BEAM161 Element Description

BEAM161 has several characteristics:

The Belytschko beam element formulation (KEYOPT(1) = 2, 4, 5) is part of a family of structural finite elements that use a "co-rotational technique" for treating large rotation.

This element is used in explicit dynamic analyses only. Refer to the LS-DYNA Theoretical Manual for more information.

Figure 161.1:  BEAM161 Geometry

BEAM161 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 161.1: BEAM161 Geometry. Node K determines the initial orientation of the cross section.

The element is defined by nodes I and J in the global coordinate system. Node K defines a plane (with I and J) containing the element s-axis. The element r-axis runs parallel to the centroidal line of the element and through nodes I and J. Node K is always required to define the element axis system and it must not be colinear with nodes I and J. The location of node K is used only to initially orient the element. (For information about orientation nodes and beam meshing, see Meshing Your Solid Model in the Modeling and Meshing Guide.)

Use the EDLOAD command to apply nodal loads and other load types described below. For detailed information on how to apply loads in an explicit dynamic analysis, see the ANSYS LS-DYNA User's Guide.

Pressures can be input as surface loads on the element faces as shown by the circled numbers in Figure 161.1: BEAM161 Geometry. Note, however, that pressure is actually a traction load applied to the center line of the element. Use the EDLOAD command to apply the pressure load, and input the pressure as a force per unit length value. Positive normal pressures act into the element.

Base accelerations and angular velocities in the x, y, and z directions can be applied at the nodes using the EDLOAD command. To apply these loads, you need to first select the nodes and create a component. The load is then applied to that component.

You can also use the EDLOAD command to apply loads (displacements, forces, etc.) on rigid bodies.

You can choose from the following materials when working with BEAM161, with the restrictions as noted:

KEYOPT(1) allows you to specify one of four element formulations for BEAM161 (see "BEAM161 Input Summary"). For details of real constants to be specified for each element formulation, see Table 161.1: BEAM161 Real Constants.

KEYOPT(2) is valid only with rectangular element formulations (KEYOPT(1) = 0, 1, 4).

The following illustrations show the valid standard beam cross sections when KEYOPT(4)>0, and KEYOPT(5) = 2 (standard beam cross section).

Figure 161.2:  Standard Beam Cross Sections

Figure 161.3:  Standard Beam Cross Sections (continued)

KEYOPT(5) is not valid when KEYOPT(1) = 2.

A summary of the element input is given in "BEAM161 Input Summary". Additional information about real constants for this element is provided in Table 161.1: BEAM161 Real Constants. For more information about this element, see the ANSYS LS-DYNA User's Guide.

BEAM161 Input Summary

Nodes

I, J, K (K is the orientation node)

Degrees of Freedom

UX, UY, UZ, VX, VY, VZ, AX, AY, AZ, ROTX, ROTY, ROTZ

---

Note:  For explicit dynamics analyses, V(X, Y, Z) refers to nodal velocity, and A(X, Y, Z) refers to nodal acceleration. Although V(X, Y, Z) and A(X, Y, Z) appear as DOFs, they are not actually physical DOFs. However, these quantities are computed as DOF solutions and stored for postprocessing.

---

Real Constants

See Table 161.1: BEAM161 Real Constants for a description of the real constants.

Material Properties

TB command: See Element Support for Material Models for this element.

MP command: EX, NUXY, DENS, ALPD, BETD, DMPR

EDMP command: RIGID (KEYOPT(1) = 1,2)

Surface Loads

Pressure -- 

face 1 (I-J) (+r tangential direction), face 2 (I-J) (-s normal direction), face 3 (I) (-t normal direction)

Body Loads

None

Special Features

All nonlinear features allowed for an explicit dynamic analysis.

KEYOPT(1)

Element formulation:

0, 1 -- 

Hughes-Liu with cross section integration (default)

2 -- 

Belytschko-Schwer resultant beam (resultant)

4 -- 

Belytschko-Schwer full cross section integration

5 -- 

Belytschko-Schwer circular beam with cross section integration

KEYOPT(2)

Quadrature rule:

1 -- 

One integration point

0, 2 -- 

2 x 2 Gauss quadrature (default)

3 -- 

3 x 3 Gauss quadrature

4 -- 

3 x 3 Lobatto quadrature

5 -- 

4 x 4 Gauss quadrature

---

Note:  KEYOPT(2) is valid only with rectangular element formulations (KEYOPT(1) = 0, 1, 4).

