You can use the Contact Wizard to create a contact pair for either rigid-to-flexible or flexible-to-flexible contact. In addition, you can use the wizard to create contact pairs for surface-based constraints. As you progress through the various dialog boxes in the wizard, remember that the contact pair isn't actually created until you complete all of the requirements and click the button. At any point before you click , you can click the button to abort the process. You can also return to previous dialog boxes (and change your settings) by clicking the button.
Contact Wizard: Select Target
Use this dialog box to define the target surface.
- Target Surface:
Select the Target Surface type.
- Target Type:
Select the Target Type. For rigid-to-flexible contact, the target surface must be either Rigid or Rigid w/ Pilot (with a pilot node). For a surface-based constraint (force-distributed or rigid constraint), you must use the Pilot Node Only option.
- Pick Target ...
Click this to launch the target picker. Pick the target surface or nodes and then click to return to this dialog. For rigid-to-flexible analysis, the picker will only let you select unmeshed surfaces or nodes as the target.
After you have selected the target surface and its parameters, click to continue.
Contact Wizard: Define Pilot Node
Use this dialog box to define the pilot node for a rigid-to-flexible contact pair or surface-based constraint.
- Pilot Name:
(Optional) You can specify a name for a nodal component that will contain the pilot node. This allows easier interaction with the pilot node later on.
You can define the pilot node in several ways.
Allow the program to automatically define the pilot node at the centroid of selected geometric entities (keypoints, lines, or areas). Target entities are considered for rigid-to-flexible contact, and contact entities are considered for a surface-based constraint.
Pick an existing keypoint, node, or working plane location.
Type in coordinates in the active coordinate system.
Click this to launch the pilot node location picker. Pick the keypoint, node, or working plane location and then click to return to this dialog. Only one entity or location is allowed.
After you have selected the pilot node, click to continue.
Contact Wizard: Select Contact
Use this dialog box to define the contact surface.
- Contact Surface:
Select the Contact Surface type.
For 2D analysis this can be keypoints (node-to-surface contact only), lines, body (areas), nodes, or nodal components.
For 3D analysis this can be lines (node-to-surface contact only), areas, body (volumes), nodes, or nodal components.
This option determines the specific element type that will be used. For Surface-to-Surface contact, CONTA172 (2–D) or CONTA174 (3D) will be used as the contact element type. For Node-to-Surface contact, CONTA175 will be used (2D or 3D).
Click this to launch the contact picker. Pick the keypoints, lines, surface, or nodes and then click to return to this dialog. Note that in a 2D analysis, only lines and keypoints that are part of areas are valid selections and, therefore, only these are shown.
After you have selected the contact surface and its parameters, click to continue.
Contact Wizard: Set Parameters and Create
Flexible-to-Flexible or Rigid-to-Flexible Contact Pair
Use this dialog box to specify parameters for your contact analysis and create the contact pair. This dialog provides some of the most commonly used parameters. The button lets you select additional parameters.
The Contact Wizard automatically detects which degrees of freedom are active in your model (based on element type):
If only structural degrees of freedom are detected, thermal, electric, and magnetic options for contact are ignored and KEYOPT(1) is set to 0.
If structural and thermal degrees of freedom are detected, electric and magnetic contact options are ignored and KEYOPT(1) is set to 1.
If only the thermal degree of freedom is detected, thermal options are available and KEYOPT(1) is set to 2. Heat generation due to friction is ignored.
If structural, thermal, and electric degrees of freedom are detected, all contact options except magnetic are available and KEYOPT(1) is set to 3.
If thermal and electric degrees of freedom are detected, all structural and magnetic contact options are ignored and KEYOPT(1) is set to 4.
If structural and electric degrees of freedom are detected, all thermal and magnetic options are ignored and KEYOPT(1) is set to 5.
If only the electric degree of freedom is detected, electric options are available and KEYOPT(1) is set to 6.
If only the magnetic degree of freedom is detected, magnetic options are available and KEYOPT(1) is set to 7.
- Create symmetric pair
When on, two companion (symmetric) contact pairs will be created instead of a single pair. The contact surface of each pair is identical to the target surface of its companion pair, and vice versa. Although they will use different real constant and element type IDs, both pairs will have the same settings. This symmetric pair capability is applicable to flexible-to-flexible contact only.
- Include initial penetration
When on, initial penetration includes the geometrical penetration. When off, initial penetration is excluded.
- Friction:
Select the material ID and then set the coefficient of friction (any non-negative value). You can use this to create a new material ID. Also, a coefficient of friction value entered here will overwrite any previously entered value.
Only isotropic friction can be defined through the Contact Wizard. For a detailed description of the friction model and information on how to define orthotropic friction (available for 3D contact only), see Choosing a Friction Model.
- Thermal Contact Conductance:
For a thermal analysis, input the thermal conductance between the two contacting surfaces. You can input a constant value or a table. The drop-down list box lists all tables that have been defined.
- Electric Contact Conductance:
For an electric current conduction analysis, input the electrical conductance between two contacting surfaces if KEYOPT(1) = 3 or 4, or input the electrical capacitance per unit area between two contacting surfaces for piezoelectric (KEYOPT(1) = 5) or electrostatic (KEYOPT(1) = 6) analyses. You can input a constant value or a table. The drop-down list box lists all the tables that have been defined.
- Magnetic Contact Permeance:
For a magnetic field analysis, input the magnetic permeance at the contact interface. You can input a constant value or a table. The drop-down list box lists all the tables that have been defined.
This button launches the Contact Parameters dialog box. These settings provide a finer degree of control over your contact analysis.
Click this button to create the contact pair.
Contact Wizard: Set Parameters and Create
Surface-based Constraint Contact Pair (Pilot Node Only)
Use this dialog box to specify parameters for your analysis and create the contact pair that will support a surface-based constraint.
- Constraint Surface Type:
The constraint surface type is either Rigid Constraint or Force-distributed Constraint. See Surface-based Constraints for more information.
The boundary conditions on the pilot node (target) can be either user-specified or set automatically based on the dimensionality of the model.
Only checked degrees of freedom will be constrained according to the constraint surface type. The button sets all available degrees of freedom to be included in the constrained DOF set.
Click this button to create the contact pair.
Flip Normals
This dialog box indicates that the contact pair was created and lists the real set ID for the contact pair. At this point, you should check the normals for the contact pair.
The node order of the target surface elements is critical because it defines contact direction. For 2D contact, the associated contact elements must lie to the right of the target surface when moving from the first node to the second node along the target surface line.
For 3D contact, the target element numbering should be such that the surface's outward normal points toward the contact surface. The outward normal is determined by the right-hand rule.
If the element normals do not point toward the contact surface, click to reverse the direction of the surface normals. Click when you have verified that the direction of the normals is correct.
Finish
This dialog box indicates that the contact pair was created and lists the real set ID for the contact pair. Each contact pair is identified via the same real constant number.