Release 10.0 Documentation for ANSYS

BEAM188

3-D Linear Finite Strain Beam 三维线性有限应变梁单元

BEAM188 Element Description BEAM188单元描述

BEAM188 is suitable for analyzing slender to moderately stubby/thick beam structures. This element is based on Timoshenko beam theory. Shear deformation effects are included.

Beam188 单元适合于分析从细长到中等粗短的梁结构，该单元基于铁木辛哥梁结构理论，并考虑了剪切变形的影响。

BEAM188 is a linear (2-node) or a quadratic beam element in 3-D. BEAM188 has six or seven degrees of freedom at each node, with the number of degrees of freedom depending on the value of KEYOPT(1). When KEYOPT(1) = 0 (the default), six degrees of freedom occur at each node. These include translations in the x, y, and z directions and rotations about the x, y, and z directions. When KEYOPT(1) = 1, a seventh degree of freedom (warping magnitude) is also considered. This element is well-suited for linear, large rotation, and/or large strain nonlinear applications.

Beam188 是三维线性（2 节点）或者二次梁单元。每个节点有六个或者七个自由度，自由度的个数取决于KEYOPT(1)的值。当KEYOPT(1)＝0（缺省）时，每个节点有六个自由度；包括节点坐标系的x、y、z 方向的平动和绕x、y、z 轴的转动。当KEYOPT(1)=1 时，每个节点有七个自由度，这时引入了第七个自由度（横截面的翘曲）。这个单元非常适合线性、大角度转动以及大应变等非线性问题。

BEAM188 includes stress stiffness terms, by default, in any analysis with

NLGEOM,ON. The provided stress stiffness terms enable the elements to analyze flexural, lateral, and torsional stability problems (using eigenvalue buckling or collapse studies with arc length methods).

当NLGEOM 选项打开的时候，beam188 的应力刚化，在任何分析中都是缺省项。应力刚化选项使本单元能分析弯曲、横向及扭转稳定问题（用弧长法分析特征值屈曲和塌陷）。

BEAM188 can be used with any beam cross-section defined via SECTYPE, SECDATA, SECOFFSET, SECWRITE, and SECREAD. The cross-section associated with the beam may be linearly tapered. Elasticity, creep, and plasticity models are supported (irrespective of cross-section subtype). A cross-section

associated with this element type can be a built-up section referencing more than one material.

Beam188可以采用sectype、secdata、secoffset、secwrite 及secread 命令定义横截面。本单元支持弹性、蠕变及塑性模型（不考虑横截面子模型）。这种单元类型的截面可以由不同材料组成。

BEAM188 ignores any real constant data beginning with Release 6.0. See the SECCONTROLS command for defining the transverse shear stiffness, and added mass.

Beam188 从6.0 版本开始忽略任何实常数，参考seccontrols 命令来定义横向剪切刚度和附加质量。

For BEAM188, the element coordinate system (/PSYMB,ESYS) is not relevant.

单元坐标系统（/psymb，esys）与beam188 单元无关。

Figure 188.1: BEAM188 Geometry 图188.1：Beam188 单元几何示意图

BEAM188 Input Data

BEAM188 输入数据

The geometry, node locations, and coordinate system for this element are shown in Figure 188.1: \. BEAM188 is defined by nodes I and J in the global coordinate system.

该单元的几何形状、节点位置、坐标体系如图188.1 “Beam188 单元几何示意图”所示，beam188 由整体坐标系的节点I 和J 定义。

Node K is a preferred way to define the orientation of the element. For information about orientation nodes and beam meshing, see Generating a Beam Mesh With Orientation Nodes in the ANSYS Modeling and Meshing Guide. See the LMESH and LATT command descriptions for details on generating the K node automatically.

节点K 是定义单元方向的首选方式，有关方向节点和梁的网格划分的信息可以参见ANSYS Modeling and Meshing Guide中的Generating a Beam Mesh With Orientation Nodes。参考LMESH和LATT命令描述可以得到k 节点自动生成的详细资料。

BEAM188 may also be defined without the orientation node. In this case, the element x-axis is oriented from node I (end 1) toward node J (end 2). For the two-node option, the default orientation of the element y-axis is automatically calculated to be parallel to the global X-Y plane. For the case where the element is parallel to the global Z-axis (or within a 0.01 percent slope of it), the element y-axis is oriented parallel to the global Y-axis (as shown). For user control of the element orientation about the element x-axis, use the third node option. If both are defined, the third node option takes precedence. The third node (K), if used, defines a plane (with I and J) containing the element x and z-axes (as shown). If this element is used in a large deflection analysis, it should be noted that the location of the third node (K) is used only to initially orient the element.

Beam188 也以在没有方向节点的情况下被定义。在这种情况下，单元的x 轴方向为I 节点指向J节点。对于两节点的情况，默认的y 轴方向按平行x－y 平面自动计算。对于单元平行与z 轴的情况（或者斜度在0.01％以内），单元的y 轴的方向平行与整体坐标的y 轴（如图188.1）。用第三个节点的选项，用户可以定义单元的x 轴方向。如果两者都定义了，那么第三节点的选项优先考虑。第三个节点（K）如果采用的话，将和I、J 节点一起定义包含单元x 轴和z 轴的平面(如图188.1)。如果该单元采用大变形分析，需要注意这个第三号节点仅仅在定义初始单元方向的时候有效。

The beam elements are one-dimensional line elements in space. The cross-section details are provided separately using the SECTYPE and SECDATA commands (see Beam Analysis and Cross Sections in the ANSYS Structural Analysis Guide for

details). A section is associated with the beam elements by specifying the section ID number (SECNUM). A section number is an independent element attribute. In addition to a constant cross-section, you can also define a tapered cross-section by using the TAPER option on the SECTYPE command (see Defining a Tapered Beam).

梁单元是一维空间线单元。横截面资料用sectype和secdata 命令分别提供，参见ANSYS Structural Analysis Guide 的Beam Analysis and Cross Sections 看详细资料。截面与单元用截面ID 号（SECNUM）来关联，截面号是独立的单元属性。除了等截面，还可以用sectype 命令中的锥形选项来定义楔形截面（参考Defining a Tapered Beam）。

The beam elements are based on Timoshenko beam theory, which is a first order

shear deformation theory: transverse shear strain is constant through the cross-section; that is, cross-sections remain plane and undistorted after deformation. BEAM188 is a first order Timoshenko beam element which uses one point of integration along the length with default KEYOPT(3) setting. Therefore, when SMISC quantities are

requested at nodes I and J, the centroidal values are reported for both end nodes. With KEYOPT(3) set to 2, two points of integration are used resulting in linear variation along the length.

单元基于铁木辛哥梁理论，这个理论是一阶剪切变形理论；横向剪切应力在横截面是不变的，也就是说变形后横截面保持平面不发生扭曲。Beam188 是一阶铁木辛哥梁单元，沿着长度用了一个积分点，用默认的KEYOPT(3)设置。因此，在I 和J 节点要求SMISC 数值的时候，中间数值在两端节点均输出。当KEYOPT（1） 设置为2，两个积分点作为延长的线性变量被运用。

BEAM188 lements can be used for slender or stout beams. Due to the limitations of first order shear deformation theory, only moderately \The slenderness ratio of a beam structure (GAL2/(EI)) may be used in judging the applicability of the element, where:

Beam188单元可以用在细长或者短粗的梁。由于一阶剪切变形的限制，只有适度的“粗”梁可以分析。梁的长细比（GAL2/(EI))可以用来判定单元的适用性，式中：

G

Shear modulus 剪切模量 A

Area of the cross section 截面积 L

Length of the member 构件长度