3-D Target Segment

TARGE170 Element Description

TARGE170 is used to represent various 3-D "target" surfaces for the associated contact elements (CONTA173, CONTA174, CONTA175, CONTA176, and CONTA177). The contact elements themselves overlay the solid, shell, or line elements describing the boundary of a deformable body and are potentially in contact with the target surface, defined by TARGE170. This target surface is discretized by a set of target segment elements (TARGE170) 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 TARGE170 in the Mechanical APDL Theory Reference for more details about this element. To represent 2-D target surfaces, use TARGE169, a 2-D target segment element.

For rigid target surfaces, these elements can easily model complex target shapes. For flexible targets, these elements will overlay the solid, shell, or line elements describing the boundary of the deformable target body.

Figure 170.1  TARGE170 Geometry

TARGE170 Geometry

TARGE170 Input Data

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 via 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 a 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, that have separate real constant set numbers.

Figure 170.2 shows the available segment types for TARGE170. The general 3-D surface segments (3-node and 6-node triangles, and 4-node and 8-node quadrilaterals) and the primitive segments (cylinder, cone, and sphere) can be paired with 3-D surface-to-surface contact elements, CONTA173 and CONTA174, the 3-D node-to-surface contact element, CONTA175, and the 3-D line-to-surface contact element, CONTA177. The line segments (2-node line and 3-node parabola) can only be paired with the 3-D line-to-line contact element, CONTA176, to model 3-D beam-to-beam contact.

For any target surface definition, the node ordering of the target segment element is critical for proper detection of contact. For the general 3-D surface segments (triangle and quadrilateral segment types), the nodes must be ordered so that the outward normal to the target surface is defined by the right hand rule (see Figure 170.2). Therefore, for the surface target segments, the outward normal by the right hand rule is consistent to the external normal. For 3-D line segments (straight line and parabolic line), the nodes must be entered in a sequence that defines a continuous line. For a rigid cylinder, cone, or sphere, contact must occur on the outside of the elements; internal contacting of these segments is not allowed.

Considerations for Rigid Target Surfaces

Each target segment of a rigid surface is a single element with a specific shape, or segment type.The segment types are defined by several nodes and a target shape code, TSHAP, and are described in Table 170.1: TARGE170 3-D Segment Types, Target Shape Codes, and Nodes. The TSHAP command indicates the geometry (shape) of the element. The segment radii are defined by real constants (R1 and R2), and the segment location is determined by the nodes. ANSYS supports eleven 3-D segment types; see Table 170.1: TARGE170 3-D Segment Types, Target Shape Codes, and Nodes.

Table 170.1  TARGE170 3-D Segment Types, Target Shape Codes, and Nodes

TSHAPSegment TypeNodes (DOF)[1]R1R2
TRIA3-node triangle1st - 3rd nodes are corner points (UX, UY, UZ) (TEMP) (VOLT) (MAG)NoneNone
QUAD4-node quadrilateral1st - 4th nodes are corner points (UX, UY, UZ) (TEMP) (VOLT) (MAG)NoneNone
TRI66-node triangle1st - 3rd nodes are corner points, 4th - 6th are midside nodes (UX, UY, UZ) (TEMP) (VOLT) (MAG)NoneNone
QUA88-node quadrilateral1st - 4th nodes are corner points, 5th - 8th are midside nodes (UX, UY, UZ) (TEMP) (VOLT) (MAG)NoneNone
LINE2-node straight line1st - 2nd nodes are line end points (UX, UY, UZ)Target Radius[4]Contact Radius[5]
PARA3-node parabola1st - 2nd nodes are line end points, 3rd is a midside node (UX, UY, UZ) Target Radius[4]Contact Radius[5]
CYLICylinder[2]1st - 2nd nodes are axial end points (UX, UY, UZ) (TEMP) (VOLT) (MAG)RadiusNone
CONECone[2]1st - 2nd nodes are axial end points (UX, UY, UZ) (TEMP) (VOLT) (MAG)Radius at node 1Radius at node 2
SPHESphere[2]Sphere center point (UX, UY, UZ) (TEMP) (VOLT) (MAG)RadiusNone
PILOPilot node[3]1st point: (UX, UY, UZ, ROTX, ROTY, ROTZ) (TEMP) (VOLT) (MAG)NoneNone
POINTPoint61st point: (UX, UY, UZ)NoneNone
  1. The DOF available depends on the setting of KEYOPT(1) of the associated contact element. Refer to the element documentation for either CONTA173, CONTA174, or CONTA175 for more details.

