# DGAP elements DGAP elements are used to model thermal interactions between two nodes in heat transfer analyses. The behavior of the interaction being modeled is defined by the initial separation distance (clearance), d, of the gap. # Clearance between DGAP nodes Abaqus/Standard defines the clearance between two nodes of the gap, h, as $$ h = d. $$ Since there are no displacements in a heat transfer analysis, the clearance remains unchanged. The clearance is used only for clearance-dependent thermal interactions. You specify a value for d. If you provide a positive value, the gap is open initially. If d=0, the gap is closed initially. If d is negative, the gap is considered overclosed but no interference fit is performed. The contact direction does not need to be specified: any contact direction specified is ignored in the analysis. You must supply the contact area associated with these elements for Abaqus/Standard to compute the heat flux value per unit area. Input File Usage: $\ast \mathrm { G A P }$ $d , \ , \ , \ c r o s s { - } s e c t i o n a l \ a r e a$ # Defining nondefault mechanical interactions with gap elements The default mechanical interaction model for problems modeled with gap elements is “hard,” frictionless contact. You can assign optional mechanical interaction models. The following mechanical interaction models are available: • Friction. See “Frictional behavior,” Section 37.1.5, for details. • Modified “hard” contact, softened contact, and viscous damping. See “Contact pressure-overclosure relationships,” Section 37.1.2, and “Contact damping,” Section 37.1.3, for details. # Defining thermal surface interactions with GAPUNIT and DGAP elements You can assign thermal interaction models to these elements. The following thermal interaction models are available: • Gap conduction. • Gap radiation. • Gap heat generation. These thermal interaction models are discussed in “Thermal contact properties,” Section 37.2.1. # Modeling large initial interference with gap elements Specifying a large negative initial overclosure (interference) may lead to convergence problems as Abaqus/Standard tries to resolve the overclosure in a single increment. You can prescribe an allowable interference to allow Abaqus/Standard to resolve the overclosure gradually. See “Modeling contact interference fits in Abaqus/Standard,” Section 36.3.4, for more details on modeling interference fit problems. Input File Usage: \*CONTACT INTERFERENCE, TYPE=ELEMENT # 40.2.2 GAP ELEMENT LIBRARY Product: Abaqus/Standard # References • “Gap contact elements,” Section 40.2.1 • \*GAP # Overview This section provides a reference to the gap elements available in Abaqus/Standard. # Element types # Stress/displacement elements GAPUNI Unidirectional gap between two nodes GAPCYL Cylindrical gap between two nodes GAPSPHER Spherical gap between two nodes Active degrees of freedom 1, 2, 3 Additional solution variables Three additional variables relating to the contact and friction forces. # Coupled temperature-displacement element GAPUNIT Unidirectional gap and thermal interactions between two nodes Active degrees of freedom 1, 2, 3, 11 Additional solution variables Three additional variables relating to the contact and friction forces. # Heat transfer element DGAP Thermal interactions between two nodes Active degree of freedom 11 Additional solution variables None. # Nodal coordinates required For DGAP elements, and for GAPUNI and GAPUNIT if you specify the contact direction , the nodal coordinates are not used in the contact calculations; however, it is useful to define the coordinates of the two nodes for plotting purposes. GAPCYL and GAPSPHER: X, Y, Z # Element property definition You can specify the initial clearance, the contact direction (normal to the interface), and the contact area. For GAPUNI, GAPUNIT, and DGAP elements, a negative clearance indicates an initial overclosure. For GAPCYL and GAPSPHER elements, specify the maximum separation as a positive number or the minimum separation as a negative number. Input File Usage: \*GAP # Element-based loading None. Element output

S11	Pressure transmitted between the surfaces. The pressure is defined as the force divided by the user-specified area.
S12	First frictional shear stress normal to the gap direction.
S13	Second frictional shear stress normal to the gap direction.
E11	Current opening h of the gap element.
E12	Relative displacement (“slip”) in the first direction orthogonal to the contact direction.
E13	Relative displacement (“slip”) in the second direction orthogonal to the contact direction.

