4.161 BEAM161 Explicit 3-D Beam

• It is incrementally objective (rigid body rotations do not generate strains), allowing for the treatment of finite strains that occur in many practical applications.
• It is simple for computational efficiency and robustness.
• It is compatible with the brick elements.
• It includes finite transverse shear strains. However, the added computations needed to retain this strain component, compared to those for the assumption of no transverse shear strain, are significant.

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

Figure 4.161-1 BEAM161: Explicit 3-D Beam

4.161.1 Input Data

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 Chapter 7 of the ANSYS 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 Chapter 4 of 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 4.161-1. 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 any of four materials when working with BEAM161, with the restrictions as noted:

• Elastic
• Bilinear Kinematic (Except KEYOPT(1)=2)
• Plastic Kinematic, rate dependent (Except KEYOPT(1)=2)
• Viscoelastic (KEYOPT(1)=1 only)
• Power Law Plasticity (KEYOPT(1)=1 only)
• Piecewise Linear Plasticity (KEYOPT(1)=1 only)

KEYOPT(2) is valid only with rectangular element formulations (KEYOPT(1) = 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 4.161-2 Standard beam cross sections.

Figure 4.161-3 Standard beam cross sections.

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

A summary of the element input is given in Table 4.161-1. Additional information about real constants for this element is provided in Table 4.161-1a. For more information about this element, see the ANSYS/LS-DYNA User's Guide.

Table 4.161-1 BEAM161 Input Summary

Element Name	BEAM161
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 post-processing.
Real Constants	See Table 4.161-1a.
Material Properties	EX, NUXY, DENS, DAMP (MP command) RIGID (KEYOPT(1)=1,2) (EDMP command) BKIN, EVISC, PLAW (TB command; see Section 2.6)
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	This element supports all nonlinear features allowed for an explicit dynamics 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)	1 - One integration point 0, 2 - 2x2 Gauss quadrature (default) 3 - 3x3 Gauss quadrature 4 - 3x3 Lobatto quadrature 5 - 4x4 Gauss quadrature Note-KEYOPT(2) is valid only with rectangular element formulations (KEYOPT(1) = 1, 4).
KEYOPT(4)	0 - Standard integration option n - User-defined integration rule ID (valid range: 1 to 9999)
KEYOPT(5)	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.

No.	Name	Description	Use if...
1	SHRF	Shear factor. Default = 1.0 Recommended for rect. 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 11	KEYOPT (1) = 0, 1, or 5 KEYOPT (4) = 0 KEYOPT (5) = 1
3	DS2	Beam outer diameter at node 21	KEYOPT (1) = 0, 1, or 5 KEYOPT (4) = 0 KEYOPT (5) = 1
4	DT1	Beam inner diameter at node 11	KEYOPT (1) = 0, 1, or 5 KEYOPT (4) = 0 KEYOPT (5) = 1
5	DT2	Beam inner diameter at node 21	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	KEYOPT (4) = 0 KEYOPT (1) =2
9	ISS	Moment of inertia about about s-s axis	KEYOPT (4) = 0 KEYOPT (1) =2
10	ITT	Moment of inertia about about t-t axis	KEYOPT (4) = 0 KEYOPT (1) =2
11	IRR	Polar moment of inertia	KEYOPT (4) = 0 KEYOPT (1) =2
12	SA	Shear area	KEYOPT (4) = 0 KEYOPT (1) =2
13	NIP	Number of integration points	KEYOPT (4) > 0 and KEYOPT (5) = 2
14	RA	Relative area of cross section; i.e., 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 (4.161-3).	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 Figures 4.161-2, 4.161-3.	KEYOPT (4) > 02 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...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...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...81	WF(i)	Weighting factor; i.e., the area associated with the integration point divided by the actual cross section area. i = 1, NIP (NIP = 20 max)3 See Figure 4.161-4.	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 providethis 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).

Figure 4.161-4 Properties of beam cross section for several common cross sections.

Figure 4.161-5 Definition of relative area for user define integration rule.

Figure 4.161-6 Definition of integration points for user defined integration rule.

4.161.2 Output Data

To display the data for BEAM161, you must use the ETABLE command. Then, you can use the PRETAB command to print the output data.

A colon (:) in the Name column indicates the item can be accessed by the Component Name method [ETABLE, ESOL] (see Section 2.2.2). These items are available on the results file.

Table 4.161-2 BEAM161 Element Output Definitions

Name	Definition
S (r, rs, rt)	Stresses
EPEQ	Average equivalent plastic strain
EPEL	Average elastic strain
MFORr	Member force in the element coordinate system, r direction
N (s, t )	Out-of-plane (s, t) shear
M (s, t )	Element (s, t) moments
TORQ	Torsional resultant

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

Table 4.161-3 lists output available through the ETABLE command using the Sequence Number method. See Chapter 5 of the ANSYS Basic Analysis Procedures Guide and Section 2.2.2.2 of this manual for more information. The following notation is used in Table 4.161-3:

Name - output quantity as defined in the Table 4.161-2

Item - predetermined Item label for ETABLE command

E - sequence number for single-valued or constant element data

1st IP - sequence number for the first integration point

nth IP - sequence number for the nth integration point as defined by the EDINT command.

Name	Item	E	1st IP	nth IP
MFORr	SMISC	1	-	-
Ns	SMISC	2	-	-
Nt	SMISC	3	-	-
Ms	SMISC	4	-	-
Mt	SMISC	5	-	-
TORQ	SMISC	6	-	-
Sr	LS	-	1	5 x (n-1) +1
Srs	LS	-	2	5 x (n-1) +2
Srt	LS	-	3	5 x (n-1) +3
EPEQ	LS	-	4	5 x (n-1) +4
EPEL	LS	-	5	5 x (n-1) +5

1. In this table, n refers to the current integration point for which you want output data.

4.161.3 Assumptions and Restrictions

Warping of the cross section is unconstrained and is the same for all cross sections; therefore, the torsional rotation of the cross section is assumed to vary linearly along the length. However, warping is not applicable to the resultant beam formulation (KEYOPT(1)=2).

4.161.4 Product Restrictions