Optionally, you can redefine the overclosure tolerance to include larger overclosures in the interference fit. If you specify a tolerance that is smaller than the default calculated tolerance, Abaqus/Standard uses the default calculated tolerance instead. Input File Usage: \*CONTACT INITIALIZATION DATA, INTERFERENCE FIT, SEARCH BELOW=b Abaqus/CAE Usage: Interaction module: Interaction→Contact Initialization→Create: Treat as interference fits: Ignore overclosures greater than: b # Specifying the interference distance By default, the interference distance is implied by the initial overclosure of the mesh; alternatively, you can specify the interference distance. In this case Abaqus/Standard first makes strain-free adjustments of nodal positions such that the initial overclosure in the adjusted configuration corresponds to the specified interference distance and then invokes the shrink fit method discussed above, as depicted in Figure 36.2.4–3. Mesh distortion can occur if large strain-free adjustments are necessary to achieve the specified interference distance. The search region for the strain-free adjustments and subsequent shrink fit resolution is at least at large as the search region for the case discussed previously in which the interference distance is not specified. The search region will include overclosures at least as large as the specified interference fit and openings at least as large as the optionally specified search distance above a surface. Input File Usage: \*CONTACT INITIALIZATION DATA, INTERFERENCE FIT=h, SEARCH ABOVE=a, SEARCH BELOW=b Abaqus/CAE Usage: Interaction module: Interaction→Contact Initialization→Create: Treat as interference fits: Specify interference distance: h: Ignore overclosures greater than: b, Ignore initial openings greater than: a # Deactivating friction while resolving interference fits The presence of a friction model can degrade the robustness of resolving interference fits. It is generally recommended that you temporarily deactivate friction models while Abaqus/Standard resolves interference fits. You can deactivate the friction model in the first step while interference fits are resolved using the “change friction” method discussed in “Changing friction properties during an Abaqus/Standard analysis” in “Frictional behavior,” Section 37.1.5. # Cases in which interference fit resolution with contact pairs is preferred Large interferences may be difficult to resolve with the finite-sliding, surface-to-surface formulation. Using this formulation, overclosures tend to be resolved along the slave facet normal directions; using the node-to-surface formulation, which is available only with the contact pair algorithm, overclosures tend to be resolved along the master surface normal directions. Figure 36.2.4–4 illustrates a case where differing normal directions lead to undesirable tangential motion during an interference fit. In some cases it may be preferable to resolve large initial overclosures with node-to-surface discretization using the contact pair algorithm (see “Modeling contact interference fits in Abaqus/Standard,” Section 36.3.4).  Original mesh geometry After strain-free adjustments Middle of step End of step Figure 36.2.4–3 Treatment of a specified interference distance that differs from the interference implied by the original mesh. 

text_image

surface-to-surface node-to-surface master surface overclosure resolution direction

Figure 36.2.4–4 Comparison of contact formulations in an example with a large interference fit. # Assigning contact initialization methods You can assign contact initialization methods to selected surface pairings. The surface names used in the assignment of contact initialization methods do not have to correspond to the surface names used to specify the general contact domain. In many cases nondefault contact initialization methods will be assigned to a subset of the overall general contact domain. Any contact initialization assignments for regions that fall outside of the general contact domain are ignored. The last assignment takes precedence if the specified interactions overlap. # Input File Usage: Use the following option to assign contact inititialization methods: \*CONTACT INITIALIZATION ASSIGNMENT surface\_1, surface\_2, contact\_initialization\_method\_name This option must be used in conjunction with the \*CONTACT option. The data line can be repeated as often as necessary to assign contact initialization methods to different regions. If the first surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. If the second surface name is omitted or is the same as the first surface name, contact between the first surface and itself is assumed. Keep in mind that surfaces can be defined to span multiple unattached bodies, so self-contact is not limited to contact of a single body with itself. If the contact initialization method name is omitted, the default contact