  2. When creating a cylinder, cone, or sphere via direct generation, define the real constant set before creating the element.

  3. Only pilot nodes have rotational degrees of freedom (ROTX, ROTY, ROTZ).

  4. Input the target radius as a negative value when modeling internal pipe-to-pipe contact (a pipe contacting/sliding inside another pipe). Input a positive value to model external 3-D beam-to-beam contact.

  5. Input a positive contact radius when modeling internal pipe-to-pipe contact or external 3-D beam-to-beam contact.

  6. Rigid surface node. This segment type is only used to apply boundary conditions to rigid target surfaces.

Figure 170.2 shows the 3-D segment shapes.

Figure 170.2  TARGE170 Segment Types

TARGE170 Segment Types

For simple rigid target surfaces (including line segments), you can define the target segment elements individually by direct generation. You must first specify the SHAPE argument on the TSHAP command. When creating cylinders, cones, or spheres through direct generation, you must also define the real constant R1 (and R2 for cones) before creating the element. Real constants R1 and R2 (see Table 170.1: TARGE170 3-D Segment Types, Target Shape Codes, and Nodes) define the dimensions of the target shape.

For general 3-D rigid surfaces, target segment elements can be defined by area meshing (AMESH). Set KEYOPT(1) = 0 (the default) to generate low order target elements (3-node triangles and/or 4-node quadrilaterals) for rigid surfaces. Set KEYOPT(1) = 1 to generate target elements with midside nodes (6-node triangles and/or 8-node quadrilaterals).

For 3-D rigid lines, target segment elements can be defined by line meshing (LMESH). Set KEYOPT(1) = 0 (the default) to generate low order target elements (2-node straight lines). Set KEYOPT(1) = 1 to generate target elements with midside nodes (3-node parabolas).

You can also use keypoint meshing (KMESH) to generate the pilot node.

If the TARGE170 elements will be created via program meshing (AMESH, LMESH, or KMESH commands), then the TSHAP command is ignored and ANSYS chooses the correct shape automatically.

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.

Considerations for Deformable Target Surfaces

For general deformable surfaces, use the ESURF command to overlay the target elements on the boundary of the existing mesh. By default, the command generates a target element with an external surface that has the same shape as the underlying element. You can issue ESURF,,,LINE to generate 3-D line or parabola segments on an exterior of selected 3-D elements (e.g., shell edges). Segment types (TSHAP command) should not be used prior to ESURF when generating target elements on deformable target surfaces.

The cylinder, cone, sphere, point, and pilot node target segments should not be used for deformable target surfaces. However, you can use geometry correction (see below) for deformable target surfaces that represent (or approximately represent) a sphere, cylinder, or cone.

Considerations for Geometry Correction

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 faceted surface in place of the true curved geometry can significantly affect the accuracy of contact stresses. An optional geometric correction can be used for two types of curved surfaces (spherical and revolute) 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.

Considerations for Fluid Penetration Loading

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.

Considerations for Thermal Contact Analysis

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.

However, the thermal contact surface status is ignored if KEYOPT(3) = 1 is set, and the surface is always treated as a free surface (see CONTA173, CONTA174, or CONTA175 for details).

A summary of the element input is given in "TARGE170 Input Summary". A general description of element input is given in Element Input.

TARGE170 Input Summary


I, J, K, L, M, N, O, P (J - P are not required for all segment types)

Degrees of Freedom

UX, UY, UZ, TEMP, VOLT, MAG (ROTX, ROTY, ROTZ for pilot nodes only)

Real Constants

R1, R2, [the others are defined through the associated CONTA173, CONTA174, CONTA175, CONTA176, or CONTA177 elements]

Material Properties


Surface Loads

Pressure, Face 1 (I-J-K-L) (opposite to target normal direction)

Body Loads


Special Features
Birth and death
Fluid pressure penetration
Linear perturbation
Section definition for geometry correction of spherical and revolute surfaces

Element order (used by AMESH and LMESH commands only):

0 -- 

Low order elements

1 -- 

High order elements


Boundary conditions for rigid target nodes:

0 -- 

Automatically constrained by ANSYS

1 -- 

Specified by user


Behavior of thermal contact surface:

0 -- 

Based on contact status

1 -- 

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.

n -- 

Enter a six digit value that represents the DOF set to be constrained. The first to sixth digits represent ROTZ, ROTY, ROTX, UZ, 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, 100011 means that UX, UY, and ROTZ will be used in the multipoint constraint. Leading zeros may be omitted; for example, you can enter 11 to indicate that UX and UY are the only active DOF. If KEYOPT(4) = 0 (which is the default) or 111111, all DOF are constrained.


