A surface-to-surface contact definition can be used as an alternative to general contact to model contact interactions between specific surfaces in a model. Certain interaction behaviors can be defined only by using surface-to-surface contact. For a brief overview of surface-to-surface contact and other types of interactions available in Abaqus, see “Understanding interactions,” Section 15.3, and “Contact interaction analysis: overview,” Section 36.1.1 of the Abaqus Analysis User's Guide.
You can define surface-to-surface contact in any step, including the initial step. Select Interaction
Create from the main menu bar, and select the master and slave surfaces. You can define contact between edges of a wire or between faces of a solid or shell. Certain connectivity restrictions apply to contact surfaces depending on the type of contact formulation. You can deactivate a surface-to-surface contact interaction in a step and, if desired, reactivate this interaction in a subsequent step. You can deactivate the interaction in a step if it will no longer be needed in the analysis.
If you are creating multiple surface-to-surface contact interactions, you may want to use the contact detection tool. This tool automates the process of selecting surfaces and allows you to create multiple interactions simultaneously. For more information, see “Using contact and constraint detection,” Section 15.16.
You can obtain contact data for a specific surface-to-surface contact interaction by using the field and history output request editors in the Step module. In the Domain section of the editors, select Interaction and choose the name of the surface-to-surface contact interaction from the menu that appears. For more information, see “Creating an output request,” Section 14.12.1.
The procedure for defining surface-to-surface contact depends on whether you are performing an analysis using Abaqus/Standard or Abaqus/Explicit. This section provides instructions for using the interaction editor to define the different surface-to-surface contact options. The following topics are covered:
“Defining surface-to-surface contact in an Abaqus/Standard analysis”
“Defining surface-to-surface contact in an Abaqus/Explicit analysis”
Certain interaction behaviors can be defined in Abaqus/Standard only by using surface-to-surface contact; see “Contact simulation capabilities in Abaqus/Standard” in “Contact interaction analysis: overview,” Section 36.1.1 of the Abaqus Analysis User's Guide, for more information.
To define surface-to-surface contact in an Abaqus/Standard analysis:
From the main menu bar, select InteractionCreate.
Tip:
You can also create a surface-to-surface contact interaction using the 
tool in the Interaction module toolbox.
In the Create Interaction dialog box that appears, do the following:
Name the interaction. For more information about naming objects, see “Using basic dialog box components,” Section 3.2.1.
Select the step in which the interaction will be created.
Select the Surface-to-surface contact (Standard) type of interaction.
Click Continue to close the Create Interaction dialog box.
Use one of the following methods to select the master surface:
Use an existing surface to define the region. On the right side of the prompt area, click Surfaces. Select an existing surface from the Region Selection dialog box that appears, and click Continue.
Note: The default selection method is based on the selection method you most recently employed. To revert to the other method, click Select in Viewport or Surfaces on the right side of the prompt area.
Use the mouse to select a region in the viewport. (For more information, see “Selecting objects within the current viewport,” Section 6.2.) Click mouse button 2 to indicate you have finished selecting. Certain connectivity restrictions apply to contact surfaces depending on the type of contact formulation. For detailed information, see “Defining contact pairs in Abaqus/Standard,” Section 36.3.1 of the Abaqus Analysis User's Guide.
If the model contains a combination of mesh and geometry, click one of the following from the prompt area:
Click Geometry if you want to select the surface from a geometry region.
Click Mesh if you want to select the surface from a native or orphan mesh selection.
The master surface that you select becomes highlighted in red in the viewport.
Select the slave surface.
In the prompt area, select one of the following:
Select Surface if you want to select a surface.
Select Node Region if you want to select a region from which to create a contact node set.
Use one of the same methods described earlier to select the slave surface or region.
The slave surface or region that you select becomes highlighted in magenta in the viewport.
The Edit Interaction dialog box appears.
The Switch Surfaces option allows you to interchange your master and slave surface selections without having to start over. The Switch Surfaces 
icon is available only if you selected Surface in the previous step.
Choose the sliding formulation.
Choose Finite sliding to use the finite-sliding formulation, which is the most general and allows any arbitrary motion of the surfaces.
Choose Small sliding to use the small-sliding formulation, which assumes that although two bodies may undergo large motions, there will be relatively little sliding of one surface along the other.
Select the discretization method.
Select Node to surface to use the node-to-surface discretization method.
Select Surface to surface to use the surface-to-surface discretization method.
Different fields become available depending upon the combination of your sliding formulation and discretization method selections.
By default, shell and membrane thicknesses are included in contact calculations for the following combinations: Small sliding and Node to surface, Small sliding and Surface to surface, and Finite sliding and Surface to surface. You can toggle on Exclude shell/membrane element thickness to ignore shell and membrane thickness for any of these combinations.
Contact interactions using Finite sliding and Node to surface do not account for surface thickness. For more information, see “Accounting for shell and membrane thickness” in “Assigning surface properties for contact pairs in Abaqus/Standard,” Section 36.3.2 of the Abaqus Analysis User's Guide.
