The target surface can be 2-D or 3-D and either rigid or deformable. For deformable target surfaces, you will normally use the ESURF command to generate the target elements along the boundaries of an existing mesh. You can follow the same method to generate the deformable contact surface (see Defining the Deformable Contact Surface for details). If you are modeling 3-D line-to-line contact and the underlying elements are a part of shell edges, issue ESURF,,,LINE to generate 3-D line or parabola segments along the shell edges.
You should not use the following rigid target segments for a deformable target surface: ARC, CARC, CIRC, CYL1, CONE, SPHE, POINT, or PILO. For rigid target surfaces, the following provides general guidelines.
In 2-D cases, the shape of the target surface is described by a sequence of straight lines, circular arcs, and parabolas, all of which can be represented with the target segment element TARGE169. You can use any combination to define the complex target surface geometry. In 3-D cases, the shape of the target surfaces is described by a sequence of triangles, quadrilaterals, straight lines, parabolas, cylinders, cones, and spheres, which can be represented with TARGE170. You can use any reasonable combination of low/high-order triangles and quadrilaterals to model a target surface with a complex, arbitrary geometry.
The rigid target surface can also be associated with a "pilot node," which is really an element with one node, whose motion governs the motion of the entire target surface. You can think of a pilot node as a handle for the rigid target surface. Forces/moments or rotations/displacements for the entire target surface usually should be prescribed on the pilot node. The pilot node can be one of the nodes on the target element or a node at any arbitrary location. The location of the pilot node is important only when rotation or moment loading is required.
You can use circle, cylinder, cone, and sphere primitives to model the target (which require real constants to define the radius). You can combine primitive segments with general segments (such as lines, parabolas, triangles, and quadrilaterals) to define a target surface. Primitives cannot be defined directly in the Contact Wizard. The primitives do not support MPC based bonded or no-separation contact.
|GUI:||Main Menu> Preprocessor> Element Type> Add/Edit/Delete|
You define characteristics of the target element geometry through real constants R1 and R2 as follows:
R1 is the radius if the target shape (TARGE169) is a circle.
R2 is the element thickness if the underlying element is a superelement set as plane stress with thickness (KEYOPT(3) = 3). The default value is 1.
R1 is the radius if the target shape (TARGE170) is a cylinder, cone, or sphere.
R2 is the radius of a cone at the second node.
For CONTA176, used to model 3-D beam-to-beam contact:
R1 is the radius of circular beams on the target side (target radius). Use a positive value when modeling external beam-to-beam contact. Use a negative value to represent the inner radius of the outer beam (or pipe) when modeling internal beam-to-beam contact.
R2 is the radius of circular beams on the contact side (contact radius). Use a positive value for both external and internal beam-to-beam contact.
To set the real constant number for the target elements:
|GUI:||Main Menu> Preprocessor> Real Constants|
For TARGE169 and TARGE170, you need only set real constants R1 and R2 (if required). For a complete description of the target elements, element shapes, and real constants, see the description of TARGE169 and TARGE170 in the Element Reference.
Specifying real constants (R1, R2) manually is necessary only if you use direct generation to create your target elements, or if you model 3-D beam-to-beam contact with CONTA176. You can also use the ANSYS meshing tools to create the elements, or use the Contact Manager Toolbar.
To generate target elements directly, use the following command or GUI path:
|GUI:||Main Menu> Preprocessor> Modeling> Create> Elements> Elem Attributes|
You then specify the element shape. Possible shapes are:
Straight line (2-D and 3-D)
Parabola (2-D and 3-D)
Clockwise arc (2-D)
Counterclockwise arc (2-D)
Three-node triangle (3-D)
Six-node triangle (3-D)
Four-node quadrilateral (3-D)
Eight-node quadrilateral (3-D)
Point (2-D or 3-D)
Pilot node (2-D and 3-D)
Once you specify a target element shape, all subsequent elements will have that shape until you specify another shape.
You cannot mix 2-D and 3-D target elements on the same target surface.
You cannot mix rigid target elements with deformable target elements on the same target surface. During solution, ANSYS assigns a deformable status to target elements with underlying elements and assigns a rigid status to target elements without underlying elements. If a portion of the underlying elements of a deformable surface are deleted, an error will occur in solution.
You can generate the nodes and elements using standard ANSYS direct generation techniques. For more information on direct generation modeling techniques, see "Direct Generation" in the Modeling and Meshing Guide.