initialization method in Abaqus/Standard is assumed. If a contact initialization method name is specified, it must also appear as the value of the NAME parameter on a \*CONTACT INITIALIZATION DATA option in the model portion of the input file. # Abaqus/CAE Usage: Interaction module: Create Interaction: General contact (Standard): Contact Properties: Initialization assignments: Edit: select the surfaces and the initialization in the columns on the left, and click the arrows in the middle to transfer them to the list of contact initialization assignments # Assigning contact initializations to shell surfaces The surfaces in a contact initialization assignment can be either single- or double-sided. Single-sided surfaces must have consistent surface normal orientations for adjacent faces. Strain-free adjustments will not move surface nodes past the reference surface of the opposing surface if the assignment of a contact initialization method is made with double-sided surfaces. Using single-sided surfaces in the assignment of a contact initialization method for shells or membranes provides enhanced control over contact initialization for cases in which shell or membrane reference surfaces are initially crossed or are initially on the wrong side of each other. Figure 36.2.4–5 shows examples of adjustments for nearby segments of shell surfaces. For the case shown on the left it is assumed that single-sided surfaces with normal directions pointing away from each another are used in the assignment of the contact initialization method. In this case nodes are moved across the opposing reference surface during the strain-free adjustments. For the case shown on the right in Figure 36.2.4–5 it is assumed that single-sided surfaces with normal directions pointing toward each other are used in the assignment of the contact initialization method. In this case an initial gap is observed between the single-sided surfaces (which is also the case if double-sided surfaces are used in the contact initialization assignment). No strain-free adjustments will be made by default for openings such as this; however, if a nondefault contact initialization method is specified with an initial opening search tolerance set to a value exceeding the initial separation distance, strain-free adjustments will close the gap as shown in the figure (without moving nodes past the opposing reference surface). # Examples The following contact initialization assignments are specified below as model data in a general contact analysis: • a global assignment of shrink\_fit to the entire general contact domain; • a local assignment of shrink\_fit\_local to contact between surfaces surface\_A and surface\_B—the search zone is specified explicitly to increase the default overclosure tolerance; • a local assignment of the default Abaqus contact initialization method to contact between surface\_C and surface\_D; and • a local assignment of sfa\_pickside to contact between double-sided surfaces surface\_1 and surface\_2 by specifying one side of each surface, surface\_1\_TOP and surface\_2\_BOTTOM, in the data lines (see bottom left of Figure 36.2.4–5).  Figure 36.2.4–5 Strain-free adjustments during contact initialization for single-sided shell surfaces. ```c *CONTACT INITIALIZATION DATA, NAME=shrink_fit, INTERFERENCE FIT *CONTACT INITIALIZATION DATA, NAME=shrink_fit_local, INTERFERENCE FIT, SEARCH BELOW = 15.0 *CONTACT INITIALIZATION DATA, NAME=sfa_pickside, SEARCH BELOW = 10.0 ... *CONTACT *CONTACT INCLUSIONS, ALL EXTERIOR *CONTACT INITIALIZATION ASSIGNMENT , , shrink_fit ``` surface\_A, surface\_B, shrink\_fit\_local surface\_C, surface\_D, surface\_1\_TOP, surface\_2\_BOTTOM, sfa\_pickside # 36.2.5 STABILIZATION FOR GENERAL CONTACT IN Abaqus/Standard Products: Abaqus/Standard Abaqus/CAE # References • “Defining general contact interactions in Abaqus/Standard,” Section 36.2.1 • \*CONTACT • \*CONTACT STABILIZATION • “Creating contact stabilization definitions,” Section 15.12.5 of the Abaqus/CAE User’s Guide, in the HTML version of this guide • “Specifying and modifying contact stabilization assignments for general contact,” Section 15.13.4 of the Abaqus/CAE User’s Guide, in the HTML version of this guide # Overview Contact stabilization for general contact in Abaqus/Standard: • is often helpful in stabilizing unconstrained rigid body modes in static analyses; • can be applied selectively to particular regions within a general contact domain; and • can vary over time. # Stabilization based on viscous damping of relative motion between surfaces Contact stabilization is based on viscous damping opposing incremental relative motion between nearby surfaces, in the same manner as contact damping (see “Contact damping,” Section 37.1.3). The most common purpose of contact stabilization is to stabilize otherwise unconstrained “rigid body motion” before contact closure and friction restrain such motions. A goal of