Tie Surface (Abaqus)

When you are working with Abaqus as your solver, you can use the Tie Surface command to tie two separate surfaces together so there is no relative motion between them. You can use Tie Surface to make the translational and rotational motion equal for a pair of surfaces. You can use Tie Surface to tie selected surfaces even if the meshes on those surfaces are dissimilar.

Defining the master and slave surfaces in a tie constraint

With Tie Surface, you use simulation Regions to define the master and slave surfaces in the tie constraint. In Abaqus, you can use either an element-based surface or node-based surface as the master or slave surface. When you create a region to use in a Tie Surface definition, you can select either Node or Element from the Surface Definition Type list in the New Region dialog box.

The characteristics of the tie formulation depend on whether you create the Tie Surface constraint on node-based or element-based master and slave surfaces.

Selecting the appropriate tie formulation

You use the Tie Formulation list in the Options group of the Tie Surface dialog box to specify the tie formulation Abaqus uses to create the constraint.

• With the Surface to Surface formulation, Abaqus generates the tie coefficients such that stress accuracy is optimized for the surface pairs. Generally, the Surface to Surface formulation avoids stress noise at tied interfaces.Note: If you select the Surface to Surface formulation, you should use element-based regions to define the master and slave surfaces in the tie constraint. If you use a node-based region to define either the master or the slave surface, Abaqus uses the Node to Surface formulation instead.

• With the Node to Surface formulation, Abaqus generates the tie coefficients according to interpolation functions at the points where slave nodes project onto the master surface. With the Node to Surface formulation, master surfaces must not contain any complex intersections, such as T-type intersections.

For more information, see:

• Tie Surface dialog box (Abaqus)

• Defining the surfaces to be constrained in the Mesh Tie Constraints article in the Abaqus Analysis User's Guide.

• The surface-based tie constraint formulation in the Mesh Tie Constraints article in the Abaqus Analysis User's Guide.

Adjusting the surfaces

The Adjust option in the Tie Surface dialog box controls whether Abaqus automatically repositions the nodes on the slave surface to be tied in the initial configuration. Abaqus accomplishes this without causing strain to resolve gaps such that the surfaces are just touching. Abaqus performs all adjustments such that the master and slave surfaces are never pushed apart; they only come closer together as a result of the adjustments.

In general, you should allow the automatic adjustments to occur, especially if neither the master nor the slave surface has rotations. For more information see Adjusting the surfaces and considering offsets in the Mesh Tie Constraints article in the Abaqus Analysis User's Guide.

Associated Abaqus keywords

When you export or solve your model, the software uses the options you specify in the Tie Surface dialog box to define the *TIE keyword in your Abaqus input file. For more information, see Mesh tie constraints in the Abaqus Analysis User's Guide and *TIE in the Abaqus Keywords Reference Guide.

Where do I find it?

Application	Pre/Post
Prerequisites	A Simulation file as the work part and displayed part and an active solutionAbaqus as the specified solver Structural or Thermal(Optional) Cyclic symmetric modeling object
Command Finder	Tie Surface
Simulation Navigator	Under the active solution, right-click Simulation Objects→New Simulation Object→Tie Surface

Learn more

Contact and glue overview (Abaqus)

Comparison of general contact and contact pair (Abaqus)

Contact with Clearance (Abaqus)

Bolt Contact with Clearance (Abaqus)

Surface Based Coupling (Abaqus)

Modeling cohesive behavior in Abaqus contact analyses

Defining damage modeling for Abaqus cohesive behavior

Removing elements and contact pairs (Abaqus)

Automatic face pairing

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Tie Surface (Abaqus), Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });