TARGE169 is used to represent various 2-D "target" surfaces for the associated contact elements (CONTA171, CONTA172, and CONTA175). The contact elements themselves overlay the solid elements describing the boundary of a deformable body and are potentially in contact with the target surface, defined by TARGE169. This target surface is discretized by a set of target segment elements (TARGE169) and is paired with its associated contact surface via a shared real constant set. You can impose any translational or rotational displacement, temperature, voltage, and magnetic potential on the target segment element. You can also impose forces and moments on target elements. See TARGE169 in the Mechanical APDL Theory Reference for more details about this element. To represent 3-D target surfaces, use TARGE170, a 3-D target segment element. For rigid targets, these elements can easily model complex target shapes. For flexible targets, these elements will overlay the solid elements describing the boundary of the deformable target body.
The target surface is modeled through a set of target segments, typically, several target segments comprise one target surface.
The target surface can either be rigid or deformable. For modeling rigid-flexible contact, the rigid surface must be represented by a target surface. For flexible-flexible contact, one of the deformable surfaces must be overlayed by a target surface. See the Contact Technology Guide for more information about designating contact and target surfaces.
The target and associated contact surfaces are identified by a shared real constant set. This real constant set includes all real constants for both the target and contact elements.
Each target surface can be associated with only one contact surface, and vice-versa. However, several contact elements could make up the contact surface and thus come in contact with the same target surface. Likewise, several target elements could make up the target surface and thus come in contact with the same contact surface. For either the target or contact surfaces, you can put many elements in a single target or contact surface, or you can localize the contact and target surfaces by splitting the large surfaces into smaller target and contact surfaces, each of which contain fewer elements.
If one contact surface may contact more than one target surface, you must define duplicate contact surfaces that share the same geometry but relate to separate targets, that is, have separate real constant set numbers.
For any target surface definition, the node ordering of the target segment element is critical for proper detection of contact. The nodes must be ordered so that, for a 2-D surface, the associated contact elements (CONTA171, CONTA172, or CONTA175) must lie to the right of the target surface when moving from target node I to target node J. For a rigid 2-D complete circle, contact must occur on the outside of the circle; internal contacting is not allowed.
Each target segment is a single element with a specific shape, or segment type. The segment types are defined by one, two, or three nodes and a target shape code, TSHAP, and are described in Table 169.1: TARGE169 2-D Segment Types, Target Shape Codes, and Nodes. The TSHAP command indicates the geometry (shape) of the element. The segment dimensions are defined by a real constant (R1), and the segment location is determined by the nodes. ANSYS supports seven 2-D segment types; see Table 169.1: TARGE169 2-D Segment Types, Target Shape Codes, and Nodes.
Table 169.1 TARGE169 2-D Segment Types, Target Shape Codes, and Nodes
|TSHAP||Segment Type||Node1 (DOF)||Node 2 (DOF)||Node 3 (DOF)||R1||R2|
|LINE||Straight line||1st corner pt (UX, UY) (TEMP) (VOLT) (AZ)||2nd corner pt (UX, UY) (TEMP) (VOLT) (AZ)||None||None||None|
|ARC||Arc, clockwise||1st corner pt (UX, UY) (TEMP) (VOLT) (AZ)||2nd corner pt (UX, UY) (TEMP) (VOLT) (AZ)||Circle center pt (UX, UY) (TEMP) (VOLT) (AZ)||None||None|
|CARC||Arc, counter- clockwise||1st corner pt (UX, UY) (TEMP) (VOLT) (AZ)||2nd corner pt (UX, UY) (TEMP) (VOLT) (AZ)||Circle center pt (UX, UY) (TEMP) (VOLT) (AZ)||None||None|
|PARA||Parabola||1st corner pt (UX, UY) (TEMP) (VOLT) (AZ)||2nd corner pt (UX, UY) (TEMP) (VOLT) (AZ)||Midside pt (UX, UY) (TEMP) (VOLT) (AZ)||None||None|
|CIRC||Circle||Circle center pt (UX, UY) (TEMP) (VOLT) (AZ)||None||None||Radius||None|
|PILO||Pilot node||1st point (UX, UY, ROTZ) (TEMP) (VOLT) (AZ)||None||None||None||None|
|POINT||Point||1st point (UX, UY)||None||None||None||None|
For simple rigid target surfaces, you can define the target segment elements individually by direct generation. You must first specify the SHAPE argument for the TSHAP command. When creating circles through direct generation, you must also define the real constant R1 before creating the element. Real constant R1 (see Table 169.1: TARGE169 2-D Segment Types, Target Shape Codes, and Nodes) defines the radius of the target circle.
