Assigning Surface Properties for General Contact in Abaqus/Explicit

Surface property assignments:

can be used to change the contact thickness used for regions of a surface based on structural elements or to add a contact thickness for regions of a surface based on solid elements;
can be used to specify surface offsets for regions of a surface based on shell, membrane, rigid, and surface elements;
can be used to specify which edges of a model should be included in the general contact domain;
can be used to specify geometric corrections for regions of a surface;
can be used to assign a coordinate system for local tangent directions to the surface and/or specify preferential frictional directions to the surface in the context of anisotropic friction;
can be used to assign surface-based friction coefficients, such that friction coefficients for interactions can be approximated from surface-based friction coefficients; and
can be applied selectively to particular regions within a general contact domain.

This page discusses:

Assigning Surface Properties
Surface Thickness
Surface Offset
Feature Edges
Surface Geometry Correction
Surface-Based Friction Coefficients
Orientations
Preferred Fraction of Frictional Work Directed to a Surface as a Surface Property

Assigning Surface Properties

You can assign nondefault surface properties to surfaces involved in general contact interactions. These properties are considered only when the surfaces are involved in general contact interactions; they are not considered when the surfaces are involved in other interactions such as contact pairs. The general contact algorithm does not consider surface properties specified as part of the surface definition. The regions with nondefault surface properties are identified with surface names or material names. For example, surface property SurfProp_A can assign a nondefault surface thickness to surface Surf_1 or to the surface whose underlying elements have a section assignment with material Rubber. Material names cannot be used to assign geometric corrections.

Surface property assignments propagate through all analysis steps in which the general contact interaction is active.

The surface names used to specify the regions with nondefault surface properties do not have to correspond to the surface names used to specify the general contact domain. In many cases the contact interaction will be defined for a large domain, while nondefault surface properties will be assigned to a subset of this domain. Any surface property assignments for regions that fall outside the general contact domain will be ignored. The last assignment will take precedence if the specified regions overlap.

Surface Thickness

The default calculation of the nodal surface thickness (described in detail below) is appropriate for most analyses; one exception is sheet forming analysis, in which the thinning of a sheet significantly influences contact. This case can be modeled by specifying that the decreasing parent element thickness should be used. As a third alternative, you can specify a value for the surface thickness. A nonzero thickness can be assigned to solid element surfaces, for example, to model the effect of a finite-thickness surface coating. Element-Based Surface Definition contains information on the spatial variation of the surface thickness.

Specifying the original or decreasing thickness results in a zero thickness for node-based surfaces; you can specify a nonzero thickness for a node-based surface used with the general contact algorithm (the contact pair algorithm will not consider a nonzero thickness for such surfaces).

The general contact algorithm requires that the contact thickness does not exceed a certain fraction of the surface facet edge lengths or diagonal lengths. This fraction generally varies from 20% to 60% based on the geometry of the element. The general contact algorithm will scale back the contact thickness automatically where necessary without affecting the thickness used in the element computations for the underlying elements. Diagnostic information is provided in the status (.sta) file if such scaling is performed.

To bypass this limitation on thickness, the contact surface can be modeled with surface elements (see Surface Elements). The surface elements must be attached to the underlying elements using a surface-based tie constraint (see Mesh Tie Constraints), and a physically reasonable mass must be associated with the surface elements. This requires a significant fraction of the mass to be transferred to the surface elements from the underlying elements without appreciably altering the bulk mass properties. Alternatively, contact controls settings can be used to limit the thickness reduction checks (see Contact Controls for General Contact in Abaqus/Explicit).

The “bull-nose” effect that occurs at shell perimeters with the contact pair algorithm (see Assigning Surface Properties for Contact Pairs in Abaqus/Explicit) is avoided with the general contact algorithm by default. Shell element edges, nodes, and facets reflect the shell thickness in the normal direction only and do not extend past the perimeter. Contact controls settings can be used to turn off the bull-nose prevention checks (see Contact Controls for General Contact in Abaqus/Explicit).

Using the Original Parent Element Thickness

By default, the nodal thickness for surfaces based on shell, membrane, or rigid elements equals the minimum original thickness of the surrounding elements (see Figure 1 and Table 1). If a node is shared by shell and beam elements, the contact thickness that takes precedence is the one derived from the shell element. To account for thick beams that are colocated with shell edges, the beam elements must be attached to the shell edges using a tie constraint (see Mesh Tie Constraints).

