact element number associated with each secondary node
or facet, and a summary of contact interaction properties. Internally generated contact
elements are not user-defined and do not appear in the input file, so they can be difficult
to locate if an error or warning message refers to them. The information in the data file
can be used to locate these contact elements in the model.
The data file also lists the key parameters for every contact interaction in
the model. These parameters include:
Parameters are listed only for the interactions to which they are
applicable. For example, ,
surface smoothing, and the extension ratio are not used for surface-to-surface
contact calculations (including general contact), so
Abaqus
does not report values for these parameters in surface-to-surface interactions.
Output of Main Surface Nodes Associated with Secondary Nodes for Small-Sliding Contact
When you print initial contact conditions to the data file for contact pairs using the
small-sliding tracking approach, Abaqus creates an output table showing the main nodes associated with each secondary node.
Each row of the table lists a secondary node and the main nodes to which the secondary
node transfers load when in contact with the main surface. The number of nodes in the
table indicates whether or not the anchor point for a secondary node lies on an element
face or at a node. For details on the small-sliding tracking approach and load transfer,
see Using the Small-Sliding Tracking Approach.
In the output shown below for a two-dimensional model, secondary node 2 has an anchor point at
main surface node 101 because it interacts with three main surface nodes. Secondary node 1
has an anchor point between nodes 100 and 101. This table also provides a list of
secondary nodes that did not find an intersection with the main surface. This is important
because these nodes have no local tangent plane and, hence, can penetrate the main
surface.
SMALL SLIDING NON-RIGID AX ELEMENT(S)
INTERNALLY GENERATED FOR SECONDARY BLANK AND MAIN SPHERE
WITH SURFACE INTERACTION INF1
ELEMENT SECONDARY MAIN
NUMBER NODE(S) NODE(S)
46 1 101 100
47 2 102 101 100
50 9 NO INTERSECTION
***WARNING: 1 SECONDARY NODES FOUND NO INTERSECTION WITH A MAIN
SURFACE
Tracking Contact Status during a Simulation
You can write contact output to the data (.dat) file for tracking the
status of contact interactions over the course of an analysis. Tracking
contact status helps you ensure contact surfaces are defined appropriately,
troubleshoot a terminated contact analysis, and verify that contact
interactions behave realistically.
The data file offers a
detailed summary of the overall contact conditions and the forces
driving these conditions. However, it only provides output for successfully
completed increments.
Contact Output in the Data File
When you request contact output to the data file (see
Surface Output from Abaqus/Standard),
Abaqus
lists the contact status for every constraint point at each increment of the
analysis. The values of CPRESS,
CSHEAR, COPEN, and
CSLIP at each constraint point are also reported
by default.
Example: Forming a Channel
Contact diagnostics are often helpful in confirming that the interactions
in a model are behaving realistically and as intended. The diagnostics also
provide a means of tracing the evolution of contact statuses on a node-by-node
basis. In this example the diagnostics are based on a channel forming model.
The channel is formed from a steel plate (or blank) with appreciable thickness.
The blank is modeled with two-dimensional, plane strain elements; the forming
tools (die, holder, and punch) are modeled as analytical rigid surfaces. The
initial and final configurations of the model are displayed in
Figure 1.
You can
use the contact conditions to review changes in contact status
throughout the forming process.
This information might be used to confirm frictional or material effects.
For example, you can draw the following conclusions about these diagnostics in
the channel forming analysis:
If the slipping does not occur until well into the forming process,
frictional forces were probably holding the blank in place between the die and
holder.
Since all the nodes on the blank do not slip simultaneously, there is
most likely some mild stretching and nonuniform deformation occurring in the
blank.
For more insight on the slipping nodes, refer to the data file. The
following excerpt lists a portion of the blank-die interaction in the same
increment:
The contact status is indicated in the “footnote” column: open
(OP), closed and sticking tangentially
(ST), or closed and sliding tangentially
(SL). In the absence of frictional properties
the two contact statuses are open (OP) and
closed (CL).
