模拟方盒跌落过程的问题

useful

请教各位大虾：我想—— 模拟方盒跌落过程
目标：模拟内部装有1000kg重物的盒子在初始速度和重力作用下跌落到具有突起的刚性地面上的过程。采用单位：  质量 kg， 长度mm ，时间 ms
1 方盒采用shell  element
2重物采用mass element
3突起的刚性地面
遇到如下问题：
1.Mass 应该怎样创建，是不是在part里创建一个point，然后再在这个point上施加mass？可是我看帮助文档，Mass是施加在node上而并非point，可是在ABAQUS里不好像HM里一样直接创建node,不知该如何操作？
2.创建了mass后，mass 的node 是否还要和方盒地面node施加constraint（coupling）？
谢谢先！！！！！！！！！！！！

useful

怎么没人给个提示呢？我先发个模型上来，让大家看得清楚一些！

shaoxiaoj

1.质量可以加在一个set或者node上。
2.如果盒内还有其他重物，可以将重物建成刚体，然后将mass加在刚体的参考点上，然后定义重物、盒子、地面之间的接触就可以了。

Q.

你给的图片就是你要模拟的模型吗？

非要用mass element吗？我没有用过质量单元，不过你可以查看手册里面的例子。我的想法是，你就建立方盒模型，然后对其施加质量就可以了啊。

property功能模块－special－inertia

Q.

abaqus里面创建node的方法：

利用分割技术partition就可以

useful

原帖由 quhaibin 于 2007-3-6 13:14 发表
你给的图片就是你要模拟的模型吗？

非要用mass element吗？我没有用过质量单元，不过你可以查看手册里面的例子。我的想法是，你就建立方盒模型，然后对其施加质量就可以了啊。

property功能模块－special－ ...

这个方法我知道，我一开始建了一个REF-point，然后在REF-point上施加mass，进一步创建图示的约束，可是报错，错误提示的大概意思是说mass不能加在REF-point上，于是我又在part里创建了一个point，可是出现同样的错误，所以断定mass单元创建有无，可又不知该怎么创建？

shaoxiaoj

照我说的方法去做吧，没有问题的。有问题再提出来，我是专做跌落的。

ztmachine

我试了一下，没有碰到什么问题。

我觉的按照你的做法，将重物简化成质量点，和箱体couple起来，和实际情况是否吻合？箱中重物的分布和碰撞后的运动对箱体的响应的影响应该考评一下

shaoxiaoj

除非重物不均质，否则这样做是没有问题的。

shaoxiaoj

原帖由 ztmachine 于 2007-3-6 14:35 发表
我试了一下，没有碰到什么问题。

我觉的按照你的做法，将重物简化成质量点，和箱体couple起来，和实际情况是否吻合？箱中重物的分布和碰撞后的运动对箱体的响应的影响应该考评一下

假如有几个重物，则要分开建立模型，如果还要考察重物的受力或者相应，那就不能建刚体。建刚体的目的有：1.在不需要了解重物的响应的情况下；2.简化模型，减少网格数量，提高计算效率；3.要了解重物的加速度情况；

useful

我只想方盒经过跌落以后的变形和应力，不考察重物，所以建立刚体，再在刚体参考点上施加mass应该是可以的。但如果盒内装的是液体（如水），不知能不能用质量点来简化模型，请大家赐教。

shaoxiaoj

原帖由 useful 于 2007-3-6 16:01 发表
我只想方盒经过跌落以后的变形和应力，不考察重物，所以建立刚体，再在刚体参考点上施加mass应该是可以的。但如果盒内装的是液体（如水），不知能不能用质量点来简化模型，请大家赐教。