Table 1. Thicknesses corresponding to figure showing continuous variation.
Node	Element	Specified element thickness	Nodal surface thickness (minimum of adjacent element thicknesses)
1			0.5
	a	0.5
2			0.5
	b	0.5
3			0.5
	c	0.9
4			0.9
	d	0.9
5			0.9

The surface thickness within a facet is interpolated from the nodal values; the interpolated surface thickness never extends past the specified element or nodal thickness, which may be significant with respect to initial overclosures. The default nodal surface thickness is zero for regions of a surface based on solid elements. If a spatially varying nodal thickness is defined for the underlying elements (see Nodal Thicknesses), the nodal surface thickness may not correspond exactly to the specified nodal thickness (see node 4 in Figure 2 and Table 2).

Table 2. Thicknesses corresponding to figure showing small discrepancies.
Node	Element	Specified nodal thickness	Element thickness (average of specified nodal thickness)	Nodal surface thickness (minimum of adjacent element thicknesses)
1		0.5		0.5
	a		0.5
2		0.5		0.5
	b		0.5
3		0.5		0.5
	c		0.7
4		0.9		0.7
	d		0.9
5		0.9		0.9
	e		0.9
6		0.9		0.9

The nodal surface thickness distribution will tend to be more diffuse than the specified nodal thickness distribution (because the specified nodal thicknesses are averaged to compute the element thicknesses, and the minimum of the surrounding element thicknesses is the nodal surface thickness).

Using the Decreasing Parent Element Thickness

If you specify that the decreasing parent element thickness should be used, only decreases in the parent element thickness are reflected in the contact surface thickness; if the parent element thickness actually increases during the analysis, the contact thickness will remain constant.

Specifying a Value for the Surface Thickness

You can directly specify the surface thickness value.

Applying a Scale Factor to the Surface Thickness

You can apply a scale factor to any value of the surface thickness. For example, if you specify that the decreasing parent element thickness should be used for surf1 and apply a scale factor of 0.5, a value of one half the decreasing parent element thickness will be used for surf1 when it is involved in a general contact interaction (all other surfaces included in the general contact domain will use the default original parent element thickness). Scaling the surface thickness in this way can be used to avoid initial overclosures in some situations. Abaqus/Explicit will automatically adjust surface positions to resolve initial overclosures (see Contact Initialization for General Contact in Abaqus/Explicit). However, if nodal position adjustments are undesirable (for example, if they would introduce an imperfection in an otherwise flat part, resulting in an unrealistic buckling mode), you may prefer to reduce the surface thickness and avoid the overclosures entirely.

Surface Offset

A surface offset is the distance between the midplane of a thin body and its reference plane (defined by the nodal coordinates and element connectivities). It is computed by multiplying the offset fraction (specified as a fraction of the surface thickness) by the surface thickness and the element facet normal. This defines the position of the midsurface and, thus, the position of the body with respect to the reference surface; the coordinates of the nodes on the reference surface are not modified. Surface offsets can be specified only for surfaces defined on shell and similar elements (i.e., membrane, rigid, and surface elements). Surface offsets specified for other elements (e.g., solid or beam elements) will be ignored. By default, surface offsets specified in element section definitions will be used in the general contact algorithm.

The surface offset at each node is the average of the maximum and minimum offsets among the faces connected to the node. The offset at a point within a facet is interpolated from the nodal values. Figure 3 shows some examples of the positioning of the contact surface with respect to the reference surface for various combinations of surface offsets. Surface offsets used in the general contact algorithm are constrained to lie between −0.5 and 0.5 of the thickness.

You specify the surface offset as a fraction of the surface thickness. The surface offset fraction can be set equal to the offset fraction used for the surface's parent elements or to a specified value. Surface offsets specified for general contact do not change the element integration.

Feature Edges

Feature edges of a model are defined on beam and truss elements and edges of faces (perimeter and otherwise) of solid and structural elements. Feature edges, such as shown in Figure 4, can participate in edge-to-edge contact in Abaqus/Explicit (see Surfaces Used for General Contact).

General contact domain, including edge-to-edge contact.