You can then verify your element shapes by listing the elements.
|GUI:||Utility Menu> List> Elements> Nodes + Attributes|
You can also let ANSYS generate the elements automatically using the standard ANSYS meshing capabilities. ANSYS will recognize the proper target element shape based on the solid model and will ignore the TSHAP setting.
To generate a pilot node, use the following command or GUI path:
|GUI:||Main Menu> Preprocessor> Meshing> Mesh> Keypoints|
KMESH always creates pilot nodes.
To generate POINT segments, use the Direct Generation method or use ESURF,,,POINT command on selected nodes.
To generate 2-D rigid target elements or 3-D rigid line/parabola segments, use the following command or GUI path. ANSYS creates a single line over each line, parabolic segments over B-splines, and arc segments over each arc and line fillet (see Figure 3.2). If all the arcs form a closed circle, ANSYS creates a single circular segment (see Figure 3.3). However, if the arcs that form a closed circle are created from imported or archived geometry (such as IGES), ANSYS might not create a single circular segment.
|GUI:||Main Menu> Preprocessor> Meshing> Mesh> Lines|
To generate 3-D rigid target elements, use the following command or GUI path.
|GUI:||Main Menu> Preprocessor> Meshing> Mesh> Areas|
If the surface segments on the solid model form a complete sphere, cylinder, or cone, then ANSYS automatically generates a single primitive 3-D target element through the AMESH command. By creating fewer elements, the analysis becomes more computationally efficient. For arbitrary surfaces, you should use AMESH to generate target elements. In these cases, the quality of the meshed target shape is not important. It is more important that the target elements represent the rigid surface geometry well.
We recommend using mapped meshing on all possible areas. If there is no curvature on the edges of the surface, assign one division on that edge. TARGE169 with a rigid specification will always mesh with one element division, per line, ignoring any LESIZE setting. The default target element shape is quadrilateral. If you want a triangular target element shape, use MSHAPE,1. Figure 3.4 shows the meshing patterns for arbitrary target surfaces. The following command or GUI path will generate a mapped mesh wherever possible (otherwise, if not possible, it will generate a free mesh).
|GUI:||Main Menu> Preprocessor> Meshing> Mesh> Areas> Target Surf|
If the target surface is flat (or nearly flat), you may select low-order target elements (3-node triangular or 4-node quadrilateral elements). If the target surface is curved you should select high-order target elements (6-node triangular or 8-node quadrilateral). By doing so, set KEYOPT(1) = 1 in the target element definition.
Low-order target elements result in "cheaper" CPU usage in getting penetration and gap; however, the meshed surface may not be smooth. Higher-order target elements are more "expensive" to use in getting the penetration and gap, but they need many fewer elements to discretize the whole curved target surface.
A target surface can be made up of two or more disconnected regions. Where possible, you should localize the contact zone by defining multiple target surfaces (each with a different real constant number). There are no restrictions on the shape of the rigid surfaces. Smoothing is not required. However, you must ensure that the mesh discretization of the curved surfaces on the rigid target surface is adequate. Excessively coarse discretization can cause numerical convergence problems. It can be difficult to obtain a converged solution in a large sliding simulation if the target surface has sharp convex corners. To avoid such modeling problems, use line or area fillet functions on the solid model to smooth out the sharp corner, use a more refined mesh, or use high-order element in the region of abrupt curvature changes (see Figure 3.5).
The node order of the target surface elements is critical because it defines contact direction. For 2-D contact, the associated (deformable) 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 (see Figure 3.6).
For 3-D contact, the target element numbering should be such that the rigid surface's outward normal points toward the contact surface. The outward normal is determined by the right-hand rule.
For 3-D line segments, the target nodes must be numbered in a sequence that defines a continuous line. The line can be made up of linear or parabolic segments, depending on whether the underlying beam is made up of first order or second order elements.
To check the direction of the normals, turn on the element coordinate systems.
|GUI:||Utility Menu> PlotCtrls> Symbols|
If the element normals do not point toward the contact surface, select this element and reverse the direction of the surface normals.
|GUI:||Main Menu> Preprocessor> Modeling> Create> Elements> Surf/Contact> Surf to Surf|
or, reorient the element normals:
|GUI:||Main Menu> Preprocessor> Modeling> Move/Modify> Elements> Shell Normals|