Available for elements with temperature degrees of freedom. HFL1 Heat flux across the interface in the contact direction. The increments of shear slip are the relative displacement increments projected onto the two local directions that are orthogonal to the contact direction. In two-dimensional or axisymmetric models when the contact direction is along the first axis (X or r), the active slip direction is E13 and the active shear stress is S13. In any other two-dimensional or axisymmetric case, the active slip direction is E12 and the active shear stress is S12. Two nodes: the ends of the gap. # 40.3 Tube-to-tube contact elements • “Tube-to-tube contact elements,” Section 40.3.1 • “Tube-to-tube contact element library,” Section 40.3.2 # 40.3.1 TUBE-TO-TUBE CONTACT ELEMENTS # Product: Abaqus/Standard # References • “Tube-to-tube contact element library,” Section 40.3.2 • \*INTERFACE • \*SLIDE LINE # Overview Tube-to-tube elements: • model the finite-sliding interaction between two pipelines or tubes where one tube lies inside the other or between two tubes or rods that lie next to each other; • are slide line contact elements, in the sense that they assume that the relative motion of the two tubes or pipes is predominantly along the line defined by the axis of one of the tubes (the relative rotations of the tube or pipe axis are assumed to be small); • can be used with pipe, beam, or truss elements; and • do not consider deformations of the tube or pipe cross-section. Chapter 36, “Defining Contact Interactions,” contains a general discussion of contact modeling. # Typical applications The tube-to-tube contact elements can be used to model two specific classes of tube-to-tube contact problems: internal (tube within a tube) contact and external contact, where the two tubes are roughly parallel and contact each other along their outer surfaces. # Choosing an appropriate element Use ITT21 elements with two-dimensional beam, pipe, or truss elements. Use ITT31 elements with three-dimensional beam, pipe, or truss elements. Each of these elements is defined by a single node. # Associating the tube-to-tube contact elements with a slide line You must indicate which set of tube-to-tube contact elements will interact with a particular slide line. Details on defining slide lines are discussed below. Input File Usage: \*SLIDE LINE, ELSET=element\_set\_name # Defining the element’s section properties You must associate the geometric section properties with a set of tube-to-tube contact elements. Input File Usage: \*INTERFACE, ELSET=element\_set\_name # Defining the radial clearance when modeling contact between a pipe within another pipe You define the radial clearance between the pipes. Give a positive value to model contact between two pipes when one pipe (the one with the tube-to-tube contact elements) lies inside of the other pipe. The value given is the difference between the inner radius of the outer pipe and the outer radius of the inner pipe. Input File Usage: \*INTERFACE radial clearance # Defining the radial clearance when modeling contact between the outer surfaces of two pipes You can model external tube-to-tube contact by specifying a negative value for the radial clearance. The magnitude of the value must be the sum of the outer radii of the two pipes or rods. # Local basis for contact output variables The element output variables for ITT elements are given in a local basis system associated with the slide line. The first tangent vector, $\mathbf { t } _ { 1 : }$ , is defined by the sequence of the nodes forming the slide line. The direction of contact, , is the normal to the slide line that points toward the nodes of the ITT elements. For ITT31 elements Abaqus/Standard forms a second tangent vector, $\mathbf { t } _ { 2 } .$ , that is orthogonal to both $\mathbf { t } _ { 1 }$ and . As the elements move, the local basis system will rotate with the axis of the slide line. # Choosing which pipe (beam or truss) will have the slide line In the case of internal tube-to-tube contact, the slide line can be placed on the inner tube or the outer tube. Generally the slide line should be associated with the outer tube (see Figure 40.3.1–1); however, if the inner tube is stiffer than the outer tube, the slide line should be attached to the inner tube. If contact occurs between the exterior surface of the tubes, the slide line should be associated with the stiffer tube if the materials or tube radii are different or with the tube with the coarser mesh if they are the same. # Defining the slide line You can specify the nodes that make up the slide line, or they can be generated as described below. If you choose to specify the nodes directly, you must specify them in a sequence that defines a continuous slide line. The nodal sequence defines a tangent vector $\mathbf { t } _ { 1 }$ for the slide line. The slide line must be made up of linear segments. Input File Usage: \*SLIDE LINE, ELSET=element\_set\_name, TYPE=LINEAR first node number, second node number, etc. # Generating the slide line nodes Alternatively, you can indicate that the slide line nodes should be generated and specify only a first node number, a last node number, and an increment between node numbers.