这个问题比较好，我还没有做过液体质量的分析，不过abaqus example中似乎有一个是水的例子，可以参考一下。如果是水的话，我自己认为用质点简化模型结果可能会不准确。

useful

这个问题我已解决了，就是在方盒底部选了一个SET，然后再上面加了MASS，结果也比较合理，最大Mises应力达到235MPa，正好是Q235钢的屈服应力。可是如果方盒里装水的话问题好像比较复杂，但如果得到各位大虾的指点，我想也能够解决的。

useful

先把CAE文件上传，有兴趣的朋友也可以当个例子去做一下。特别是盒子里装水跌落的问题。

shock111

复杂点模拟盒子里有水的跌落问题,可以采用EOS来描述水

这个国内是有成功案例的,大的储油罐的跌落,模拟结果和实验结果符合的非常好

shaoxiaoj

我在abaqus benchmarks manual中找到一个eos的例子，大家一起看看：
*HEADING
ADAPTIVE MESHING VERIFICATION
SHOCK WAVE THROUGH WATER
Units: N, m, sec
*RESTART,TIMEMARKS=NO,WRITE,NUM=6
*NODE
1,5.,0.,3.0
100,5.0,0.,30.6
501,0.0,0.0,3.0
600,0.0,0.0,30.6
1001,5.,-.575,3.00
1100,5.,-.575,30.6
1501,0.0,-.575,3.00
1600,0.0,-.575,30.6
*NGEN,NSET=RBOTEU
1,501,100
*NGEN,NSET=LBOTEU
100,600,100
*NFILL,NSET=BOTEU
RBOTEU,LBOTEU,99,1
*NGEN,NSET=RTOPEU
1001,1501,100
*NGEN,NSET=LTOPEU
1100,1600,100
*NFILL,NSET=TOPEU
RTOPEU,LTOPEU,99,1
*NSET,NSET=EULER
RBOTEU,LBOTEU,RTOPEU,LTOPEU,
*NSET,NSET=NALLEU
BOTEU,TOPEU
*ELEMENT,TYPE=C3D8R,ELSET=WATEREU
1,1,101,1101,1001,2,102,1102,1002
*ELGEN,ELSET=WATEREU
1,99,1,1,5,100,99,
*ELSET, ELSET=EULER1
1,100,199,298,397
*ELSET, ELSET=EULER2
99,198,297,396,495
*******************
*NODE
10001,5.,2.0,3.00
10100,5.0,2.0,30.6
10501,0.0,2.0,3.00
10600,0.0,2.0,30.6
11001,5.,1.425,3.00
11100,5.,1.425,30.6
11501,0.0,1.425,3.00
11600,0.0,1.425,30.6
*NGEN,NSET=RBOTLAG
10001,10501,100
*NGEN,NSET=LBOTLAG
10100,10600,100
*NFILL,NSET=BOTLAG
RBOTLAG,LBOTLAG,99,1
*NGEN,NSET=RTOPLAG
11001,11501,100
*NGEN,NSET=LTOPLAG
11100,11600,100
*NFILL,NSET=TOPLAG
RTOPLAG,LTOPLAG,99,1
*NSET,NSET=NALLLAG
BOTLAG,TOPLAG
*ELEMENT,TYPE=C3D8R,ELSET=WATERLAG
10000,10001,10101,11101,11001,10002,10102,11102,11002
*ELGEN,ELSET=WATERLAG
10000,99,1,1,5,100,99,
*******************
*SOLID SECTION,ELSET=WATEREU,MATERIAL=WATER, CONTROL=SECTEU
*SECTION CONTROLS, NAME=SECTEU,HOURGLASS=STIFFNESS
*SOLID SECTION,ELSET=WATERLAG,MATERIAL=WATER, CONTROL=SECTLAG
*SECTION CONTROLS, NAME=SECTLAG,HOURGLASS=STIFFNESS
*MATERIAL,NAME=WATER
*EOS,TYPE=USUP
1450.6,0.0,0.0,0.0
*DENSITY
983.2,
*NSET,NSET=OUT
1,101,25,50,75,
10001,10101,10025,10050,10075
*NSET,NSET=XSYM1,GEN
501,600,1
1501,1600,1
10501,10600,1
11501,11600,1
*NSET,NSET=XSYM2,GEN
401,500,1
1401,1500,1
10401,10500,1
11401,11500,1
*NSET,NSET=XSYM3,GEN
301,400,1
1301,1400,1
10301,10400,1
11301,11400,1
*NSET,NSET=XSYM4,GEN
201,300,1
1201,1300,1
10201,10300,1
11201,11300,1
*NSET,NSET=XSYM5,GEN
101,200,1
1101,1200,1
10101,10200,1
11101,11200,1
