Contact Interfaces

Use a contact interface within a component and between components when you want the contacts to have the freedom to move relative to each other but not interpenetrate each other. The contacts within a component or between components transfer forces to each other when they touch each other at a contact interface. Define a contact interface to indicate the curves or surfaces on which Creo Simulate considers the effect of load during a static analysis with contacts.

• Two individual surfaces

• An individual surface and an intent surface

• Two intent surfaces

• Between two components

• Within a component

For a component-component reference type, contacts between any two assembly components satisfying the criteria specified under Selection Filtering Tolerance are created.

Check for Contact within component—Select this check box to create contacts within components. If you do not select this check box, contacts are created between components only. This check box is not selected by default.

Use Selection Filtering Tolerance—If you select this check box, contacts are created only between two components that satisfy the following selection filtering criteria:

• Separation Distance—Specifies the value for the separation distance or accepts the default value which is close to 1% of the model size. The separation distance is the maximum distance between the surface pairs that you want to use to define a contact. You can select length units for separation distance from the adjacent drop-down list or accept the default units.

• Angle (between planar surfaces)—Specifies an angle or accepts the default value of 5 degrees to automatically detect the surfaces for contact definition. You can specify a value in the range of 0 to 45 degrees. You can only check the planar surfaces with the angle control.

• Check for Contact only between planar surfaces—Creates contacts only between planar surfaces.

• Override Model Contact Penetration—Allows you to specify the percent value of Contact Penetration for an interface. You can specify values from 1 to 100.

• Split Surfaces—Splits the surfaces in contact along the boundaries. This check box is cleared by default.

• Generate Compatible Mesh—Creates a compatible mesh for the surfaces in contact. Creo Simulate creates geometrically consistent node locations when it generates the mesh for the surfaces of your interface. This check box is selected by default in Native mode. It is available for selection, when you split surfaces in the contact. In FEM mode, when you split surfaces in the contact, by default Creo Simulate creates a compatible mesh for the surfaces.

If the two surfaces in contact cannot be split, for example, a cylindrical and a planar surface, the Split Surfaces check box is not available. You cannot generate a compatible mesh for such surfaces.

When you create a contact interface in a version prior to Pro/Engineer Wildfire 3.0, the surfaces in the contact are split by default in Pro/Engineer Wildfire 4.0 and later releases if they are compatible and coincident.

• Friction—Specifies the friction at the contact interface.

◦ Finite—Creates a contact with finite friction. Two components or surfaces with a finite friction contact interface between them will slip relative to each other if and only if the tangential traction between them exceeds the coefficient of friction times the normal force.

◦ None—Creates a frictionless interface. Two components with a frictionless contact interface between them will slip relative to each whenever there is a tangential traction between them.

• Create Slippage Indicators—Creates three slippage indicator measures. It is available for selection only if you select the Infinite option for friction. All the slippage measures are created automatically. For a frictionless interface, no slippage measures are created.

These measures check if slippage occurred in the contact region during a static analysis with contacts. If any of the slippage indicator measure values is positive during a static analysis with contacts, a warning appears in the summary report (.rpt file). This warning indicates that the surfaces in contact may have slipped relative to each other. In this case the assumption of infinite friction is inaccurate.

• Static Coefficient of Friction—Specifies the ratio of the tangential stress to the normal stress at a contact. Above this value, sliding occurs. For finite friction, it is used during a static analysis to determine when slippage occurs. For both finite and infinite friction it is used in computing the slippage indicator measures. If friction type is infinite and you want to compute slippage indicators, you must select the Create Slippage Indicators check box and specify a positive value for the static coefficient of friction. If the friction type is infinite, then the coefficient of friction is used only for computing the slippage indicators and does not affect the displacements or stresses near the contact interface.

• Dynamic Coefficient of Friction—Specifies the ratio of the tangential stress to the normal stress at a contact that was previously sliding, above which value sliding continues. You can specify this value only for an interface with finite friction. You must also clear the Same as static check box for this field to be available. The value of the dynamic coefficient of friction must be less than or equal to the value of the static coefficient of friction.

• Same as static—Equates the value of the static and dynamic coefficients of friction. You can clear or select this check box only for an interface with finite friction.

• Detailed Stresses—This area is available only when you select Finite as the type of friction at the contact interface.

Override Analysis Settings—Overrides the Calculate detailed stresses at contact interfaces setting on the Convergence tab of the Analysis dialog box. Select Override Analysis Settings as well as the Calculate check box if you want the application to calculate detailed stresses for the interface.

Creo Simulate also creates a measure for maximum tangential traction, when you select Finite or Infinite friction. Interface force and area measures are also calculated.

You can automatically create one or more contacts between selected components or surfaces. Click Refine Model and then click the arrow next to

Interface. Click Detect Contacts and specify the separation distance and the angle between the surfaces on which you want Creo Simulate to automatically create one or more contacts. All the suitable surfaces in the model are first detected and then one or more contacts are created. Additionally, you can choose to create contacts only between planar surfaces.