---

KEYOPT(4)

Integration rule for section:

0 -- 

Standard integration option

n -- 

User-defined integration rule ID (valid range: 1 to 9999)

KEYOPT(5)

Cross section type:

0 -- 

Rectangular cross section

1 -- 

Circular cross section

2 -- 

Arbitrary cross section (user defined integration rule) or standard beam cross section, if KEYOPT (4) > 0.

Table 161.1:  BEAM161 Real Constants

No.	Name	Description	Use if...
1	SHRF	Shear factor. Default = 1.0 Recommended for rectangular sections = 5/6.	KEYOPT (1) = 0,1, 4, or 5
2	TS1	Beam thickness in s direction at node 1; if KEYOPT (5) = 2, then use for arbitrary cross section only.	KEYOPT (1) = 0, 1, or 4 KEYOPT (5) = 0 or 2
3	TS2	Beam thickness in s direction at node 2; if KEYOPT (5) = 2, then use for arbitrary cross section only.	KEYOPT (1) = 0, 1, or 4 KEYOPT (5) = 0 or 2
4	TT1	Beam thickness in t direction at node 1; if KEYOPT (5) = 2, then use for arbitrary cross section only.	KEYOPT (1) = 0, 1, or 4 KEYOPT (5) = 0 or 2
5	TT2	Beam thickness in t direction at node 2; if KEYOPT (5) = 2, then use for arbitrary cross section only.	KEYOPT (1) = 0, 1, or 4 KEYOPT (5) = 0 or 2
2	DS1	Beam outer diameter at node 1[1]	KEYOPT (1) = 0, 1, or 5 KEYOPT (4) = 0 KEYOPT (5) = 1
3	DS2	Beam outer diameter at node 2[1]	KEYOPT (1) = 0, 1, or 5 KEYOPT (4) = 0 KEYOPT (5) = 1
4	DT1	Beam inner diameter at node 1[1]	KEYOPT (1) = 0, 1, or 5 KEYOPT (4) = 0 KEYOPT (5) = 1
5	DT2	Beam inner diameter at node 2[1]	KEYOPT (1) = 0, 1, or 5 KEYOPT (4) = 0 KEYOPT (5) = 1
6	NSLOC	Location of reference surface normal to s-axis = 1 side at s = 1 = 0 center = -1 side at s = -1	KEYOPT (1) = 0, 1, 4, or 5 KEYOPT (4) = 0
7	NTLOC	Location of reference surface normal to t-axis = 1 side at t = 1 = 0 center = -1 side at t = -1	KEYOPT (1) = 0, 1, 4, or 5 KEYOPT (4) = 0
8	A	Cross sectional area See Table 161.2: Properties of Beam Cross Sections for Several Common Cross Sections	KEYOPT (4) = 0 KEYOPT (1) = 2
9	ISS	Moment of inertia about s-axis See Table 161.2: Properties of Beam Cross Sections for Several Common Cross Sections	KEYOPT (4) = 0 KEYOPT (1) = 2
10	ITT	Moment of inertia about t-axis See Table 161.2: Properties of Beam Cross Sections for Several Common Cross Sections	KEYOPT (4) = 0 KEYOPT (1) = 2
11	IRR	Polar moment of inertia See Table 161.2: Properties of Beam Cross Sections for Several Common Cross Sections	KEYOPT (4) = 0 KEYOPT (1) = 2
12	SA	Shear area See Table 161.2: Properties of Beam Cross Sections for Several Common Cross Sections	KEYOPT (4) = 0 KEYOPT (1) = 2
13	NIP	Number of integration points See Figure 161.5: Definition of Integration Points for User Defined Integration Rule	KEYOPT (4) > 0 and KEYOPT (5) = 2
14	RA	Relative area of cross section; that is, the actual cross-sectional area divided by the area defined by the product of the specified thickness in the s direction and the thickness in the t direction. See Figure 161.4: Definition of Relative Area for User Defined Integration Rule.	KEYOPT (4) > 0 and KEYOPT (5) = 2
15	ICST	Standard cross section type. Note:  If this type is nonzero, then NIP and RA should be zero. Cross section types are: 1 - W-section 2 - C-section 3 - Angle section 4 - T-section 5 - Rectangular tubing 6 - Z-section 7 - Trapezoidal section See Figure 161.2: Standard Beam Cross Sections, Figure 161.3: Standard Beam Cross Sections (continued).	KEYOPT (4) > 0[2] and KEYOPT (5) = 2 (standard cross section only)
16	W	Flange width	ICST > 0, and NIP = RA = 0
17	TF	Flange thickness	ICST > 0, and NIP = RA = 0
18	D	Depth	ICST > 0, and NIP = RA = 0
19	TW	Web thickness	ICST > 0, and NIP = RA = 0
20	SREF	Location of reference surface normal to s Note:  If KEYOPT (1) = 1 only	ICST > 0, and NIP = RA = 0
21	TREF	Location of reference surface normal to t Note:  If KEYOPT (1) = 1 only	ICST > 0, and NIP = RA = 0
22, 25, 28, ...79	S(i)	s coordinate of integration point i = 1, NIP (NIP = 20 max)[3]	KEYOPT (4) > 0 KEYOPT (5) = 2, arbitrary cross section only NIP > 0, RA > 0, ICST = 0
23, 26, 29, ...80	T(i)	t coordinate of integration point i = 1, NIP (NIP = 20 max)[3]	KEYOPT (4) > 0 KEYOPT (5) = 2, arbitrary cross section only NIP > 0, RA > 0, ICST = 0
24, 27, 30, ...81	WF(i)	Weighting factor; that is, the area associated with the integration point divided by the actual cross-section area. i = 1, NIP (NIP = 20 max)[3] See Table 161.2: Properties of Beam Cross Sections for Several Common Cross Sections	KEYOPT (4) > 0 KEYOPT (5) = 2, arbitrary cross section only NIP > 0, RA > 0, ICST = 0