*NSET,NSET=XSYM6,GEN
1,100,1
1001,1100,1
10001,10100,1
11001,11100,1
*NSET,NSET=YSYM1,GEN
1,100,1
101,200,1
201,300,1
301,400,1
401,500,1
501,600,1
10001,10100,1
10101,10200,1
10201,10300,1
10301,10400,1
10401,10500,1
10501,10600,1
*NSET,NSET=YSYM2,GEN
1001,1100,1
1101,1200,1
1201,1300,1
1301,1400,1
1401,1500,1
1501,1600,1
11001,11100,1
11101,11200,1
11201,11300,1
11301,11400,1
11401,11500,1
11501,11600,1
*BOUNDARY
XSYM1,XSYMM
XSYM6,XSYMM
YSYM1,YSYMM
YSYM2,YSYMM
*AMPLITUDE, DEFINITION=SMOOTH STEP,NAME=AMP,TIME=TOTAL TIME
0.0, 57.14, 12.E-4, 492.14,24.E-4, 57.14,1.0, 57.14
*INITIAL CONDITIONS, TYPE=VELOCITY
NALLLAG,3,57.14
NALLEU,3,57.14
*ELSET,ELSET=OUT,GEN
1,10,1
10000,10009,1
*SURFACE,TYPE=ELEMENT, NAME=EULER2, REGION TYPE=EULERIAN
EULER2,S2
*ELSET,ELSET=QA_TEST_OUT
OUT,
*NSET,NSET=QA_TEST_OUT
OUT,
**
*STEP
*DYNAMIC,EXPLICIT
,60.E-4
*BOUNDARY,TYPE=VELOCITY,AMPLITUDE=AMP
1,3,3,1.0
101,3,3,1.0
201,3,3,1.0
301,3,3,1.0
401,3,3,1.0
501,3,3,1.0
1001,3,3,1.0
1101,3,3,1.0
1201,3,3,1.0
1301,3,3,1.0
1401,3,3,1.0
1501,3,3,1.0
10001,3,3,1.0
10101,3,3,1.0
10201,3,3,1.0
10301,3,3,1.0
10401,3,3,1.0
10501,3,3,1.0
11001,3,3,1.0
11101,3,3,1.0
11201,3,3,1.0
11301,3,3,1.0
11401,3,3,1.0
11501,3,3,1.0
*FILE OUTPUT, NUMBER=2, TIME MARKS=YES
*EL FILE,ELSET=OUT
PRESS
*NODE FILE,NSET=OUT
U,
***OUTPUT,HISTORY,TIME INTERVAL=1.E-4
***ELEMENT OUTPUT,ELSET=OUT
**S,PRESS
***NODE OUTPUT,NSET=OUT
**U,V
***ENERGY OUTPUT
**ALLKE,ALLIE,ALLAE,ALLVD,ALLWK,ETOTAL,
**DT,
*OUTPUT,FIELD,NUMBER INTERVAL=2,VARIABLE=PRESELECT
*OUTPUT, FIELD, NUMBER INTERVAL=2, TIMEMARKS=YES
*ELEMENT OUTPUT, ELSET=QA_TEST_OUT
PRESS
*NODE OUTPUT, NSET=QA_TEST_OUT
U,
*OUTPUT,HISTORY,VARIABLE=PRESELECT,TIMEINT=0.003
*END STEP
*STEP
*DYNAMIC,EXPLICIT
,1.15E-2
*BOUNDARY,TYPE=VELOCITY,AMPLITUDE=AMP,REGION TYPE=EULERIAN
1,3,3,1.0
101,3,3,1.0
201,3,3,1.0
301,3,3,1.0
401,3,3,1.0
501,3,3,1.0
1001,3,3,1.0
1101,3,3,1.0
1201,3,3,1.0
1301,3,3,1.0
1401,3,3,1.0
1501,3,3,1.0
*ADAPTIVE MESH,ELSET=WATEREU,CONTROLS=UPDATED,FREQUENCY=1,
INITIAL MESH SWEEPS=1,MESH SWEEPS=1
*ADAPTIVE MESH CONSTRAINT
EULER,3,3, 0.0
*ADAPTIVE MESH CONTROLS,NAME=UPDATED,
MOMENTUM ADVECTION=HALF INDEX SHIFT,MESHING PREDICTOR=PREVIOUS
*FILE OUTPUT, NUMBER=2, TIME MARKS=YES
*EL FILE,ELSET=OUT
PRESS
*NODE FILE,NSET=OUT
U,
*OUTPUT, FIELD, NUMBER INTERVAL=2, TIMEMARKS=YES
*ELEMENT OUTPUT, ELSET=QA_TEST_OUT
PRESS
*NODE OUTPUT, NSET=QA_TEST_OUT
U,
*OUTPUT,HISTORY,VARIABLE=PRESELECT,TIMEINT=0.00575
*END STEP

