Nonlinear Analysis:  changing contact or interference between parts of an assembly 
[Requires: contact/target elements on surfaces which may change contact, plus settings and properties for the contact surface]

Parts or bodies in a model are not related to one another unless contact behavior is defined

The user determines if contact behavior is needed for a simulation.  If so, the user specifies which surfaces can experience changing contact.

If contact behavior is defined, only surfaces of the same contact pair are monitored for closing, separating, or sliding

CONTACT ELEMENT CHOICES

• "Contact Pairs" 
• ANSYS: Contact Wizard for elements: TARGE169, 170 and CONTA171, 172, 173, 174
• point-to-point contact, ANSYS CONTA178

ANSYS contact models (element options, real constants, material properties):

• formulation: Augmented LaGrange method (default) or penalty method
• load increment control: predicting contact changes
• behavior: sliding with friction, bonded, hook, initial interference, and more
• Status: open = no stiffness, closed = stiff spring (stiffness may default or may require user specification), and near/far determination

Guidelines for Target/Contact Surface Selection:  (not needed if "symmetric" pattern is used)

• if a convex face will contact a flat or concave face, the flat or concave face should be the target surface.
• if one surface has a coarser mesh, it should be the target surface.
• if one surface is stiffer than the other, it should be the target surface.
• if one surface is higher-order and the other is lower-order, the lower-order surface should be the target surface.
• if one surface is larger, it should be the target.

ALWAYS use large deformations because contact technology was developed to work best w/large deformation effects, ON.

WHAT TO DO WHEN THE SOLUTION WON'T CONVERGE

• check the solution output and error log files for messages
• apply the load in more, smaller substeps
• allow more equilibrium iterations
• try alternative material models (bilinear vs. multilinear, different hardening rules, etc.)
• inspect the mesh in high stress regions for poor element shapes
• re-evaluate you choice of loads (get rid of point loads, overconstrained edges)
• look at the last good solution for any irregularities
• re-check EVERYTHING ! [element options, and material properties, and real constants, and load values, and dimensions]
• experiment with convergence enhancement tools in the code
• deactivate one or more of the nonlinear conditions to find the problem
• (rarely) loosen the convergence criteria - to find the problem - then tighten it up again

ANSYS Help System

Contact Technology Guide, Chapters 1 - 6, 8 - 11

Difficulties with contact problems:  Final contact is not know in advance, friction

Classification: rigid-to-flexible OR flexible-to-flexible

CH 2: The Contact Manager

Some operations of the contact manager are available ONLY in the correct processor (preprocessor, solution, or postprocessor)

Buttons: Contact Wizard, Properties, Delete, Selection Options, Plot, Show Normals, Flip Normals, Switch Contacts/Targets, List, Context, Check, Show Results

The Contact Wizard:  to assist in defining contacting surfaces and properties

CH 3: Surface-to-Surface Contact

               Use “contact pairs” of TARGE1xx with CONTA17x elements

               A “contact pair” contact and target elements share the same REAL constant ID number

Steps in a contact analysis:

1.      Create the model geometry and mesh

2.      Identify the contact pairs

Define smaller, localized contacting zones, be sure zones are adequate to capture all necessary contact

3.      Designate contact and target surfaces

a. Guidelines:

             i.  If a convex surface is expected to come into contact with a flat or concave surface, the flat/concave surface should be the target surface.

             ii.  If one surface has a fine surface mesh and, in comparison, the other has a coarse mesh, the fine mesh should be the contact surface and the coarse mesh should be the target surface.

             iii.  If one surface is stiffer than the other, the softer surface should be the contact surface and the stiffer surface should be the target surface.

             iv.  If higher-order elements underly one of the external surfaces and lower-order elements underly the other surface, the surface with the underlying higher-order elements should be the contact surface and the other surface should be the target. However, for 3-D node-to-surface contact, the lower-order elements should be the contact surface. The higher-order elements should be the target surface.

             v.  If one surface is markedly larger than the other surface, such as in the instance where one surface surrounds the other surface, the larger surface should be the target surface.

             vi.  In the case of 3-D internal beam-to-beam contact modeled by CONTA176 (a beam or pipe sliding inside another hollow beam or pipe), the inner beam should be considered the contact surface and the outer beam should be the target surface. However, when the inner beam is much stiffer than the outer beam, the inner beam can be the target surface.

b.  Asymmetric Contact vs. Symmetric Contact

               i.  Asymmetric contact has all contact elements on one surface and all target elements on the other

               ii.  Asymmetric contact is usually the most efficient way to model surface-to-surface contact

               iii.  Symmetric contact has each surface designated to be both a target and a contact surface (two sets of contact pairs for the same surfaces)

               iv.  Use symmetric contact when:

    1. It is not clear which surface should be the contact or target

    2. When both surfaces have coarse meshes

               v.  With Symmetric contact, the total contact pressure acting on both sides is the average of the contact pressures on each side of the surface

4.  Define the target surface

a.  Little info is needed for flexible-to-flexible contact

b.  For Rigid-to-flexible contact

               i.  The target face is the rigid face

               ii.  May require a “pilot node” to control the motion of the surface

               iii.  May use primitive shapes to define the rigid surface (circle, cylinder, sphere, cone)

               iv.  Arbitrary rigid target shapes can be created by constructing and meshing areas

5.  Define the contact surface

Check the “normal” direction of contact (and targets); make sure they point toward each other

6.  Set the element KEYOPTS and real constants

Real constants and element options (KEYOPTS) define the behavior of the contact pairs

7.  Define/control the motion of the target surface (rigid-to-flexible only)

8.  Apply necessary boundary conditions

9.  Define solution options, load steps (substeps, automatic time stepping, output controls, etc.)

10.  Solve the contact problem

11.  Review the results (incl. contact pressure, status, gap/penetration, sliding, etc.)

Animation of results is useful to examine intermediate results.

CH 4: NODE-to-Surface Contact

       CONTA175 (at a node on one surface) to TARGE169 or TARGE170 (on another face)

Recommended for point-to-surface or edge-to-surface problems.

Avoid midside-noded (higher-order) underlying elements of the contact surface

CH 5: 3D Beam-to-Beam Contact

CONTA176  to TARGE170 can handle internal contact (beam within another) or external contact (beams parallel or perpendicular)

CH 5: Line-to-Surface Contact

        CONTA177 (along a line on one surface) to TARGE170 (on another face)

CH 8: NODE-to-NODE Contact, CONTA178

The nodes of the two opposing surfaces must match up geometrically

The relative sliding between the two surfaces is negligible

The deflections (rotations) of the two surfaces must remain small

CH 9: Multipoint Constraints (MPC)

Element behavior option [KEYOPT(2)=2, along with KEYOPT(12) = 4, 5, or 6] of CONTA17x

To form an assembly of parts with no sliding/friction and no separation

Can be used to distribute a force evenly over a surface.

CH 10: Dynamic Contact and Impact Modeling

Transient analysis w/contact: more difficult (velocity & acceleration included, energy must be conserved)

Automatic time stepping is useful to adjust time increments near an impact event

CH 11: Spotwelds:  To model thin sheet components that are connected with spot welds, rivets, or fasteners

Can be located anywhere between the parts that are to be connected, independent of the mesh and the node locations