Contact Diagnostics in an Abaqus/Standard Analysis

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.

PREPRINT, CONTACT=YES 

Job module: job editor: General: Preprocessor Printout: Print contact constraint data

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. A symbol plot of this variable in the Visualization module of Abaqus/CAE shows vectors that represent how individual nodes have been adjusted, and a contour plot of this variable shows the distribution of the adjustment magnitude (you must select the original output frame at zero time in the Visualization module of Abaqus/CAE before choosing the STRAINFREE output variable). 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.

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

The diagnostics tool in the Visualization module of Abaqus/CAE can be used with the following procedure types:

• static stress/displacement;

• coupled thermal/stress; and

• coupled pore fluid flow/stress.

The diagnostics tool tracks all changes in contact during an analysis. Each time a constraint point's contact status changes from closed to open, it is recorded as an “opening.” Each time the status changes from open to closed, it is recorded as an “overclosure.” If the contact interaction involves frictional effects, the diagnostics note when a constraint point begins sliding along the main surface (“slipping”) and when a constraint point in motion stops on the main surface (“sticking”). The diagnostics tool lists the constraint point involved in the status change and allows you to highlight the location of the constraint point in the model. The calculated clearance or overclosure distance is also shown, and the maximum penetration is reported when the penetration tolerance for augmented Lagrange contact is exceeded (see Augmented Lagrange Method).

For the default contact convergence criteria, the diagnostics tool shows the maximum penetration error and the maximum estimated contact force error; these determine whether the contact conditions have converged (for details, see Severe Discontinuities in Abaqus/Standard). If you choose to use the traditional contact convergence criteria, these error measures are not reported. For analyses involving Lagrange friction, the diagnostics show the maximum slip error for points that should be sticking (see Shear Stress Versus Elastic Slip While Sticking).

For detailed instructions on using the diagnostics tool, see Viewing diagnostic output. The contact diagnostic information available in Abaqus/CAE can also be printed to the Abaqus message file. For details, see The Abaqus/Standard Message 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.

Figure 1. Model for channel-forming example. (The blank has been extruded for visualization purposes.)

If you include a step or prescribed condition in your model intended to establish contact between two surfaces, the diagnostics tool in Abaqus/CAE can confirm the success of this modeling technique. In this example contact must be firmly established between the blank, the die, and the holder before the forming process begins. Small but consistent overclosures in the nodes along the surface of the blank indicate that the contact conditions are appropriate to begin forming the channel (see Figure 2).

Figure 2. Diagnostics confirming contact conditions between the blank, die, and holder.

You can also use the contact conditions to review changes in contact status throughout the forming process. Figure 3 depicts the onset of slipping for two nodes on the blank.

Figure 3. Diagnostics for the onset of slipping.

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 depicted in Figure 3:

    NODE  FOOT-   CPRESS      CSHEAR1     COPEN       CSLIP1  
          NOTE 

      290  OP    0.000       0.000      4.1155E-07 -2.8783E-07
      295  SL   4.4632E+06 -4.4632E+05   0.000     -5.1137E-06
      300  ST   9.5643E+06 -9.3177E+05   0.000     -4.8711E-06
      305  ST   2.9421E+06 -2.7867E+05   0.000     -4.7359E-06

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, ${\tau }_{crit}$ , can be determined by the equation ${\tau }_{crit}=\mu p$ , where p is the value of contact pressure shown under CPRESS and $\mu$ is the coefficient of friction for the contact interaction. In this model $\mu$ = 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.

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, as shown in Figure 4.

Figure 4. Changes in contact status during 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.

Using the visualization tools, you can see which areas of the model are involved in contact changes. 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.

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 (see Figure 4, for example). Techniques for resolving contact chattering problems are discussed in Excessive Iterations in Contact Simulations.

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, as seen in the highlighted constraint point in Figure 5.

Figure 5. The overclosure at one constraint point is significantly higher than the overclosures at other constraint points.

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.

Contact diagnostics do not always involve severe discontinuity iterations. Poorly defined contact can lead to nonconvergence of the force equations in an analysis (see Figure 6).

Figure 6. The diagnostics tool reports equilibrium difficulties.

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 7.

Figure 7. Two surfaces in a region of nonconverging force equations.

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

• refining the mesh on the secondary surface.