For guidelines on using different contact
types, click here.Use the Contact Set PropertyManager to define contact between source and target entities for assembly documents and multibody part documents. You define two sets of entities. The target entities can be faces (of solids or shells) only. In general, the source entities can be faces, edges, and vertices except for the Node to Node option which allows faces only for the source. Entities in the source and target sets may not belong to the same component, body, or shell (self contact is not allowed). You can apply multiple contact conditions to override the global contact setting by adding component contact and local contact sets.
The Contact Set PropertyManager is the only way to define interaction between solids and shells in a mixed mesh study.
For guidelines on using different contact
types, click here.
Type. Sets the type of contact between the source and target entities. The available options depend on the type of the study:
No Penetration. Available for static, drop test, and nonlinear studies only. This contact type prevents interference between source and target entities but allows gaps to form. This is the most time-consuming option to solve.
Bonded. Available for all types of studies that require meshing. The program bonds the source and target entities. The entities may be touching or within a small distance from each other. The program issues an error message if the distance between bonded entities is larger than the average element size of the associated elements. Only source and target entities are required to define this contact type.
For drop test studies, you
can only bond touching faces.
For mixed mesh studies, you can bond source entities (vertices, edges, and faces) to target faces. The source and target entities can belong to shells or solids. The behavior of the bond depends on whether the source entity belongs to a solid or a shell. If the source entity belongs to a shell, the bond acts like a rigid connection where the original angle between the shell and the solid is maintained during deformation. If the source entity belongs to a solid, the bond acts like a hinge, where the original angle between the shell and the solid is not necessarily maintained.
When bonding a shell edge
to a solid or shell target face, the software rigidly bonds each node
of the edge to the nearest element's face on the target. The rigidity
of the connection depends on the element size near the interface. To improve
accuracy, the element size on the target face should be equal to
the thickness of the shell if no weld is used. If a weld is used, the
element size on the target face should be equal to the weld size.
Shrink Fit. Available for static and nonlinear studies only. You select faces from two components that are initially interfering with each other. Click Tools, Interference Detection to make sure that the faces are interfering.
Free (No Interaction). Available for static, nonlinear, frequency, buckling, and drop test studies. The program treats source and target faces as disjointed. For static and nonlinear studies, the loads are allowed to cause interference between parts. Using this option can save solution time if the applied loads do not cause interference. Do NOT use this option unless you are sure that loads will not cause interference. Plot the deformed shape with a scale factor of 1.0 to check for interference. Only source and target entities are required to define this contact type.
Virtual Wall. Available for static studies only. This contact type defines contact between the source entities and a virtual wall defined by a target plane. The target plane may be rigid or flexible. You can define friction between the source and the target plane by assigning a non-zero value for the friction coefficient.
Insulated. Available for thermal studies only. This option is similar to the Free (No Interaction) option for structural studies. The program treats source and target faces as disjointed. The program prevents heat flow due to conduction through the source and target entities.
Thermal Resistance. Available for thermal studies only. This option allows you to specify thermal resistance between source and target faces.
Entities for
Source 
. Select vertices, edges, and/or faces for
source.
Entities for
Target 
. Select faces for target.
Options
Node to Node. Require compatible source and target meshes. Available for touching source and target faces only.
Node to Surface. Does not require compatible source and target meshes.
Surface to Surface. Does not require compatible source and target meshes.
Friction. Specify a value for the Friction
Coefficient 
for use with No
Penetration contact for static, nonlinear, and drop test studies.
You can specify values up to 1.0. This local value overrides the global
friction coefficient specified in the Static
dialog box for static studies. For nonlinear studies, the default coefficient
is 0.05.
Gap (clearance). Set the condition for ignoring clearances. Used with Node to Surface and Surface to Surface options for No penetration and Virtual wall contact for static studies only. This local setting overrides the global setting specified in the Static dialog box.
Always ignore clearance. Ignore clearance regardless of the gap.
Ignore clearance if: Allows you to set a maximum value for the clearance to be ignored.
Thermal Resistance. Used with the Thermal Resistance option to define the thermal resistance.
Units 
. Select the unit system. You can specify the total or distributed
resistance value.
Total. Type the value of the total thermal resistance between the source and target entities.
Distributed. Type the value of the resistance per unit contact area.
Wall Type. Used with Virtual Wall contact to specify parameters of wall stiffness.
Rigid. Sets the wall type to rigid.
Flexible. Sets the wall type to flexible.
Wall Stiffness. Used to specify parameters for a Flexible wall type.
Units
. Select the unit system you want to use to enter
the wall stiffness values.
Axial
Stiffness 
. Sets the value of the wall axial stiffness.
Shear
Stiffness 
. Sets the value of the wall shear stiffness.
To define a contact set:
In the COSMOS AnalysisManager tree, right-click Contact/Gaps and select Define Contact Set.
The Contact Set PropertyManager appears.
Under Type, select a contact type.
Select the source and target entities.
Define parameters relevant to the contact type that you selected.
To include friction , select Include Friction and type the value of the Friction Coefficient.
Click 
.
Use the Find
Contact Sets PropertyManager to find and define contact sets between
faces that are touching or within a specified distance from each other.