By default in Abaqus/Explicit:

“Contact edges” of beam and truss elements and perimeter edges of shells and membranes act as primary feature edges (see Primary and Secondary Feature Edges), as long as the underlying elements remain active.
Feature angle thresholds of 30° for primary feature edges and 20° for secondary feature edges are applied dynamically throughout a simulation to determine which edges of solid elements and which non-perimeter edges of shell elements currently act as primary or secondary feature edges. The feature angle is the angle formed between the normal directions of the two facets connected to an edge, as discussed further in The Feature Angle. As an edge’s feature angle evolves during a simulation, its classification as a primary feature edge, a secondary feature edge, or not a feature edge may also change. Figure 5 shows a crumpling example in which many feature edges form during a simulation. Other types of simulations (such as airbag deployment) involve many feature edges unfolding over the course of a simulation.

Using a Fixed Set of Active Feature Edges for Contact Based on Original Feature Angles

Optionally, Abaqus/Explicit can establish a fixed set of active feature edges for contact based on original feature angles. If no feature angle thresholds are specified explicitly, the list of active feature edges matches the default initially active feature edges for dynamically applied criteria (30° for primary feature edges and 20° for secondary feature edges), but this list is not updated during the simulation. This option is not well suited for common scenarios involving significant deformation during a simulation. However, using a fixed set of active feature edges can save computational time for simulations involving small deformation.

Limiting Feature Edges to Perimeter Edges and Contact Edges of Beams and Trusses

You can limit feature edges for edge-to-edge contact to perimeter edges and contact edges of beams and trusses. Perimeter edges occur on “physical” perimeters of shell elements and on “artificial” edges that occur when a subset of exposed facets on a body are included in the general contact domain. When structural elements share nodes with continuum elements, the perimeter edges are not activated on the structural elements because the criterion to designate them as such is no longer satisfied.

Specifying Particular Feature Edges to Be Activated

You can choose particular feature edges on surface, structural, and rigid elements to be activated in domain. A surface containing a list of element labels and edge identifiers (see “Defining edge-based surfaces” in Element-Based Surface Definition) is used to specify the edges to activate.

Specifying That All Feature Edges Should Be Activated

You can choose to activate all edges each increment in a given surface in the general contact domain. However, this option degrades performance.

Specifying That All Feature Edges Should Be Deactivated

You can choose to deactivate all feature edges (including perimeter edges) in the general contact domain. This option does not deactivate “contact edges” associated with beam and truss elements.

Specifying a Cutoff Feature Angle

If you specify a cutoff feature angle as the feature edge criteria, perimeter edges and geometric edges with feature angles greater than or equal to the specified angle are activated in the general contact domain. By default, the feature angle thresholds are applied dynamically throughout the simulation. Optionally, you can specify that the feature angle thresholds are applied only once at the beginning of the analysis. As described previously, you can activate additional feature edges if required.

Example: Assigning Different Feature Edge Criteria to Different Regions

You can assign a different feature edge criteria to different regions of the general contact domain. For example, Table 3 shows the input that could be used to specify that none of the feature edges of surf1, only perimeter edges of surf2, and perimeter edges and feature edges of surf3 with a feature angle greater than 30° should be considered for edge-to-edge contact.

Table 3. Feature edge criteria example: input file.
Input File Syntax
`surf1, NO FEATURE EDGES`
`surf2, PERIMETER EDGES`
`surf3, 30`

Primary and Secondary Feature Edges

To reduce computational cost in certain situations, it may be desirable to specify two feature angle criteria for a given surface. Edges satisfying the more restrictive criteria are considered primary feature edges, and edges satisfying the less restrictive criteria only are considered secondary feature edges. If primary and secondary feature edge criteria are in effect, Abaqus/Explicit enforces edge-to-edge contact between primary feature edges and between primary feature edges and secondary feature edges only. Edge-to-edge contact is not enforced between secondary feature edges. This ensures that interpenetrations are avoided at locations where there are “true” edges in the model, without the need to activate primary feature edges at locations where the gradients in the surface normals are only moderate. A judicious choice of criteria for selecting primary and secondary feature edges can lead to significant savings in computational costs.

Secondary feature edges can be selected for a surface by specifying a secondary feature edge criterion in addition to the criterion used to select the primary feature edges for that surface. If the secondary feature edge criterion is omitted, only primary feature edges are activated for the surface. Allowable criteria for secondary feature edges are:

all edges that have not been selected as primary feature edges;
all picked edges that have not been selected as primary feature edges;
all perimeter edges that have not been selected as primary feature edges; and
all edges with a feature angle greater than a specified cutoff angle value that have not been selected as primary feature edges.

The allowable values for the secondary feature edge criterion permit possible combinations of criteria for primary feature edges and secondary feature edges, shown in Table 4.