DOF set to be used in internally-generated multipoint constraints (MPCs), with the MPC algorithm and no separation or bonded behavior (KEYOPT(2) = 2 and KEYOPT(12) = 4, 5, or 6 on the contact element). Note that this key option is not used for surface-based constraints. (See "Multipoint Constraints and Assemblies" in the Contact Technology Guide for more information):

0 -- 

Automatic constraint type detection (default)

1 -- 

Solid-solid constraint (no rotational DOFs are constrained)

2 -- 

Shell-shell constraint (both translational and rotational DOFs are constrained independently). Also used with penalty based shell-shell assembly (KEYOPT(2) = 0 or 1 and KEYOPT(12) = 5 or 6 on the contact element); see Bonded Contact for Shell-Shell Assemblies in the Contact Technology Guide for more information.

3 -- 

Shell-solid constraint - contact normal direction (both translational and rotational DOFs from the contact surface are included in the constraint set; only translational DOFs from the target surface are included in the constraint set).

4 -- 

Shell-solid constraint - all directions. This option acts the same as KEYOPT(5) = 3 if an intersection is found from the contact normal to the target surface. Otherwise, constraint equations are still built as long as contact node(s) and target segments are inside the pinball region.

5 -- 

Shell-solid constraint - anywhere inside pinball region. Constraint equations are always built as long as contact node(s) and target segments are inside the pinball region, regardless of whether an intersection exists between the contact normal and the target surface.


When the no separation option (KEYOPT(12) = 4 on the contact element) is used with the MPC approach, only the KEYOPT(5) = 0 and 1 options (auto detection or solid-solid constraint) described above are valid. If the auto detection option is set and the program finds a shell-shell or shell-solid constraint in this situation, the solution will terminate.


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:

n -- 

Enter a three digit value that represents the symmetry conditions on the constrained surface. Symmetry is defined with respect to the nodal coordinate system of the pilot node. The first, second, and third digits represent a symmetry condition with respect to the xy, xz, and yz planes, respectively. The number 1 (one) indicates a symmetry condition, and the number 0 (zero) indicates no symmetry condition. For example, KEYOPT(6) = 110 means the force distributed constraint is built on a surface or edge that has symmetry about the xy and xz planes. Leading zeros may be omitted (e.g., KEYOPT(6) = 10 indicates symmetry about the xz plane only).


Keep the following points in mind when using this symmetry condition:

  • When a symmetry condition is used, the pilot node must be defined on the symmetry plane/edge.

  • KEYOPT(6) = 111 is not valid input.

TARGE170 Output Data

The solution output associated with the element is shown in Table 170.2: TARGE170 Element Output Definitions.

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 170.2  TARGE170 Element Output Definitions

ELElement NumberYY
NODESNodes I, J, and KYY
ITRGETTarget surface number (assigned by ANSYS)YY
TSHAPSegment shape typeYY
ISEGSegment numbering11
FPRSActual applied fluid penetration pressureYY
  1. An internal segment number determined by ANSYS. ISEG for the target element has a different meaning than ISEG reported for the contact element.

You can display or list the actual fluid pressure applied to the target element through several POST1 postprocessing commands, as shown below:


Note that only the FPRS (fluid penetration pressure) output item is meaningful when the PRESOL and PRNSOL commands are used for target elements.

Table 170.3: TARGE170 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 170.3: TARGE170 Item and Sequence Numbers:


output quantity as defined in the Table 170.2: TARGE170 Element Output Definitions


predetermined Item label for ETABLE command


sequence number for single-valued or constant element data


sequence number for data at nodes I, J, K, L

Table 170.3  TARGE170 Item and Sequence Numbers

Output Quantity NameETABLE and ESOL Command Input

TARGE170 Assumptions and Restrictions

  • Generally speaking, you should not change real constants R1 or R2, either between load steps or during restart stages; otherwise ANSYS assumes the radii of the primitive segments varies between the load steps. When using direct generation, the real constants for cylinders, cones, and spheres may be defined before the input of the element nodes. If multiple rigid primitives are defined, each having different radii, they must be defined by different target surfaces.

  • 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 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.

TARGE170 Product Restrictions

There are no product-specific restrictions for this element.

Release 14.0 - © 2011 SAS IP, Inc. All rights reserved.