For rigid-to-flexible contact, by default, ANSYS automatically fixes the structural degree of freedom for rigid target nodes if they aren't explicitly constrained (KEYOPT(2) = 0). If you wish, you can override the automatic boundary condition settings by setting KEYOPT(2) = 1 for the target elements. For flexible-to-flexible contact, no special boundary conditions treatment is performed, and the KEYOPT(2) = 0 setting should be used.
For each rigid-flexible contact pair, you can assign only one pilot node to an entire rigid target surface (or none if it is not needed). The pilot node, unlike the other segment types, is used to define the degrees of freedom for the entire target surface. This node can be any of the target surface nodes, but it does not have to be. All possible rigid motions of the target surface will be a combination of a translation and a rotation around the pilot node. The pilot node provides a convenient and powerful way to assign boundary conditions such as rotations, translations, moments, temperature, voltage, and magnetic potential on an entire rigid target surface. By default (KEYOPT(2) = 0), you can assign the boundary conditions only to the pilot node, eliminating the need to assign boundary conditions to individual target nodes, thus reducing the chance of errors. ANSYS will also automatically fix the structural degrees of freedom on the pilot node if they aren't explicitly constrained.
By setting KEYOPT(2) = 1 for the target elements, you can apply boundary conditions on any rigid target nodes rather than only on the pilot node. It is your responsibility to make sure the rigid target surface is not under-constrained or over-constrained. It is still recommended that you apply all boundary conditions on the pilot node, even when KEYOPT(2) = 1.
For general deformable surfaces, you will normally use the ESURF command to overlay the target elements on the boundary of the existing mesh. Note that the segment types (TSHAP command) should not be used for this case.
In general, curved contact and target surfaces can be well approximated by linear or quadratic contact and target elements when the mesh is sufficiently refined. However, in certain circumstances (for example, when linear elements are used or when the midside nodes of quadratic elements do not lie exactly on the initial curved geometry because a third party mesh generator was used), using a straight line in place of the true curved geometry can significantly affect the accuracy of contact stresses. An optional geometric correction can be used for a circular (or nearly circular) arc via SECTYPE and SECDATA section commands. The defined geometry correction can be applied to specific contact elements via a section ID (SECNUM command). For details, see Geometry Correction for Contact and Target Surfaces in the Contact Technology Guide.
To model fluid penetration loads, use the SFE command to specify the fluid pressure and fluid penetration starting points. For more information, see Applying Fluid Pressure-Penetration Loads in the Contact Technology Guide.
By default, the temperature is set to the value of TUNIF, and if this has no explicit value the temperature is set to zero. For thermal contact analysis, such as convection and radiation modeling, the behavior of a thermal contact surface (whether a “near-field” or “free” surface) is usually based on the contact status. Contact status affects the behavior of the contact surface as follows:
If the contact surface is outside the pinball region, its behavior is as a far-field of free surface. In this instance, convection/radiation occurs with the ambient temperature.
If the contact surface is inside the pinball region, the behavior is as a near-field surface.