artificial stabilization, such as contact stabilization, is to provide enough stabilization to enable a robust, efficient simulation without degrading the accuracy of the results. In most cases contact stabilization is not activated by default (an exception is discussed in “Contact at a single point” in “Common difficulties associated with contact modeling in Abaqus/Standard,” Section 39.1.2), so you will generally need to activate contact stabilization if convergence problems associated with unconstrained rigid body modes may be present in your analysis. Once activated, contact stabilization is highly automated. The following expressions for the normal pressure, $\sigma _ { s t a b }$ , and shear stress, $\tau _ { s t a b }$ , associated with contact stabilization involve many semi-automated factors to facilitate achieving the desired stabilization characteristics: $$ \sigma_ {s t a b} = s _ {c o n s t} s _ {i t e r} s _ {a m p l} s _ {i n c r} s _ {g a p} c _ {d} v _ {r e l N}, $$ $$ \tau_ {s t a b} = s _ {c o n s t} s _ {i t e r} s _ {a m p l} s _ {i n c r} s _ {g a p} s _ {t a n g} c _ {d} v _ {r e l T}, $$ where

$c_d$	is a damping coefficient;
$v_{relN}$ and $v_{relT}$	are the relative normal and tangential velocities, respectively, between nearby points on opposing contact surfaces;
$s_{const}$	is a constant scale factor;
$s_{iter}$	is an iteration-dependent scale factor;
$s_{ampl}$	is a time-dependent scale factor;
$s_{incr}$	is a scale factor based on the increment number;
$s_{gap}$	is a scale factor based on the separation distance; and
$s_{tang}$	is a constant scale factor for tangential stabilization.

The damping coefficient and relative velocities are computed by Abaqus/Standard. The damping coefficient is equal to a fixed, small fraction, , times a representative stiffness of elements underlying the contact surfaces, $k _ { r e p } ,$ times the time period of the step, $t _ { s t e p }$ . Relative velocities in a static analysis are computed by dividing relative incremental displacements, $\Delta u _ { r e l N }$ and $\Delta u _ { r e l T }$ , by the time increment size, . Therefore, the following contact stabilization expressions apply to statics: $$ \sigma_ {s t a b} = \left[ s _ {c o n s t} s _ {i t e r} s _ {a m p l} s _ {i n c r} s _ {g a p} \left(\frac {t _ {s t e p}}{\Delta t}\right) f k _ {r e p} \right] \Delta u _ {r e l N}, $$ $$ \tau_ {s t a b} = \left[ s _ {c o n s t} s _ {i t e r} s _ {a m p l} s _ {i n c r} s _ {g a p} s _ {t a n g} \left(\frac {t _ {s t e p}}{\Delta t}\right) f k _ {r e p} \right] \Delta u _ {r e l T}, $$ where the portions within brackets can be thought of as stabilization stiffnesses (representing resistance to relative motion between nearby surfaces). The stabilization stiffness is inversely proportional to the time increment size, which is a desirable characteristic. Stabilization stiffness increases if the time increment size is reduced, which happens automatically in Abaqus/Standard if convergence difficulties occur for a particular time increment size. # Assigning stabilization to interactions Contact stabilization assignments for specific interactions within general contact can be made globally or locally and are specified as part of step definitions. In most cases you only need to specify which interactions are eligible for contact stabilization without adjusting the scale factors discussed previously. # Input File Usage: Use the following option to specify which interactions should use contact stabilization: \*CONTACT STABILIZATION surf\_1, surf\_2 If the first surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. If the second surface name is omitted, contact between the first surface and itself is assumed. Abaqus/CAE Usage: Use the following options to assign contact stabilization definitions to individual surface pairs: Interaction module: Create Interaction: General contact (Standard): Contact Properties: Stabilization assignments: Edit: select the surfaces and the stabilization name in the columns on the left, and click the arrows in the middle to transfer them to the list of contact stabilization assignments # Specifying stabilization scale factors In some cases you may want to adjust one or more scale factors associated with contact stabilization. You can use multiple instances of this option to achieve different scale factor settings for different general contact interactions. # Constant scale factors As shown in the expressions above for the stabilization pressure and shear stress, the scale factor $s _ { c o n s t }$ applies to normal and tangential stabilization, whereas the scale factor $s _ { t a n g }$ applies only to tangential stabilization. The default setting of the constant scale factor $s _ { c o n s t }$ is unity for the specified interactions. The default setting of $s _ { t a n g }$ is zero such that no tangential stabilization stiffness exists by default for the specified