[Ls dyna] 单元和结果局部坐标系
2012-11-07 20:41阅读：
简要理顺下：
1.壳单元坐标系：局部坐标系x为节点1到节点2的方向；局部坐标系z为法线方向；
局部坐标系y=z叉乘x，x=y叉乘z
所以在分析壳单元时保证局部坐标系保持一致是非常重要的，这样有利于后处理结果的解读；
2.结果
（1）实体和厚壳的结果是基于整体坐标系；
（2）梁单元的应力和合力结果均基于局部坐标系；
（3）壳单元的应力应变，在D3PLOT结果中是基于整体坐标系；ELOUT是基于单元坐标系；
在LSPP进行D3PLOT后处理时，有三种设置方法，可以将壳单元的结果转变为基于单元坐标系：（a）在VIew-》激活Local
axes；（b）在Fcomp底部设置Local；（3）在History中设置E-axes-Local。
（4）注意，对正交各向异性材料的壳、厚壳和实体单元，当*DATABASE_EXTENT_BINARY中设置CM
PFLG为1时,单元的应力应变将以材料的局部坐标系结果输出，但是在LSPP后处理中不能将材料的局部坐标系转变为单元局部坐标系。
Coordinate system for stress
Shell stresses are reported at through-thickness integration
points. Location of those integration points depend on the number
of integration points and the type of integration rule used, e. g.,
Gaussian, Lobatto, trapezoidal, user-defined rule (see NIP and
QR/IRID in *SECTION_SHELL).
Fully-integrated shell formulations have 4 in-plane integration
points at each through-thickness location. For these formulations,
the 4 values of each stress component are averaged before being
written.
Shell stresses can be shown in the global, element, or material
coordinate systems. By default, shell stresses/strains written to
D3PLOT are global; shell stresses/strains written to
ELOUT are in the element local coordinate system
(except for the case of linear analysis with shell formulations
18,20,21, in which case stresses are in the global system OR when
NSOLVR=1 in *CONTROL_IMPLICIT_SOLUTION).
Shell stresses/strains from D3PLOT are converted by
LS-Prepost to the shell element coordinate system, if you select
Toggle > Local axes on from the top menu bar or,
alternately, choose E-axes > Local when plotting
element time histories or, in the case of fringe plots, switch to
Local by clicking on the Glob button at the bottom of the
FCOMP menu. The element local coordinate system of a
shell is defined as local-x = node 1 to node 2. Local z is normal
to the shell.
By default, stresses/strains for solids and thick shells are
written to D3PLOT and ELOUT in the global
coordinate system. Stresses and resultants for beams are written to
D3PLOT and ELOUT in the element
coordinate system.
For shells, solids, and thick shells comprised of orthotropic
materials, stresses/strains are written to all databases in the
material coordinate system if CMPFLG is set to 1 in
*DATABASE_EXTENT_BINARY. (Do NOT toggle to local in
LS-Prepost if you use this option.) The material coordinate system
varies from integration point to integration point within a shell
element based on the beta angles given in
*SECTION_SHELL.
Summary:
For shells, you can view stresses/strains in the the global
coordinate system, in the local element coordinate system
(determined solely by element connectivity, i. e., N1-to-N2 is the
element x-direction), or (if material is orthotropic and
CMPFLG=1 in *DATABASE_EXTENT_BINARY) in
the material coordinate system.
For solids or thick shells, you can view stresses/strains in the
the global coordinate system or (if material is orthotropic and
CMPFLG=1 in *DATABASE_EXTENT_BINARY) in
the material coordinate system.