Table 4. Valid combinations of primary feature edge and secondary feature edge criteria.
Primary Feature Edge Criterion	Secondary Feature Edge Criterion
No feature edges	All remaining edges, picked edges, perimeter edges, cutoff angle
All edges	Any criterion specified for secondary feature edges will be ignored
Picked edges	All remaining edges, perimeter edges, cutoff angle
Perimeter edges	All remaining edges, picked edges, cutoff angle
Cutoff angle	All remaining edges, picked edges, perimeter edges, cutoff angle

Specifying All Remaining Edges as Secondary Feature Edges

You can specify that all edges belonging to the surface that have not been selected as primary feature edges become secondary feature edges.

Specifying Picked Edges as Secondary Feature Edges

You can specify that all picked edges of the surface that have not already been selected as primary feature edges become secondary feature edges.

Specifying Perimeter Edges as Secondary Feature Edges

You can specify that all perimeter edges of the surface that have not already been selected as primary feature edges become secondary feature edges.

Specifying a Cutoff Feature Angle for Secondary Feature Edges

You can specify that edges on the surface with a feature angle greater than the specified value that have not been selected as primary feature edges become secondary feature edges. If an angle value has also been specified for primary feature edges, the angle value specified for secondary feature edges must be smaller than the value specified for primary edges.

Specifying That Edges Are Activated Only as Secondary Feature Edges

For a particular surface you may not want to activate any primary feature edges; instead, you might want to activate all or some edges on the surface as secondary feature edges (to enforce contact between these secondary feature edges and primary feature edges on another surface in the model). In that case you can specify that no feature edges should be activated as the primary feature edge criterion for the surface, while using any criterion of choice for the secondary feature edges.

The Feature Angle

The feature angle is the angle formed between the normals of the two facets connected to an edge. By default, the angles between facets are based on the initial configuration. However, the most efficient approach for accurately resolving contact is often to apply the feature edge criteria to the current configuration. In this case the edges that are eligible for edge-to-edge contact evolve during the simulation.

A negative angle will result at concave meetings of facets; therefore, these edges are not included in the contact domain if the feature edge criteria is based on a cutoff feature angle. Figure 6 shows some examples of how the feature angle is calculated for different edges.

The feature angle for edge A is 90° (the angle between $n_{1}$ and $n_{2}$ ); the feature angle for edge B is −25° (the angle between $n_{2}$ and $n_{3}$ ). Edge C forms a T-intersection with three facets (shown in two dimensions in Figure 7); its feature angles are 0°, −90°, and −90°.

Perimeter edges (for example, edge D in Figure 6) can be thought of as a special type of feature edge where the feature angle is 180°.

The sign of the feature angle is considered when determining whether or not a geometric feature edge should be activated in the general contact domain. For example, if a cutoff feature angle of 20° were specified, edge A would be activated as a feature edge in the contact model (90° > 20°) but edges B and C would not be activated: −25° < 20° and 0° (the maximum feature angle for edge C) < 20°.

Figure 8 illustrates further how the feature angle is used to determine which geometric feature edges should be activated in the general contact domain.

The table to the right of the figure lists the feature angle values for various edges in the model. Edges connected to more than two facets, as well as edges connected to two shell facets, have more than one corresponding feature angle. The largest feature angle at an edge is compared to the specified cutoff feature angle. For example, if a cutoff feature angle of 20° were specified, edges A, D, and E would be considered feature edges, while edges B, C, and F would be ignored for edge-to-edge contact.

Output

The contact output variable CEDGEACTIVE is available to identify throughout the analysis if an edge is active as a primary edge, active as a secondary edge, or has been deactivated by the contact domain.

Surface Geometry Correction

By default, contact calculations are based on unsmoothed, faceted representations of the finite element surfaces in a general contact domain. Discrepancies between the true surface geometry and the faceted surface geometry may result in significant noise in the solution. Optional contact smoothing techniques simulate a more realistic representation of curved surfaces in the contact calculations. These techniques allow a discretized surface with discontinuous surface normals to more closely approximate the behavior of a smooth surface during an analysis. Improvements to results with the surface correction include more accurate contact stresses and less solution noise upon relative sliding between contact surfaces.