interactions. Normal-direction-only contact stabilization is adequate in many cases. Other analyses can benefit from tangential stabilization stiffness; however, if you specify a nonzero setting of $s _ { t a n g }$ , keep in mind that tangential contact stabilization often absorbs significant energy if large relative tangential motion occurs between nearby surfaces. Large energy absorbed by stabilization is one indication that analysis results are likely to be significantly affected by the stabilization. Normal contact stabilization is much less likely to absorb significant energy and, thus, tends to have less influence on the results. Input File Usage: $\mathrm { * C O N T A C T ~ S T A B I L I Z A T I O N } , \mathrm { S C A L E ~ F A C T O R } = \ l _ { { s _ { c o n s t } } } ,$ TANGENT FRACTION= $\mathrm { T A N G E N T ~ F R A C T I O N } { = } s _ { t a n g }$ Abaqus/CAE Usage: Interaction module: Interaction→Contact Stabilization→Create: Scale factor: $s _ { c o n s t }$ , Tangential factor: $s _ { t a n g }$ # Iteration-dependent scale factors To reduce or eliminate the likelihood of contact stabilization significantly influencing the reported solution, scale factors can be introduced that vary across iterations of an increment. Having more stabilization in effect during the early iterations of an increment can be helpful to avoid numerical problems prior to establishing active contact regions. Having less or no stabilization in effect during the later iterations can be helpful to improve the accuracy of the final converged iteration of an increment. You can specify these scale factors. For example, specifying “1,0” results in the scale factor being unity during initial iterations (until various convergence measures are satisfied or nearly satisfied) and then the scale factor being reset to zero (effectively turning off stabilization) for the final iterations until convergence checks are again satisfied. Input File Usage: \*CONTACT STABILIZATION, SCALE FACTOR=USER ADAPTIVE # Time-dependent scale factors The scale factors $s _ { a m p l }$ and $s _ { i n c r }$ control time-dependence of the contact stabilization. By default, $s _ { a m p l }$ is equal to the fraction of the step remaining. The other factor varies according to $s _ { i n c r } = f _ { i n c r } ^ { n _ { i n c r } - 1 }$ Jincr where $f _ { i n c r }$ is a per-increment reduction factor (equal to 0.1 by default) and $n _ { i n c r }$ is the increment number within a step. These defaults imply that the stabilization is reduced by more than an order of magnitude in successive increments of the same size and that no stabilization is applied in the final increment of a step. The defaults are appropriate for most cases in which contact stabilization is intended to provide stabilization in initial increments while contact is being established. Two options are provided for adjusting the time-dependent scale factors: you can refer to an amplitude curve that will govern $s _ { a m p l } .$ , and you can specify the value of $f _ { i n c r }$ (recall the expression $\bar { s _ { i n c r } } = f _ { i n c r } ^ { n _ { i n c r } - 1 }$ given previously). For example, if unstable modes remain after contact is established, you may want $s _ { a m p l }$ and $s _ { i n c r }$ to remain equal to unity throughout a step for certain interactions, which can be accomplished by referring to an amplitude with a constant value of one and setting the per-increment reduction factor, $f _ { i n c r }$ , equal to one. Input File Usage: \*AMPLITUDE, NAME=name \*CONTACT STABILIZATION, AMPLITUDE=name, REDUCTION PER INCREMENT= Abaqus/CAE Usage: Load or Interaction module: Create Amplitude: Name: name Interaction module: Interaction→Contact Stabilization→Create: Reduction factor: $f _ { i n c r }$ , Amplitude: name Resetting time-dependent scale factors in subsequent steps Contact stabilization definitions do not affect subsequent steps unless an amplitude reference is specified. If an amplitude based on the total time is specified, the same amplitude curve continues to govern the variation of $\dot { } s _ { a m p l }$ in subsequent steps until a new contact stabilization definition is assigned to the interaction. If an amplitude based on the step time is specified, the amplitude curve governs $s _ { a m p l }$ for a single step and $s _ { a m p l }$ remains constant (at the ending value) in subsequent steps until a new contact stabilization definition is assigned to the interaction. In both cases you can also reset the contact stabilization definition to remove stabilization from a step. Resetting ensures that contact stabilization options from prior steps do not affect the current step. Input File Usage: \*CONTACT STABILIZATION, RESET Abaqus/CAE Usage: Load or Interaction module: Create Amplitude: Name: name Interaction module: Interaction→Contact Stabilization→Create: Reset values from previous steps