FOLLW201

Follower Load

FOLLW201 Element Description

FOLLW201 is a one-node 3-D element that can be overlaid onto an existing node with physical rotation degrees of freedom. The element specifies external forces and moments which follow the deformation of a structure in a nonlinear analysis. FOLLW201 contributes follower load stiffness terms in a geometrically nonlinear analysis (NLGEOM,ON).

Figure 201.1: FOLLW201 Geometry

FOLLW201 overlaid on a node shared by shell or beam elements. The element has two faces: face 1 for specifying magnitude of force and face 2 for specifying magnitude of moment.

FOLLW201 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 201.1: FOLLW201 Geometry. The element is defined by a single node. The node has three translational and rotational degrees of freedom each. The element may be defined only at those nodes which are associated with structural elements having three translational and rotational degrees of freedom; a singularity will result if the element is used in any other way.

Real constants of the element specify the direction of the force/moment vectors, and the element load command SFE specifies the magnitude of force/moment.

Element loads are described in Nodal Loading. The vectors defined by real constants will evolve with deformation (follow the displacements) in a geometrically nonlinear analysis.

KEYOPT(1) = 1 provides a means of specifying complex (real and imaginary) point loads via an element specification. You can consider it as a nodal point equivalent of surface-effect elements (such as SURF154). When KEYOPT(1) = 1 (intended primarily for use in the ANSYS Workbench interface), the direction of the load is not updated for geometrically nonlinear analyses, and the element is renamed to (and appears in the output as) CLOAD201. In this case, the applied load is the same as that generated via the F command, except that loads can be simultaneously applied in multiple directions to one node. The KEYOPT(2) = 1 setting, which can only be used with KEYOPT(1) = 1, enables use of the CLOAD201 element on nodes that may or may not have active rotational degrees of freedom.

With the exception of follower load effects, the element contributes nothing to the stiffness matrix. By default, follower (pressure) load stiffness effects are included in a geometrically nonlinear analysis. The stiffness contribution is usually unsymmetrical and may require an unsymmetrical solution option (NROPT,UNSYM).

"FOLLW201 Input Summary" contains a summary of the element input. See Element Input in the Element Reference for a general description of element input.

FOLLW201 Input Summary

Nodes

Degrees of Freedom

UX, UY, UZ, ROTX, ROTY, ROTZ

Real Constants

FX - Cosine of the angle between force vector and global X direction

FY - Cosine of the angle between force vector and global Y direction

FZ - Cosine of the angle between force vector and global Z direction

MX - Cosine of the angle between moment vector and global X direction

MY - Cosine of the angle between moment vector and global Y direction

MZ - Cosine of the angle between moment vector and global Z direction

Material Properties

None

Surface Loads

face 1 (force magnitude)

face 2 (moment magnitude)

Body Loads

None

Special Features

Birth and death

Large deflection

Linear perturbation

KEYOPT(1)

Direction load:

0 --: Updated direction load (default)
1 --: Constant direction load (intended primarily for use in the ANSYS Workbench interface)

KEYOPT(2)

Degrees of freedom control:

0 --: Use all (UX, UY, UZ, ROTX, ROTY, ROTZ) degrees of freedom (default)
1 --: Use UX, UY, and UZ degrees of freedom only (valid only when KEYOPT(1) = 1)

FOLLW201 Output Data

The Element Outputs consist of updated direction cosines of the force/moment vectors as Miscellaneous quantities (SMISC). No other output is provided.

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.

The following table lists output available via the ETABLE command using the Sequence Number method. See The General Postprocessor (POST1) in the Basic Analysis Guide and The Item and Sequence Number Table in this reference for more information.

Name: output quantity as defined above
Item: predetermined item label for ETABLE command
I: sequence number for data at node I

Table 201.1: FOLLW201 Item and Sequence Numbers

Name	Item	Location
FX	SMISC	1
FY	SMISC	2
FZ	SMISC	3
MX	SMISC	4
MY	SMISC	5
MZ	SMISC	6

FOLLW201 Assumptions and Restrictions

Follower load stiffening is ignored in geometrically linear analyses (NLGEOM,OFF), which is equivalent to the normal specification of forces and moments (F).
The element must be overlaid on a node having existing physical stiffness contributions (from other shell or beam elements).
Follower load effects are nonconservative. They often introduce dynamics instability issues (such as flutter) which may cause convergence difficulties.

FOLLW201 Product Restrictions

When used in the product(s) listed below, the stated product-specific restrictions apply to this element in addition to the general assumptions and restrictions given in the previous section.

ANSYS Mechanical Pro

Birth and death is not available.
Linear perturbation is not available.

ANSYS Mechanical Premium

Birth and death is not available.