I, J, K (J and K are not required for all segment types)
UX, UY, ROTZ, TEMP, VOLT, AZ (ROTZ is used for the pilot node only )
Pressure, Face 1 (I-J) (opposite to target normal direction)
|Birth and death|
|Fluid pressure penetration|
|Section definition for geometry correction of spherical and revolute surfaces|
Boundary conditions for rigid target nodes:
Automatically constrained by ANSYS
Specified by user
Behavior of thermal contact surface:
Based on contact status
Treated as free-surface
DOF set to be constrained on dependent DOF for internally-generated multipoint constraints (MPCs). This option is used for these situations: solid-solid and shell-shell assemblies; surface-based constraints that use a single pilot node for the target element; and rigid target surfaces that use the KEYOPT(2) = 1 setting.
Enter a three digit value that represents the DOF set to be constrained. The first to third digits represent ROTZ, UY, UX, respectively. The number 1 (one) indicates the DOF is active, and the number 0 (zero) indicates the DOF is not active. For example, 011 means that UX and UY will be used in the multipoint constraint. Leading zeros may be omitted; for example, you can enter 1 to indicate that UX is the only active DOF. If KEYOPT(4) = 0 (which is the default) or 111, all DOF are constrained.
Symmetry condition of a constrained surface. This option is only used for a force-distributed constraint that uses a single pilot node for the target element:
The constrained surface has a symmetry condition with respect to the y axis of the nodal coordinate system of the pilot node.
The constrained surface has a symmetry condition with respect to the x axis of the nodal coordinate system of the pilot node.
Keep the following points in mind when using this symmetry condition:
The solution output associated with the element is shown in Table 169.2: TARGE169 Element Output Definitions. The following notation is used:
The Element Output Definitions table uses the following notation:
A colon (:) in the Name column indicates that the item can be accessed by the Component Name method (ETABLE, ESOL). The O column indicates the availability of the items in the file Jobname.OUT. The R column indicates the availability of the items in the results file.
In either the O or R columns, “Y” indicates that the item is always available, a number refers to a table footnote that describes when the item is conditionally available, and “-” indicates that the item is not available.
Table 169.2 TARGE169 Element Output Definitions
|NODES||Nodes I, J, and K||Y||Y|
|ITRGET||Target surface number (assigned by ANSYS)||Y||Y|
|TSHAP||Segment shape type||Y||Y|
|FPRS||Actual applied fluid penetration pressure||Y||Y|
You can display or list the actual fluid pressure applied to the target element through several POST1 postprocessing commands, as shown below:
PLESOL,CONT,FPRS PLNSOL,CONT,FPRS PRESOL,CONT PRNSOL,CONT
Table 169.3: TARGE169 Item and Sequence Numbers lists output available through the ETABLE command using the Sequence Number method. See Creating an Element Table in the Basic Analysis Guide and The Item and Sequence Number Table in this manual for more information. The following notation is used in Table 169.3: TARGE169 Item and Sequence Numbers:
The 2-D segment element must be defined in an X-Y plane.
For each pilot node, ANSYS automatically defines an internal node and an internal constraint equation. The rotational DOF of the pilot node is connected to the translational DOF of the internal node by the internal constraint equation. ANSYS recommends against using external constraint equations or coupling on pilot nodes; if you do, conflicts may occur, yielding incorrect results.
For circular arcs, the third node defines the actual center of the circle and must be defined accurately when the element is generated and must be moved consistently with the other nodes during the deformation process. If the third node is not moved consistently with the other nodes, the arc shape will change with that node's movement. To ensure the correct behavior, apply all boundary conditions to a pilot node.
For parabolic segments, the third point must lie at the middle of the parabola.
Generally speaking, you should not change the R1 real constant between load steps or during restart stages; otherwise ANSYS assumes the radius of the circle varies between the load steps. When using direct generation, the real constant R1 for circles may be defined before the input of the element nodes. If multiple rigid circles are defined, each having a different radius, they must be defined by different target surfaces.
For rotation of a rigid body constrained only by a bonded, rigid-flexible contact pair with a pilot node, use the MPC algorithm or a surface-based constraint as described in "Multipoint Constraints and Assemblies" in the Contact Technology Guide. Penalty-based algorithms can create undesirable rotational energies in this situation.