For contact interactions using the Node to surface discretization method, you can specify a smoothing factor in the Degree of smoothing for master surface field. For more information, see “Smoothing master surfaces for the finite-sliding, node-to-surface formulation” in “Contact formulations in Abaqus/Standard,” Section 38.1.1 of the Abaqus Analysis User's Guide.
By default, a selective scheme of supplementary contact constraints is used for the following combinations: Finite sliding and Node to surface, Small sliding and Node to surface, and Small sliding and Surface to surface. For these combinations, you can specify when to Use supplementary contact points as follows:
Choose Selectively to use a selective scheme of supplementary contact constraints.
Choose Never to forgo the use of supplementary contact constraints.
Choose Always to add supplementary contact constraints when applicable.
For contact interactions using Finite sliding and Surface to surface, you can choose the Contact tracking method.
Choose Single configuration (state) to use the state-based tracking algorithm.
Choose Two configurations (path) to use the path-based tracking algorithm.
Note: If your contact interaction uses the surface-to-surface discretization method and one or more of the surfaces in the contact interaction is an analytical rigid surface, you should choose the state-based tracking algorithm.
Specify the slave node adjustment option. For more information, see “Adjusting initial surface positions and specifying initial clearances in Abaqus/Standard contact pairs,” Section 36.3.5 of the Abaqus Analysis User's Guide, and “Defining tied contact in Abaqus/Standard,” Section 36.3.7 of the Abaqus Analysis User's Guide.
For contact interactions using the Surface to surface discretization method, you can apply a smoothing to contacting surfaces that reduces inaccuracies in contact pressures caused by mesh discretization on curved geometries. Click the Surface Smoothing tab, and select one of the following options:
Choose Do not smooth to prevent smoothing from being applied.
Choose Automatically smooth 3D geometry surfaces when applicable to apply smoothing to axisymmetric or spherical surfaces (or portions of surfaces) that are identified automatically by Abaqus/CAE. Automatic smoothing has no effect on mesh parts or two-dimensional models.
For contact interactions using the Small sliding formulation, you can specify an initial clearance between the nodes on the slave surface and the master surface. Click the Clearance tab, select a clearance type from the Initial clearance field, and enter all of the data necessary to define the clearance and contact direction. For more information, see “Defining a precise initial clearance or overclosure for small-sliding contact” in “Adjusting initial surface positions and specifying initial clearances in Abaqus/Standard contact pairs,” Section 36.3.5 of the Abaqus Analysis User's Guide.
If you specify node-to-surface discretization for your contact interaction, you can also limit bonding to slave nodes in a particular subset. Click the Bonding tab, toggle on Limit bonding to slave nodes in subset, and select a node set from the list.
You can limit bonding for either of the following:
When you want to specify a subset of initially slave nodes that should experience cohesive forces. Strain-free adjustments will be made for those nodes initially not in contact but specified in the node set. All slave nodes outside of this set (including those that are initially contacting the master surface) will experience only compressive contact forces over the course of the analysis. For more information, see “Specifying cohesive behavior properties for mechanical contact property options” in “Defining a contact interaction property,” Section 15.14.1.
When you want to identify the initially bonded region of the slave surface in a VCCT crack. The unbonded portion of the slave surface behaves as a regular contact surface. The predetermined crack surfaces are assumed to be initially partially bonded so that the crack tips can be identified explicitly during the analysis. For more information, see “Defining initially bonded crack surfaces in Abaqus/Standard” in “Crack propagation analysis,” Section 11.4.3 of the Abaqus Analysis User's Guide.
Select a contact interaction property. If desired, click 
to create the interaction property.
For more information, see “Defining a contact interaction property,” Section 15.14.1, and “Contact constraint enforcement methods in Abaqus/Standard,” Section 38.1.2 of the Abaqus Analysis User's Guide.
To specify interference fit options, click Interference Fit. Interference fit options cannot be specified in the initial step. See “Specifying interference fit options” below for more detailed instructions on entering interference fit options.
If desired, click the arrow next to the Contact controls field and select the customized contact controls to use for this interaction. Only previously created Abaqus/Standard contact controls appear in the list. For more information, see “Specifying contact controls in an Abaqus/Standard analysis,” Section 15.13.9.
To deactivate and reactivate a contact interaction in a step, toggle Active in this step. The contact interaction is active in the step in which it was created. For more information, see “Removing and reactivating contact pairs” in “Defining contact pairs in Abaqus/Standard,” Section 36.3.1 of the Abaqus Analysis User's Guide.
Click OK to create the interaction and to close the editor.
Certain interaction behaviors can be defined in Abaqus/Explicit only by using surface-to-surface contact; see “Contact simulation capabilities in Abaqus/Explicit” in “Contact interaction analysis: overview,” Section 36.1.1 of the Abaqus Analysis User's Guide, for more information.
To define surface-to-surface contact in an Abaqus/Explicit analysis:
From the main menu bar, select InteractionCreate.
Tip:
You can also create a surface-to-surface contact interaction using the tool in the Interaction module toolbox.
In the Create Interaction dialog box that appears, do the following:
Name the interaction. For more information about naming objects, see “Using basic dialog box components,” Section 3.2.1.
Select the step in which the interaction will be created.
