ABAQUS中Truss单元预应力的两种施加方法

ABAQUS中预应力Truss单元的两种实现方法

例题：

100 m 长钢缆水平放置从 x = 0到 x = 100。两端固定。无初始拉力，计算下垂量。 截面； A = 0.01539 m2，Density: r =7800 kg/m3, g = 9.8 m/s2,E=2.1e+11 N/m2 Analytical solution of maximum displacement (u2) at x = 50m : U2_max = -((3*r*g*L^4)/(64*E))^(1/3) = -1.194944005 m

方法一. 沿 truss element 加沿长度方向初始拉应力 (see job-1.inp)

此文件中使用了initial condition, type = stress方法加初始拉应力。因工程上无此初应力, 更好的方法是使用降温法。算完后再升温。用降温法。算完后再升温。 NOTE: 降温法施加预应力（激活钢绞线）。温度=-力/（膨胀系数*弹模*钢绞线面积）

1、第一步，在truss单元中施加一个初始应力，让计算处于初始平衡状态；初始应力设置过小，可能不收敛，应多次试算，找到一个合理的应力值。一般情况下，这个初始值对最终值的影响不大，可以忽略。

2、第二步，施加truss单元的自重荷载，打开非线性开关（nlgeom=YES ）考虑几何非线性问题；

3、本例中初始值采用0.1Mpa。自重作用下缆索的拉应力约为80Mpa。最大位移为 -1.195 m，与理论计算值吻合得很好。 *Heading

Cable appling gravity load with initail stress

The maximum Analytical displacement without initail stress (at x = 50 m) U2 = -1.194944005 meter **

** Method 1. Using * initial condition,type = stress method **

*Preprint, echo=NO, model=NO, history=NO, contact=NO *Node

1, 0., 0. 101, 100., 0.

*NGEN, NSET = NALL 1, 101, 1

*Element, type=T2D2 1, 1, 2

*ELGEN, elset = ELALL 1, 100, 1

*ELSET,ELSET=EL_OUT 1, 51, 100

*Solid Section, elset=ELALL, material=steel 0.01539, **

*Nset, nset=Left 1,

*Nset, nset=right 101,

*Nset, nset=mid 51, **

** MATERIALS **

*Material, name=steel *Density 7800., *Elastic 2.1e+11, 0.3

*initial condition, type = stress

** Note: the solution will not converge as the initial stress < 100,000 N/m^2 ELALL, 100000 *Boundary Left, 1, 2 Right, 1,2

*Step, name=Step-0, inc=1000 Initial stress equilibrium

*Static 1, 1., 1e-05, 1.

*Output, field, variable=PRESELECT *Output, history, variable=PRESELECT *Node print, nset = mid, freq = 1000 U,

*EL PRINT, ELSET=EL_OUT, freq = 1000 S

*END STEP

** ---------------------------------------------------------------- **

** STEP: Step-1 **

*Step, name=Step-1, nlgeom=YES, inc=1000 Apply gravity load *Static

0.01, 1., 1e-05, 1.

** Name: GRAVITY-1 Type: Gravity *Dload

ELALL, GRAV, 9.8, 0., -1. **

** OUTPUT REQUESTS **

*Restart, write, number interval=1, time marks=NO *Output, field, variable=PRESELECT *Output, history, variable=PRESELECT *Node print, nset = mid, freq = 1000 U,

*EL PRINT, ELSET=EL_OUT, freq = 1000 S *End Step

方法二. 使用 STABILIZE parameter on the *STATIC.(see job-2.inp)

“stabilization” 在结构上附加artificial viscous damping（粘滞阻尼），使得计算结果to go beyond the instability point。但计算结果必须验证，并必须保证 ALLSD 比内能ALLIE 小很多。 NOTE:

1. 第一步用*Static, stabilize=2E-10。笫二步不用stabilize (相当于*Static, stabilize=0)。

2. 使用nlgeom=YES in the step to apply the gravity load. 3. 最终拉应力 = 8E7 N/m2 与方法一相等。

4. The maximum displacement (at node 51) equals the analytical result.

5. Check the ALLSD and ALLIE. The ALLIE is greater than ALLSD. (See figure 1)

6. The deformation shape of the cable can be examined by CAE. It may need to set the deformation scale factor to a large number (10 – 1000).

7. 使用此法必须极端谨慎。稍微不慎，结果会完全不对。For example, 用*Static, stabilize=2E-4 (default value of the stabilize parameter)重算此题。其结果如下；. Check the ALLSD and ALLIE. The ALLIE is less than ALLSD. (See figure 2) The deformation shape with deformation scale factor 1000 is shown in figure 3. In the figure, only the first and last elements are deformed. The maximum deformation value is not correct.

使用 stabilize parameter 学问很多，一般是越小越好。因为stabilize parameter 是 artificial value, 无法确定理论上的最佳值。我是用试错法。从开始 default value (2.0e-4) 往下减 (2.E-6, 2.0E-8,..)，直到不收敛 (2.0E-12). 经过验证结果 (see the note 4, 5, and 6)，我决定在计算中使用 2.0E-10。 *Heading

Cable apply gravity load using stabilize parameter

The maximum Analytical displacement without initail stress (at x = 50 m) U2 = 1.194944005 meter **

** Method 2. Using *Static, stabilize method **

*Preprint, echo=NO, model=NO, history=NO, contact=NO *Node

1, 0., 0. 101, 100., 0. *NGEN, NSET = NALL 1, 101, 1

*Element, type=T2D2 1, 1, 2

*ELGEN, elset = ELALL 1, 100, 1

*ELSET,ELSET=EL_OUT 1, 51, 100

*Solid Section, elset=ELALL, material=steel 0.01539, **

*Nset, nset=Left 1,

*Nset, nset=right 101,

*Nset, nset=mid 51, **

** MATERIALS **

*Material, name=Steel *Density 7800., *Elastic 2.1e+11, 0.3 *Boundary Left, 1, 2 Right, 1,2 **

** STEP: Step-1 **

*Step, name=Step-1, nlgeom=YES, inc=1000 Apply gravity load

** the default value of stabilize value is 2.0E-4 **Static, stabilize=2E-4 *Static, stabilize=2E-10 0.01, 1., 1e-05, 1.

** Name: GRAVITY-1 Type: Gravity *Dload

ELALL, GRAV, 9.8, 0., -1. **

** OUTPUT REQUESTS **

*Restart, write, number interval=1, time marks=NO *Output, field, variable=PRESELECT *Output, history, variable=PRESELECT ALLSD , ALLIE

*Node print, nset = mid, freq = 1000 U,

*EL PRINT, ELSET=EL_OUT, freq = 1000 S *End Step **

*Step, name=Step-2, nlgeom=YES, inc=1000 Recovery *Static

0.01, 1., 1e-05, 1. *End Step