Surface-to-Surface Contact

In order for loads to be transferred between elements, the nodes typically are connected together. For example, nodes can either be directly bonded, or they can be connected by multipoint constraint (MPC) equations or 1D elements. Consider two bodies that begin an analysis separated. Additionally, assume that you have not defined any means of connecting them. No interaction occurs during the analysis, and the bodies can pass through each other.

In linear analyses, surface contact is achieved by connecting nodes on adjacent parts with 1D gap or contact elements. In nonlinear analyses, general surface-to-surface contact is defined between parts or surfaces. The solver keeps track of the motion of the contact surfaces and produces resistive forces when the surfaces move together. Complex algorithms determine the contact stiffness and attempt to minimize contact chatter and surface penetration.

You can define surface-to-surface contact in Mechanical Event Simulation and other nonlinear stress analyses, but not for Natural Frequency (Modal) with Nonlinear Material Models. Create surface-to-surface contact pairs when surfaces might come into contact with each other during the analysis or when they are initially in contact but are free to slide or separate. The processor determines the distance between the nodes on one surface and the element faces on the adjacent surface. The distance is evaluated for each time step of the analysis. When the nodes are sufficiently close to each other to indicate surface interaction, a force is applied to prevent penetration.

Before you start a contact analysis, you must clearly identify where the contact interaction might occur during the analysis. (Although possible, it is very inefficient to define every surface of every part as contacting every surface of every other part.) Not only can multiple target surfaces interact with one master surface, but self-contact is also possible in large deformation problems. A part can deform enough that it contacts itself (such as the folds of rubber bellows when they are closed during axial compression of the bellows). In such cases, the user must define multiple contact pairs that cover all potential contact interaction.

The contact pairs can consist of any two arbitrary surfaces. Surface-to-surface contact produces interaction between the nodes on one surface and the element faces of the other surface (and optionally, vice versa). However, to speed up the contact search, the user should only specify the contact pairs that will definitely interact within the given event duration. The analysis converges more rapidly if the number of potential contact elements is minimized, especially in problems that involve small areas of sliding contact.

Tip: When a contact area consists of multiple surfaces (such as the many surfaces on a set of gear teeth), you can combine them by creating a Selection Group. Then, define contact pairs between selection groups or between one surface and a selection group. This technique is much more convenient than defining dozens of individual surface contact pairs. It is also more efficient for the solver than part-to-part contact because it limits contact consideration to specific surfaces and ignores the rest of the part surfaces.

You must take special care when working with hand-built models. To define where contact can occur, assign a unique surface number attribute to the lines along the surfaces that will come into contact. When an element face is bounded by lines of different surface numbers, a voting rule is used to determine which surface number applies to the face. To determine which of the six possible faces of a brick element are in contact, the solver checks the surface number of each line comprising the element. Each face that has a majority of boundary lines on the highest surface number (3 of 4 lines, or 2 of 3 lines) can participate in contact. Faces whose lines are not on the highest surface number of the element cannot participate in contact. Therefore, majority lines along the contact face should have the highest surface number of any of the lines comprising the elements that come into contact.

For CAD-based solid meshes, all interior mesh lines are on surface 0 (zero). Therefore, the outer (contact) surfaces are always on higher surface numbers than the other element faces, except perhaps at exterior corners, where two or more faces of a brick are on exterior surfaces. In addition, the CAD surface numbers are used to identify the contact faces, rather than the surface attributes of the individual lines around each face. Therefore, you need not be concerned about the voting rule when working with CAD-based meshes (assuming that you have not manually modified the mesh).

If you modify the mesh of a CAD-based model (such as by reassigning surface number attributes of lines or moving nodes), then the CAD surface numbers are no longer used. The CAD surface data is deemed no longer reliable, and the voting rule is used instead. In other words, modified CAD-based meshes are treated like hand-built models. For this reason, you will see a pop-up warning when attempting to modify CAD-based meshes.

For some cases, it is difficult for the user to predict the relative motion of contact pairs, and large potential contact regions must be considered. The processor provides an automatic updating scheme to improve the efficiency of such solutions. However, a large amount of memory may still be needed to keep track of the full set of potential contact regions in a 3D analysis. If the necessary memory is not available, the user must split large contact surfaces into several smaller contact surfaces.

Apply Surface-to-Surface Contact

Since it may not be possible to calculate the contact between some element types and others, the Element Type and Element Definition in the browser (tree view) should be defined before applying surface-to-surface contact.

Use the following method to define surface-to-surface contact pairs in nonlinear analyses:

1. Select two entities as the basis of the contact pair. The following combinations are supported:
   • Two surfaces
   • Two parts
   • One part and one surface (must be selected in the browser; in-canvas selection of mixed types is not possible)
   • Two selection groups (groups must consist of parts or surfaces)
   • One surface and one selection group (consisting of parts or surfaces)
   • One part and one selection group (consisting of parts or surfaces)
2. Right-click and select one of the following options, depending upon the context menu that appears:
   • Contact Surface Contact
   • Surface Contact
     Note: When the contact pair consists of a mixture of parts and surfaces, the only possible action is to set the type of contact. Therefore, the context menu that appears when you right-click shows the contact options directly, rather than in a fly-out submenu.
3. A new contact pair heading appears in the browser, and the default name of the new pair is currently selected for editing. You can type an alternative name if desired. Press Enter to accept the name of the contact pair.
   Note: If you click anywhere in the display area or browser, the contact pair heading is accepted and the edit mode is terminated. This action is equivalent to pressing Enter.
4. You can set the contact details by right-clicking the contact pair heading just created in the browser and choosing Edit Settings from the context menu. The settings are described in the Surface Contact Settings topic and its subtopics.
   Important: The first part, surface, or selection group you select becomes the primary member of the contact pair. The second selection becomes the secondary contact member. The selection order is important when the Contact type is Point to Surface. You can explicitly define this type of contact, or the processor may choose Point to Surface as the appropriate type, based on the geometry, when you specify the Automatic contact type. (Automatic is the default setting). Point to Surface contact detects when a node on the secondary member penetrates a face on the primary member. Conversely, primary nodes are allowed to pass through secondary faces. See Figure 1 on the Simulation Mechanical Surface Contact Options (Nonlinear) page.
   Tip: You can switch the order of the contact entities after the pair is created. Select the contact pair heading and choose Flip Primary and Secondary from the context menu. Be aware that, if you have overridden the default name of the contact pair, the heading in the browser will not change to reflect that the two parts/surfaces have been switched.

Note: You can right-click the Contact (Default:) heading in the browser and select one of three options—Bonded, Welded, or Free/No Contact. You cannot define surface contact as the default contact type. You must explicitly define surface contact pairs in nonlinear analyses.

• For solutions run using the native SimMech solver, the Bonded and Welded contact options are only applicable to parts with matched meshes where they meet. To bond unmatched meshes in a nonlinear analysis, create a Surface Contact pair and set the Contact method to Tied contact.
• For solutions run using the Nastran solver, the Bonded and Welded contact options are equivalent. Both options result in one of the following Nastran cards:
  • CONTACTGENERATE card (for the default contact definition), which supports two Nastran contact types—Welded Contact and Offset Weld contact. Note that both of these types are symmetric because the master and slave surfaces cannot be defined for the default contact definition.
  • BSCONP card (for explicitly defined contact pairs, which supports four Nastran contact types—Welded (symmetric), Welded (unsymmetric), Offset weld (symmetric), or Offset weld (unsymmetric).

  The meshes do not have to match when using the Nastran solver.