http://okok.org/cgi-bin/english/topic_show.cgi?id=21058&bpg=324&age=30
外包各向异性的复合材料加固。为了对其进行建模分析，用8结点实体 单元模拟砼，用层状壳单元模拟外包各向异性的复合材料，曾经考虑过用SOLID46，但本例中是一空心复合材料纵梁内填砼，且纵梁上又是全复合材料的桥 面，要用SHELL99来模拟，此时就出现了自由度耦合的问题了，应该是可以用约束方程实现耦合的，但这种方程应如何写出，例如对此例，要怎么写才能满足 自由度耦合的要求呢？？请各位大虾指教!
说明：此图中，最上面一层即是全复合材料的桥面，截面形式如下边所示，但是垂直于交通方向。下面即为纵梁，但主要考虑的是第一个方案。
有一个办法，你可以用层状实体元，solid46，可以有250层不同材料啊，自由度与混凝土就完全一样了。
你的问题在普通的cae软件中是一个很有代表性的问题，在ansys中可以通过两种办法解决：
1，直接将壳单元的边节点和实体单元的边节点连接，这种方式对连接区的应力求解结果精度影响很大，往往的到的结果是没有实际意义的。
2，通过设定藕荷方程来求解，具体内容较多，你可以参考ansys教程《建模与分网指南>>第十二章 耦合与约束方程。
就我目前应用过的cae软件中，对该问题解决得比较完美的应该是adina，该程序提供了一个过渡单元来解决此类耦合问题，精度较高。
Posted on 2003-06-18 06:40
这里有一篇讲的比较完整的文章.
另外, 据说ANSYS7.1里可以用MPC184来连接SHELL和SOLID; 但要等到7.1出来后才能证实了.
To ansys-forum@listbox.cern.ch
From Alberto Desirelli <Alberto.Desirelli@cern.ch>
Date Mon, 8 Jul 2002 11:55:00 +0200 (CEST)
FEA WITH SOLID AND SHELL ELEMENTS
It has recently come to my attention that some stress FEA done over the past few years using Ansys solid and shell elements might have at times been carried out in an erroneous way. This misuse of solid and shell elements generally results into lower stress values and higher displacement values.
It is not infrequent when doing FE modelling to use solid and shell elements together. In these cases care must be taken at the interface between the two element types. This is because, unlike shell elements, most solid elements do not have rotational DOFs. Constraint equations must therefore be used to relate the shell rotations to the solid translations. If this is not done the interface nodes will work like a hinge, the shell elements will be able to pivot around it and to undergo a
rigid-body rotation at the interface.
Contrary to what is sometimes assumed, this also happens, but in a slightly different way, when interfacing solid elements, which do have rotational DOFs like SOLID72 and SOLID73, with shell elements.
SOLID72 and SOLID73 (undocumented in ANSYS 5.7) When people encountered the rotational DOF of SOLID72 and SOLID73 they naturally thought that these element were 'designed' to work with shells and beams. However this was not the case and people were reminded of the possible 'side-effect' of their usage with shells and beams, which was discussed in the element reference manual.
Please find attached below three articles from ANSYS for your reference and the recommendation on how to work with shell/beam with solids.
1. A LITTLE TREATISE ON SOLID72 AND SOLID73
These elements were developed long ago in order to overcome a weakness of the wavefront solver (then the only solver option in ANSYS) in relation to midside-node elements (SOLID92 and SOLID95). Midside-node elements create relatively large wavefronts compared to corner-noded elements, and with the usage of automatic test meshers that were coming of age at that time, it was a big issue. Now that we offer the sparse and PCG solvers, this issue is no longer a concern and the justification for SOLID72 and SOLID3 has disappeared.
Because SOLID72 and SOLID73 have rotational DOFs, they appear attractive to mix with shells and beams. However, the rotational DOFs do have anomalies. The rotational DOFs provide the quadratic bending along an edge like a midside node does, however, there are spurious deformations (such as all rotational DOFs having equal rotations) that must be accounted for. This is done akin to the addition of weak rotational springs we add to SHELL63 out-of-plane (drilling) DOF. For example, if you add a pipe sticking straight out from a SHELL63 element and apply a torque to it, there would be no resistance to this from the SHELL63. Therefore, you must use extreme care when using SOLID72 and 73 elements and either applying moments to them or attaching them to shells or beams. The ANSYS Elements Reference manual covers these concerns in the Assumptions and Restrictions sections of those elements.
Because they are obsolete and cause much confusion over their rotational DOF, we are planning to undocument SOLID72 and SOLID73 at ANSYS 5.7.
2. FAQ ON THE USE OF SHELLS AND SOLIDS
Q: Is there a recommended way to connect a 3-DOF solid element to a 6-DOF-shell element?
A: It is difficult to answer this question without knowing the intended application, but we can give some guidelines:
1. Use compatible elements; for example, SHELL63 on SOLID45, or SHELL93 on SOLID95. Do not attach quadratic (midside node) elements to linear elements.
2. If the shell "drapes" over the solid, make sure it is completely draped. That is, if you can't do it with the ESURF command, don't do it.
3. If the shell is normal to the solid, as in a turbine blade attached to a hub, you will need to make sure that the rotational DOF at the interface
are "tied down" (unless you want to simulate a hinge effect). You can do this in one of two ways:
a) Embed the shell one to two layers deep in the solid. This is the easy way.
OR
b) Use constraint equations (CE command) to relate the shell rotations to the solid translations. This is the theoretically correct way, but constraint equations are difficult to input. You can specify a rigid
region (CERIG command) and then delete the unwanted constraint equations.
4. The PCG solver (PowerSolver) is NOT recommended for a shell+solid model.
5. You can use a solid element with rotational DOF (SOLID72), but the moment transfer is localized at the interface - see Solution 6260 below for details.
3. SOLUTION 6260
Q: Can the rotational DOF of the SOLID72 element be used for moment continuity at a connection to beams or shells?
A: The SOLID72s will not provide full moment continuity equivalent to the stiffness of the beam or shell. For one thing, the stiffness of the beam or shell is concentrated, while the SOLID72 elements at the attachment point may represent only a small part of the section on the SOLID72 side of the connection.
The test problem below illustrates this. A one inch wide model with a modulus similar to aluminium starts with a 1 inch cube of SOLID72 elements. From the centre of this projects a 29-inch long SHELL63 beam. The shells and SOLID72 elements are connected simply by their common rotational DOF. A 10-psi pressure is applied to the shell elements, which produces a moment of about 4500 in-lb at the connection to the SOLID72 elements. This results in approximately a 12.5-degree rotation between the SOLID72 portion of the model and the shells. This actually appears to be a local rotational deformation in the immediately adjacent SOLID72
elements. The SOLID72 elements do not provide full moment continuity. They will prevent a complete hinge, however, and this modelling technique may be adequate in some cases.
/prep7
et,1,72
et,2,63
r,2,1
mp,ex,1,1e7
block,,1,,.5,-.5,.5
block,,1,-.5,0,-.5,.5
wprot,,-90
rect,1,30,-.5,.5 ! area at center of two blocks
nummrg,kp
esize,.25
vmesh,all
type,2
real,2
esha,2
esize,.5
aslv,u
amesh,all
esel,s,enam,,63
nsle
sf,all,pres,10
alls
nsel,s,loc,x
d,all,all
nsel,all
save,model,db
fini
/solu
solve
fini
/post1
set,last
nsel,s,loc,x,1
prdi
nsel,all
fini
/exit,nosa
Posts
No comments:
Post a Comment