1. DS1, DS2, DT1, and DT2 are used only if KEYOPT (5) = 1. If KEYOPT (5) = 0 or 2, then use TS1, TS2, TT1, and TT2.

2. For KEYOPT (5) = 2, standard cross-section type, the integration point ID (KEYOPT (4) > 0) is not used since NIP = RA = 0. However, you must provide this input in any case.

3. Specify S(i), T(i), and WF(i) for each integration point. For example, for 20 integration points, specify S(1), T(1), WF(1), S(2), T(2), WF(2), ... S(20), T(20), WF(20).

Table 161.2:  Properties of Beam Cross Sections for Several Common Cross Sections

Figure 161.4:  Definition of Relative Area for User Defined Integration Rule

Figure 161.5:  Definition of Integration Points for User Defined Integration Rule

BEAM161 Output Data

To store output data for this element, you first need to specify the number of integration points for which you want output data. Use the EDINT,,BEAMIP command during the solution phase of your analysis to specify the number of integration points. By default, output is written for 4 integration points. For the resultant beam formulation (KEYOPT(1) = 2), there is no stress output (regardless of the BEAMIP setting). If you set BEAMIP = 0, no stress output is written for any of the beam elements. In this case, the beams will not appear in any POST1 plots because the program assumes they are failed elements.

To display the data for BEAM161, you must use the ETABLE command. Then, you can use the PRETAB command to print the output data. The RSYS command has no effect when postprocessing output for this element.

The following items are available on the results file.

For each of these output data, one set of values, given at the centroid, is output for the entire beam.

Table 161.4: BEAM161 Item and Sequence Numbers lists output available through the ETABLE and ESOL commands 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. The following notation is used in Table 161.4: BEAM161 Item and Sequence Numbers:

BEAM161 Assumptions and Restrictions

BEAM161 Product Restrictions

There are no product-specific restrictions for this element.