Component Interaction PropertyManager

You can use the Component Interaction PropertyManager to specify the interaction conditions that control the behavior of the selected components during simulations.

Component-level interactions override global-level interactions, and local interactions settings override component-level interactions. Modifying or adding an interaction setting requires remeshing the model.

Before you run the analysis, you can verify the areas of interactions (such as bonded, contact, and free) with the Interaction Viewer PropertyManager.

Interaction Type

The available options depend on the study type:

Bonded Selected components behave during simulation as if they were welded.
Contact Selected components do not interfere with each other during simulation, regardless of their initial contact condition. By default, bodies do not intersect themselves if the deformation during simulation is sufficient to cause self-intersection. Surface to surface contact formulation is applied.
The Contact interaction option for components is not available for nonlinear studies. Use the Local Interactions PropertyManager to apply local contact sets between geometric entities of selected components.
Free Selected components can intersect each other during simulation. Do not use this option unless you are sure that loads will not cause interference of the components. This interaction type overrides existing component-level interactions.
Insulated Prevents heat flow because of conduction between the selected components.

Components

  Global interaction Selects the top-level assembly to apply a global interaction condition. The selected interaction type applies to all components of the assembly.
Components for interaction Select the components to specify their interaction conditions. You can select the required components from the flyout FeatureManager design tree or from the graphics area using the Filter Solid Bodies tool on the Selection Filter toolbar.

Properties

Gap range for bonding Specifies the clearance that allows geometric entities to qualify for bonding interactions. The default value for Maximum gap percent is 0.01 % of the characteristic length of the model and is specified in Default Options > Interactions. Components that have clearances larger than this threshold are not bonded at a component-level. You can overwrite the default maximum clearance with a user-defined value.

Enter a very small value rather than zero for maximum clearance to ensure bonding of curved, coincident geometry.

You might need to increase the specified maximum gap by a small tolerance to ensure proper enforcement of bonding. To verify the areas of interactions (such as bonded, contact, and free), use the Interaction Viewer PropertyManager.
Calculate minimum gap This tool is available when you select two components in Components for interaction to apply a bonded contact.

Calculates the minimum distance between the two selected components.
Include bonding from shell edge to solid face/shell face and edge pairs (slower) Creates edge-to-edge bonded contact sets for pairs of edges located within the allowable clearance for bonding.
The valid pairs of edges of shells or sheet metal bodies that qualify for bonding are:
  • Straight, parallel, and non-interfering shell edges (or almost parallel within one degree of tolerance).
  • Circular edges that have the same radius, are concentric, and do not interfere.
  • Shell edges (straight or arc) bonded to a solid or shell face (planar or cylindrical).
Gap range to consider contact: Specifies the clearance that allows geometric entities to qualify for contact. The default value specified in Default Options > Interactions is 10 % of the characteristic length of the model.
Stabilize the area if the gap is: Applies a small stiffness to the qualified areas so the solver can overcome instability issues and start the simulation. The software applies contact stabilization to components that have an initial clearance within a threshold value of 1% of the model's characteristic length.

You can customize the allowable clearances to better fit your models.
Coefficient of friction Specifies the coefficient of static friction for the selected component. The allowable range for the friction coefficient is 0 to 1.0.

The static friction forces are calculated by multiplying the normal forces generated at the locations that come into contact by the given coefficient of friction. The direction of the friction force is opposite to the direction of motion.

Advanced

(Available for the Bonded interaction type).

Enforce common nodes between touching boundaries Enforces mesh continuity on the touching boundaries of the selected components and meshes the components as one body. Only the Curvature-based and Standard meshers support this option.
Bonding formulation Specifies the bonding formulation for components that mesh independently.

Surface to Surface

This option is more accurate, but slower. For a 2D Simplification study, the solver applies an edge-to-edge bonding.

Node to Surface

Select this option if you run into performance issues when solving models with complicated contact surfaces. For a 2D simplification analysis, the program applies a node-to-edge bonding.

Defining Component-Level Interactions

You can use component-level interactions to modify the default global interaction type for selected components, for example from a global bonded condition to a contact interaction. Component-level interactions override global-level interactions.

To specify the interaction type for selected components:

  1. In the Simulation study tree, right-click the Connections icon and select Component Interaction .
  2. In the PropertyManager, select the required interaction type, Bonded, Contact, or Free.
  3. Under Components , select the required components (parts or bodies) from the flyout FeatureManager design tree.
  4. For Contact interaction, you may specify the Friction coefficient.
  5. Click .
    An error icon appears next to the Mesh icon when you modify or add a new interaction condition after meshing. The software remeshes the model automatically before running the study.

