Mechanical APDL Basic Analysis Guide - Ansys

Modeling> Create> Elements> Auto Numbered> At Coincid Nd ...). If K is not defined, ANSYS will create
it automatically. Before using the EINTF command, the element type ID and section properties must be
defined properly. (See the SECDATA command for more information on using the PRETENSION section type.)
The connecting surfaces (A and B) must have matching mesh patterns with coincident nodes. If some node
pairs between the two surfaces are not connected with pretension elements, the resulting analysis can be
inaccurate.
2.8.3. Example Pretension Analysis
The following example describes the typical procedure used to perform a pretension analysis using the
PSMESH command.
1. Mesh the bolt joint, then cut the mesh and insert the pretension elements to form the pretension
section. For example, the following creates a pretension section called “example” by cutting the mesh
and inserting the section into volume 1. Note that a component is created as well (npts) that aids in
plotting or selecting the pretension elements.
psmesh,,example,,volu,1,0,z,0.5,,,,npts
2. In the first load step, apply a force or displacement to node K. In this case, the load is applied as a
force. The force “locks” on the second load step, allowing you to add additional loads. The effect of
the initial load is preserved as a displacement after it is locked. This is shown in the following example.
sload,1,PL01,tiny,forc,100,1,2
3. Apply other external loads as required using the SLOAD command.
The following example will help you to understand how the pretension procedure works.
Release 13.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
2.8.3. Example Pretension Analysis
65