Select the Surface-to-surface contact (Explicit) type of interaction.
Click Continue to close the Create Interaction dialog box.
Use one of the following methods to select the master surface:
Use an existing surface to define the region. On the right side of the prompt area, click Surfaces. Select an existing surface from the Region Selection dialog box that appears, and click Continue.
Note: The default selection method is based on the selection method you most recently employed. To revert to the other method, click Select in Viewport or Surfaces on the right side of the prompt area.
Use the mouse to select a region in the viewport. (For more information, see “Selecting objects within the current viewport,” Section 6.2.) Click mouse button 2 to indicate you have finished selecting. Certain connectivity restrictions apply to contact surfaces depending on the type of contact formulation. For detailed information, see “Defining contact pairs in Abaqus/Explicit,” Section 36.5.1 of the Abaqus Analysis User's Guide.
If the model contains a combination of mesh and geometry, click one of the following from the prompt area:
Click Geometry if you want to select the surface from a geometry region.
Click Mesh if you want to select the surface from a native or orphan mesh selection.
The master surface that you select becomes highlighted in red in the viewport.
Select the slave surface.
In the prompt area, select one of the following:
Select Surface if you want to select a surface.
Select Node Region if you want to select a region from which to create a contact node set.
Use one of the same methods described earlier to select the slave surface or region.
The slave surface or region that you select becomes highlighted in magenta in the viewport.
The Edit Interaction dialog box appears.
The Switch Surfaces option allows you to interchange your master and slave surface selections without having to start over. The Switch Surfaces icon is available only if you selected Surface in the previous step.
Choose the mechanical constraint formulation.
Choose Kinematic contact method to use a kinematic predictor/corrector contact algorithm.
Choose Penalty contact method to use the penalty contact algorithm.
Choose the sliding formulation.
Choose Finite sliding to use the finite-sliding formulation, which is the most general and allows any arbitrary motion of the surfaces.
Choose Small sliding to use the small-sliding formulation, which assumes that although two bodies may undergo large motions, there will be relatively little sliding of one surface along the other.
For contact interactions using the Small sliding formulation, you can specify an initial clearance between the nodes on the slave surface and the master surface. Clearance options are available only in the first general analysis step. Select a clearance type from the Initial clearance field, and enter all of the data necessary to define the clearance and contact direction. For more information, see “Specifying initial clearance values precisely” in “Adjusting initial surface positions and specifying initial clearances for contact pairs in Abaqus/Explicit,” Section 36.5.4 of the Abaqus Analysis User's Guide.
Select a contact interaction property. If desired, click to create the interaction property; see “Defining a contact interaction property,” Section 15.14.1, for more information.
Choose the weighting factor. For more information, see “Contact formulations for contact pairs in Abaqus/Explicit,” Section 38.2.2 of the Abaqus Analysis User's Guide.
If desired, click the arrow next to the Contact controls field and select the customized contact controls to use for this interaction. Only previously created Abaqus/Explicit contact controls appear in the list. For more information, see “Specifying contact controls in an Abaqus/Explicit analysis,” Section 15.13.10.
To deactivate and reactivate a contact interaction in a step, toggle Active in this step. The contact interaction is active in the step in which it was created.
Click OK to create the interaction and to close the editor.
When you are defining surface-to-surface contact for Abaqus/Standard, you can specify interference fit options that help Abaqus/Standard resolve excessive overclosure between surfaces in the initial configuration of a model. For more information, see “Modeling contact interference fits in Abaqus/Standard,” Section 36.3.4 of the Abaqus Analysis User's Guide.
To open the Interference Fit Options dialog box, click Interference Fit in the Abaqus/Standard interaction editor (see “Defining surface-to-surface contact in an Abaqus/Standard analysis” above for details).
To specify interference fit options:
In the Interference Fit Options dialog box, select Gradually remove slave node overclosure during the step to prescribe allowable intereferences.
Select one of the following options:
Select Automatic shrink fit (first general analysis step only) if you want Abaqus/Standard to assign a different allowable interference to each slave node that is equal to that node's initial penetration. If you select this option, skip to Step 6.
Select Uniform allowable interference to specify a single allowable interference that will be applied to every slave node.
Click the arrow to the right of the Amplitude field to select the name of an amplitude curve that defines the magnitude of the prescribed interference during the step. Alternatively, you can select (Ramp) to apply the prescribed interference immediately at the beginning of the step and ramp it down to zero linearly over the step.
If necessary, you can click 
to define a new amplitude curve. For more information, see “Selecting an amplitude type to define,” Section 57.3.
In the Magnitude at start of step field, enter the magnitude of the allowable interference at the start of the step.
If desired, select the Interference Direction option Along direction to specify a shift direction vector. The relative shift is applied to the slave nodes before Abaqus/Standard determines the contact conditions. If you select this option, enter the following:
In the X field, enter the X-direction cosine of the shift direction vector.
In the Y field, enter the Y-direction cosine of the shift direction vector.
In the Z field, enter the Z-direction cosine of the shift direction vector.
Click OK to save the interference fit options that you have specified and to return to the Edit Interaction dialog box.