Contact smoothing can be specified for surfaces in a general contact domain using a surface property assignment. A single surface property assignment specifies all of the surfaces to be smoothed, as well as the appropriate geometry correction method for each surface. Three geometry correction methods can be employed:

The circumferential smoothing method is applicable to surfaces approximating a portion of a surface of revolution.
The spherical smoothing method is applicable to surfaces approximating a portion of a sphere.
The toroidal smoothing method is applicable to surfaces approximating a portion of a torus (i.e., a circular arc revolved about an axis).

For each surface, you must specify the appropriate geometry correction method and either the approximate axis of revolution (for circumferential or toroidal smoothing) or the approximate spherical center (for spherical smoothing). For toroidal smoothing, you must also specify the distance of the center of the circular arc from the axis of revolution. The center of the circular arc is then located such that the line it forms with point (X_a, Y_a, Z_a) is perpendicular with the axis of revolution.

Considerations for Geometric Correction

The contact smoothing technique assumes that the initial locations of the surface nodes lie on the true initial surface geometry, with the exception of midedge nodes of C3D10M elements. This smoothing technique remains effective even if the midedge nodes of C3D10M elements do not lie on the true initial geometry.

The effects of contact smoothing tend to be most significant for analyses involving small deformation, and the smoothing technique works well for cases involving large relative motion between the surfaces. For analyses with large deformation this smoothing technique typically has an insignificant effect on the solution. However, in some cases—especially where the underlying elements can fail—the smoothing can degrade the solution accuracy after large deformation.

Effects of Geometric Correction

The impact of contact surface smoothing can be demonstrated by a simple model of contact between concentric cylinders with a small clearance between them. With a matched mesh as shown in Figure 9 there are no initial overclosures; therefore, there are no initial strain-free initial displacement adjustments. However, if the inner cylinder is rotated, the cylinders develop stresses (see Figure 10) as contact is detected due to the linear faceted representation of the main surface. This behavior is improved when the circumferential smoothing technique is applied to the contacting surfaces of the two cylinders.

Surface-Based Friction Coefficients

In Abaqus/Explicit you can establish friction coefficients as mathematical combinations of coefficients specified as surface properties (see Deriving Friction Coefficients from Quantities Specified as Surface Properties). For contact between surfaces with identical surface-based coefficients, the function to compute the friction coefficient for an interface returns the same coefficient; otherwise, this function returns a coefficient between the two surface-based coefficients and closer to the lower of the surface-based coefficients. See Deriving Friction Coefficients from Quantities Specified as Surface Properties for more details about this capability, including user control of the function for computing interaction friction coefficients for surface-based friction coefficients.

Orientations

For surface regions, you can specify

the initial orientation of local tangent directions and/or
the degree of frictional directional preference for the local $t_{1}$ versus $t_{2}$ tangent directions in the context of an anisotropic friction model.

For each surface region, you can refer to a named orientation system and, if desired, an extra rotation (in degrees) applied to the orientation system once it has been projected to the surface. If no orientations are specified or an analytical rigid surface is used, Abaqus initializes the contact directions using the standard convention (see Conventions).

The specified local coordinate system is associated with a surface; whereas, the local tangent directions discussed in Local Tangent Directions for Contact are associated with contact constraints. The local coordinate system for contact is inherited from one of the surfaces, as discussed in Local Tangent Directions for Contact.

A preferred frictional direction for a surface in conjunction with anisotropic friction behavior can be specified using a frictional directional preference factor $ϵ$ (default) or a frictional directional preference ratio r (see Anisotropic Friction with Directional Preference as a Surface Property).

Preferred Fraction of Frictional Work Directed to a Surface as a Surface Property

In Abaqus/Explicit you can specify the preferred fraction of frictional work of an interaction directed to a surface as a surface property. The default fraction is 0.5, which directs half of the friction work of an interaction to each surface. If the preferred fractions of the surfaces in an interaction do not sum to unity, a normalization process occurs in the context of the interaction such that the actual frictional work distribution fractions for that interaction sum to unity. This normalization process is described by the following equations:

f_{s u r f A}^{A B} = {\begin{matrix} \frac{1}{2} if f_{A_p r e f} = f_{B_p r e f} = 0 \\ \frac{f_{A_p r e f}}{f_{A_p r e f} + f_{B_p r e f}} o t h e r w i s e \end{matrix}, f_{s u r f B}^{A B} = 1 - f_{s u r f A}^{A B} .

Frictional work distribution factors influence the nodal frictional work output but have no influence on the distribution of heat associated with friction to the respective interacting surfaces, which can be influenced with pre-existing gap heat generation controls (Modeling Heat Generated by Nonthermal Surface Interactions).