In the output above node 290 is open; consequently, the contact pressure variable
CPRESS is zero. The
COPEN variable reports that this node
is 4.1155 × 10−7 length units away from the main surface. The
SL footnote for node 295 indicates that it is in
contact with the main surface (the die) and is “slipping.” The critical shear stress, , can be determined by the equation , where p is the value of contact pressure shown
under CPRESS and is the coefficient of friction for the contact interaction. In this
model = 0.1; the critical shear stress (4.4632 × 106 × 0.1 =
4.4632 × 105) is equal to the frictional shear stress
CSHEAR1, so the node is slipping. In
the case of node 300 the critical shear stress (9.5643 × 106 × 0.1 = 9.5643 ×
105) is greater than the frictional shear stress, so the node is sticking.
Likewise for node 305.
The CSLIP1 variable is the total accumulated
(integrated) slip at the secondary node. Accumulated slip and local tangent directions
are discussed in more detail in Output of Tangential Results.
Diagnosing a Terminated Contact Analysis
Contact diagnostics provide invaluable information when trying to resolve
errors in a terminated analysis. The diagnostics let you review trends in the
model's contact status, visually identify regions of the model involved in
contact difficulties, and numerically quantify the severity of an error.
Establishing contact conditions is a common source of difficulty in an
implicit static contact analysis. If an analysis terminates because it exceeds
the maximum number of severe discontinuity iterations (see
Severe Discontinuities in Abaqus/Standard),
the contact diagnostics give insight into how to resolve the problem. You can
plot the number of contact status changes over the course of an attempt.
If the changes are tending toward zero, increasing the allowed number of
severe discontinuity iterations or adjusting the
SDI conversion settings may allow
Abaqus
to resolve the contact conditions. If the changes are not tending toward zero,
you will need to revise your model or investigate other options.
If a particular contact pair or surface region is causing a majority of
the status fluctuations, you may need to modify the characteristics of the
associated interaction. For example, it is typically easier to resolve contact
conditions for contact pairs using the small-sliding tracking approach (if it
is applicable) than for those using the finite-sliding tracking approach.
Chattering
The contact diagnostics tool makes it very easy to detect chattering in a
model. In this situation the same node or constraint appears in the diagnostics
summary for every iteration, alternating as an overclosure or an opening. The
classic chattering scenario produces diagnostics plots that tend toward zero
but level off at a low number due to the oscillating contact status. Techniques for resolving contact
chattering problems are discussed in
Excessive Iterations in Contact Simulations.
Unrealistic and Severe Overclosures
When reviewing diagnostics, you may notice overclosures during unconverged
iterations for nodes or constraint points that are located outside of the
regions that are contacting in a converged state. The reported overclosure
value for these nodes will be significantly greater than the overclosures for
nodes within the contacting regions.
This is an indication of physical or numerical instabilities in the model.
You should take steps to more firmly establish contact before proceeding with
the simulation or add some form of stabilization to the model (see
Solving Nonlinear Problems,
Dashpots,
and
Automatic Stabilization of Rigid Body Motions in Contact Problems).
Using smaller increments can sometimes enable a solution to be obtained in
these cases.
Nonconverging Force Equations
Contact diagnostics do not always involve severe discontinuity iterations.
Poorly defined contact can lead to nonconvergence of the force equations in an
analysis.
If the same node appears repeatedly as the location of maximum residuals and
corrections, investigate the contact conditions around that node. Consider the
example in
Figure 2.
The diagnostics highlight the “problem node” on the perimeter of the secondary surface. A closer
look in the vicinity of this node reveals that the secondary surface mesh is too coarse.
Secondary nodes along the perimeter of the surface are touching the main surface, but the
next row of nodes is “hanging over” the rim of the main surface. If this contact pair uses
node-to-surface contact discretization, the main surface can penetrate the secondary
surface with little resistance between the nodes. Such penetrations can cause the
nonconverging force equations seen in the diagnostics.
Any situation in which the main surface is free to penetrate the secondary surface can prevent an
analysis from converging. Potential solutions include:
switching the main and secondary assignments;
using surface-to-surface discretization (however, using surface-to-surface discretization without
refining a coarse secondary mesh may lead to inaccurate stress results, even if the
analysis does converge); or