shaoxiaoj

以下是上面那个inp的问题描述：
Problem description

The model consists of a bar through which a one-dimensional wave is propagated. The bar is given an initial rigid body velocity of 57.14 m/sec in the positive x-direction. The analysis is run in two steps. In the first step a hat-shaped velocity pulse is defined at the left end of the bar, and a wave form is generated. In the second step the velocity at the left end of the bar is held constant at 57.14 m/sec, and the wave propagates through the bar. The wavelength of the pulse is chosen to be relatively short (over about 10 elements) for a more severe test of the advection algorithms applied to wave propagation. Problems with wavelengths that span large numbers of elements are not as difficult because overall diffusion and dispersion effects are less pronounced.

Two different techniques are used to solve the problem and are shown schematically in Figure 1.11.2–1.


Both steps are run as a pure Lagrangian analysis.

The first step is run as a pure Lagrangian analysis to generate the wave form. The second step is run in an Eulerian fashion by defining an adaptive mesh domain that incorporates the bar. Eulerian boundaries are defined at either end of the bar. Adaptive mesh constraints are used to hold the mesh in place at both the inflow and outflow boundaries. The mesh is held stationary on the interior of the domain by using the MESHING PREDICTOR=PREVIOUS setting on the *ADAPTIVE MESH CONTROLS option (the default for Eulerian adaptive mesh domains). The mesh is pulled back to its position after the last adaptive mesh increment, which has the effect of holding the mesh stationary for a uniform mesh with no boundary deformation. The MOMENTUM ADVECTION parameter on the *ADAPTIVE MESH CONTROLS option is changed from the default value, ELEMENT CENTER PROJECTION, to HALF INDEX SHIFT because a more accurate momentum advection technique is desirable for wave propagation problems such as these. Although the differences in the two methods are very slight for this problem, the half-index shift is expected to lead to marginally better dispersion characteristics than the element center projection.



Three different geometric models with three different material behaviors for each model are analyzed for both cases. In the two-dimensional, plane strain model the bar measures 27.6 m in length by 0.575 m in width. In the axisymmetric model the bar measures 27.6 m axially (length direction) by 0.575 m radially. In the three-dimensional model the bar measures 27.6 m in length, .575 m in width, and 5 m in depth. For all models the wave is propagated through the bar in the length direction.

The material models used in each analysis include an equation of state having the properties of water, a Mooney-Rivlin hyperelastic material having the properties of rubber, and a von Mises elastic-plastic material having the properties of steel. The parameters and constants used for each material model can be found in the input files that are included with the ABAQUS release. The maximum velocities of the wave pulse in the water, the rubber, and the steel are 492, 28, and 250 m/sec (Mach 0.3, 0.12, and 0.035), respectively. These velocities are typical for shock waves traveling through each type of material.

orange_zz

学习了

hrx

学习了 3x

sunset123123

lz的模型我这边算不了 啊