Guidelines on Studies with Contact Conditions
General
The following are general guidelines for specifying contact conditions:
Check the interference between components before
meshing. To detect interference in an assembly, click Tools,
Interference Detection. Interference
is allowed only when using shrink fit. The Treat
coincidence as interference option allows you to detect touching
areas. These are the only areas affected by the global and component contact
settings.
For local contact, use Contact
Set to define the connection between solids, shells, and beams.
The Find contact
sets PropertyManager helps you find and define contact pairs between
solids without having to select faces manually.
If you do not specify any contact conditions,
the software assumes that all parts are bonded at their initially touching entities. All other entities
are free.
Specify global, component, and local contact conditions
efficiently to define the problem. Note that for global and component
contact, you do not select specific entities since they apply only to
initially touching areas. Use global contact to define the most common
desired condition and then override it by specifying component and local
contact wherever needed.
You must remesh the study after editing or defining
contact conditions.
Bonding
Bonding ensures the continuity of the model to
transfer loads between two entities. You can bond a face or an edge to
any other face or edge. The meshes of the bonded entities do not have
to be compatible. Use Contact Set
to define bonding conditions between solids, shells, and beams.
Bonding with compatible mesh gives better results
but can cause meshing to fail for some assemblies. Using the Remesh failed parts with incompatible mesh
can help mesh such assemblies.
The entities do not have to be touching. The program
gives a message when trying to bond entities that are too far apart. The
software allows you to bond slightly interfering entities.
Bonding is achieved by merging nodes when the
mesh is compatible or by using multi-point restraints internally when
the mesh is not compatible. Bonding incompatible meshes can generate local
stress concentrations in the bonded areas.
When bonding solid faces through the global contact
condition, the program generates a compatible mesh on the touching areas
and merges the nodes.
See Automatic
Bonding Between Touching Entities.
If the cylinder is
connected to the plate by welding its edge only, then set the global contact
to Free and then bond the face
of the plate to the edge of the cylinder by defining a local contact set.
If a small clearance
exists, the global contact settings are irrelevant but you can use the
local Contact
Set PropertyManager to bond the cylinder's face or edges to
the plate.
Static and Nonlinear Studies
Contact is a common source of nonlinearity. Although
nonlinear studies are naturally used to solve contact problems, the software
allows you to use static studies to solve contact problems with small
and large displacements.
The properties dialog of static
and nonlinear
studies provide an option to use large displacements. Use the small displacement
formulation only if the expected motions are small and the parts are independently
stable in directions other than the primary contact direction.
NOTE:
The program automatically detects when large displacements occur and prompts
you. On selecting Yes, the simulation
is automatically rerun by activating the large
displacement flag. On selecting No,
the simulation results are displayed with small displacement formulation
even though they could be inaccurate.
Note the following limitations when using static
studies to solve contact problems with large displacements:
The results will be available only at the
last solution step. In nonlinear studies, you can get results at every
solution step.
If a nonlinearity other than that caused by
contact is present, you cannot use static studies. Common sources of nonlinearity
are material properties and changing loads and restraints.
Use the Shrink
Fit option of local contact to define shrink fit contact condition
between initially interfering components.
You can use surface to
surface or node to surface to replace node to node contact. However, using
node to node can save you time and give you similar results if the loading
does not cause relative sliding of the contacting areas.
In general, using the
surface to surface contact with the No
penetration option is more accurate than using the node to surface
option. However, it takes longer to solve and may not converge when the
contact area becomes too small. In such cases, use the node to surface
option.
Thermal Studies
The Bonded,
Thermal resistance, and Insulated contact conditions are available.
Free faces (faces without any boundary conditions) are insulated. A free
face is thermally similar to a face with a zero temperature gradient in
the normal direction. Faces of thermal symmetry can be modeled as free
faces. Heat can flow parallel to the face but cannot flow normal to it.
The node to node option does not allow you to
specify thermal
resistance as the connected nodes will have the same temperature
(perfect conduction). Use surface to surface contact to simulate thermal
resistance.
Buckling Studies
Only the
Bonded and Free options
are available.
Frequency Studies
Only the Bonded
and Free options are available.
Use caution when specifying the Free
option and interpreting results associated with it as the parts
are considered disjointed. Since there is no real amplitude associated
with frequency results, we recommend that you run frequency analysis independently
on isolated parts by creating a study in the part document. You can also
run frequency analysis on connected subassemblies independently.
Linear Dynamic Studies
The Bonded
and Free options are available
for all linear dynamic study types.
Drop Test Studies
The Bonded,
Free, and No
penetration options are available. Only the node to surface option
is available for No penetration.
Related Topics
Node
to Node Contact
Node
to Surface Contact
Surface
to Surface Contact