Thermal Contact Resistance

The usefulness of the analogy between the flow of electric current and the flow of heat becomes apparent when a satisfactory description of the heat transfer at the interface of two conducting media is needed. Due to machining limitations, no two solid surfaces will ever form a perfect contact when they are pressed together. Tiny air gaps will always exist between the two contacting surfaces due to their roughness.

Through the interface between the two contacting faces, two modes of heat transfer exist. The first is conduction through points of solid-to-solid contact (Qconduction) which is very effective. Secondly, convection through the gas filled gaps (Qgap) which, due to its low thermal conductivity, can be very poor. To treat the thermal contact resistance, an interfacial conductance, hc, is placed in series with the conducting media on both sides as shown in the next figure.

The conductance hc is similar to the convection heat transfer coefficient and has the same units (W/m2 ºK). If ΔT is the temperature difference across an interface of area A, then the rate of heat transfer Q is given by Q = A hc ΔT. Using the electrical-thermal analogy, you can write Q = ΔT/Rt, where Rt is the thermal contact resistance and is given by Rt = 1/(A hc).

The interfacial conductance, hc, depends on the following factors:

  • The surface finish of the contacting faces.
  • The material of each face.
  • The pressure with which the surfaces are forced together.
  • The substance in the gaps between the two contacting faces.

The following table shows some typical values of the interfacial conductance for normal surface finishes and moderate contact pressures (1 to 10 atm). Air gaps not evacuated unless so indicated:

Thermal Resistance, RthermalX10-4 (m2.K/W)
 
Contact Pressure 100 kN/m2 10,000 kN/m2
Stainless Steel 6-25 0.7-4.0
Copper 1-10 0.1-0.5
Magnesium 1.5-3.5 0.2-0.4
Aluminum 1.5-5.0 0.2-0.4

The following table lists the thermal contact resistance for metallic interfaces under vacuum conditions:

Contacting Faces Conductance (hc) (W/m2 ºK)
Iron/aluminum 45,000
Copper/copper 10,000 - 25,000
Aluminum/aluminum 2200 - 12000
Stainless steel/stainless steel 2000 - 3700
Stainless steel/stainless steel (evacuated gaps) 200 - 1100
Ceramic/ceramic 500 - 3000

Thermal Contact Resistance - Example

In the electronic industry, chips are usually joined to substrates by a thin layer of epoxy. Similar situations are encountered in other industries. Modeling the epoxy layer as a separate component requires the use of a very small element size that can result in meshing failure or an unnecessarily large number of elements.

To consider the thermal resistance caused by the epoxy layer, you do not need to model it. Thermal contact resistance is implemented as a surface-to-surface contact condition. You can either specify the total resistivity or the resistivity per unit area.

Modeling Thermal Contact Resistance

There are two ways of modeling thermal contact resistance:
  • You can neglect the thin layer of epoxy when creating the geometry. In other words, the faces of the components that are separated by the thin layer in reality, will be touching in the model.
  • You can consider the thin epoxy layer when creating the geometry. In this case there will be a gap between the faces of thermal contact. When using this approach, there are two points to consider:
    • Results are most accurate when the distance between the two contact faces is less than or equal to the element size in the neighborhood. The below example may provide inaccurate results.

    • Splitting the faces for proper pairing of thermal contact, although not necessary, improves the accuracy.

  • To specify different thermal resistances between a large face and a number of smaller faces, you must first split the large face to a number of smaller faces before assigning thermal contact resistance for different pairs.

Defining Thermal Contact Resistance

To define thermal contact resistance:

  1. In a thermal study, right-click Connections and select Contact Set.
    The Contact Set PropertyManager appears.
  2. Set Type to Thermal Resistance.
  3. In Faces, Edges, Vertices for Set 1 , select the desired entities associated with one or more components.
  4. In Faces for Set 2 , select the desired faces from another component.
  5. Select Thermal Resistance and do the following:
    1. Set Units to the unit system you want to use.
    2. Select Total or Distributed and enter a value.
  6. Under Advanced, select Node to surface or Surface to surface.
    The Node to node option does not allow you to specify a thermal resistance as connected nodes of touching faces will have the same temperature (perfect conduction).
  7. Click .