PRETS179 is used to define a 2-D or 3-D pretension section within a meshed structure. The structure can be built from any 2-D or 3-D structural elements (solid, beam, shell, pipe, or link). The PRETS179 element has one translation degree of freedom, UX. (UX represents the defined pretension direction. ANSYS transforms the geometry of the problem so that, internally, the pretension force is applied in the specified pretension load direction, regardless of how the model is defined.) Loads can be applied using the SLOAD command. These loads will overwrite any F or D command specifications on the same nodes at solution time. Only tension loads can be applied; bending or torsion loads are ignored. See PRETS179 in the Mechanical APDL Theory Reference for more details about the element. See Defining Pretension in a Joint Fastener in the Basic Analysis Guide for a discussion of how to generate PRETS179 elements automatically using the PSMESH command. When creating the PRETS179 elements, the pretension load direction is specified relative to surface A. (For backward compatibility, it is also possible to generate such elements using the EINTF command.)
The pretension section is modeled by a set of pretension elements. The geometry, node locations, and the coordinate system for the pretension element are shown in Figure 179.1: PRETS179 Geometry. The pretension element is defined by three nodes I, J, K and the section data NX, NY, NZ which define the pretension load direction relative to surface A. The pretension load direction is constant and is not updated for large displacements. Although it is not recommended, the pretension load direction can be changed between load steps by changing the section data. For large-deflection problems, you could track the deflection and change the pretension load direction accordingly.
Nodes I and J are initially coincident and they should be defined in the same nodal coordinate system. No boundary conditions apply on node J. For each pretension section, the node ordering of the pretension elements is critical. The I and J nodes must be ordered so that all nodes I are on surface A and all nodes J are on surface B.
Node K is the pretension node. This pretension node provides a convenient way to assign boundary conditions on an entire pretension section. Node K can be anywhere in space; however, its nodal coordinate system must be global Cartesian. Each pretension section has only one pretension node associated with it. Node K should only connect to pretension elements that use the same section number.
The pretension node K has only one translation degree of freedom UX, which defines the relative displacement between the two sections A and B in the pretension load direction. Sliding motion is prevented automatically. If the pretension node and the bolted structure are not well constrained, rigid body motion can occur. Therefore, in the beginning of each load step, you should verify the boundary conditions for bolt structures carefully.
The following table summarizes the element input. Element Input gives a general description of element input.
Nodal displacements are included in the overall displacement solution. There is no printed or post element data output for the pretension element. ANSYS automatically determines the deformations of the bolt structure. The underlying elements connected to both sides of cutting surfaces appear overlap under the pretension load. The displacement of the pretension node gives the adjustment of the pretension. Use PRNSOL to list the adjustment. The reaction force on the pretension node provides the total normal force across the pretension section. Use PRRSOL or PRRFOR command to list the tension force. The stress distribution of underlying elements provides a good estimation of the stress across the pretension section.
The nodal coordinate system of the pretension node K must be global Cartesian.
You cannot apply any constraint equations (or coupling) on any pretension element nodes.
The NROTAT command can not be applied on pretension node K. NROTAT can be applied to the other nodes I and J in such way that they are rotated into the same nodal coordinate system. If K has been mistakenly rotated into another coordinate system, ANSYS will issue a warning and will automatically rotate it back into the global Cartesian system. Similarly, if I and J are rotated into different coordinate systems, ANSYS will issue a warning and will automatically rotate J to be consistent with I.
The pretension normal NX, NY, NZ must be specified through section data. You should not change section data either between load steps or during restart stages; otherwise ANSYS assumes the pretension normal varies between the load steps.
The pretension force is actually applied in the direction of the pretension section normal. However, the pretension force is always specified and displayed in the global X direction since the element has only one degree of freedom, UX.
The structure can be composed of superelements. However, all the pretension nodes must remain as the master nodes.
The element may not be deactivated with the EKILL command.
Use of this element is limited to structural analyses only.