加载中…
正文 字体大小:

错误node set ErrNodeBCInactiveDof

(2012-06-21 13:45:52)
标签:

杂谈

As I defined a moment load at the free end of a tube, an error occured describing the following message

 ***ERROR: DEGREE OF FREEDOM 6 IS NOT ACTIVE ON NODE 12 INSTANCE OUTERTUBE-1 - 
           THIS LOADING IS NOT VALID
 ***NOTE: DUE TO AN INPUT ERROR THE ANALYSIS PRE-PROCESSOR HAS BEEN UNABLE TO 
          INTERPRET SOME DATA.  SUBSEQUENT ERRORS MAY BE CAUSED BY THIS OMISSION

 ***ERROR: DEGREE OF FREEDOM 6 IS NOT ACTIVE ON NODE 12 INSTANCE OUTERTUBE-1 - 
           THIS LOADING IS NOT VALID

 ***ERROR: 1 nodes have inactive dof on which boundary conditions are 
           specified. The nodes have been identified in node set 
           ErrNodeBCInactiveDof

This was a simplified model. The cross section of the tube lies in the X-Y plane. I added a moment at one node at the free end of the tube with value of CM3. The cross section surface at another end was constrained in Z direction and one node on the surface was constrained in X and Y direction to avoid the rigid body motion. The boundary condtion of X-Y plane rotation on this surface was also added. 
Node 12 in the error message is the node where the moment load added. I am sure that there were no over-constraints. so I am confused with this situation. Is it the problem degree of freedom of element? The linear brick element C3D8 was utilized.

C3D8 doesn't have degree of freedom 6, hence the error. You can only apply a direct load in directions 1 to 3. For a moment load it should be in the direction perpendicular to the axis.

Thanks for your information. I noticed this problem later. But only solid elements C3D... or axissymetric elements CAX... are supported by the postprocessor that I used. In this case, There seems to be two ways that I can follow, one is to develop new element within ABAQUS, and the second one is to modify the postprocessor program, istn't it? However they are both a big job. Are there any easier ways for the simulation?

Axisymmetric elements won't be much use if you're applying a moment at the top unless it's a moment only about the theta direction to cause the edge to curl. 
For solid elements a moment can be applied by applying two forces (a couple) in equal and opposite directions at an equidistance away from the bending axis. As the saying goes: Every couple have their moment.

I am appreciated for your help. The further problem is how to assign a linear distributed moments(in this case, it is transfered to forces) along with the tube. This is another problem in this project that makes me headache.
Using *AMPLITUDE command? But it is described in the manual as following:

Complex time- or frequency-dependent boundary conditions, loads, and predefined fields can be specified by using the AMPLITUDE parameter on the prescribed condition option to refer to an amplitude curve. 

I tried with user subroutine, but the definition of CLOAD is not provided in it.

What else can I do? If *AMPLITUDE is suggested, I wish you can give the tips with a little bit more detail.

If it says that *Amplitude is for applying a time based dependancy then it means that.
If you're applying a variable force along the length of the tube to apply your moment then it's probably easier just to edit the input file manually. Alternatively you could apply a variable pressure along the length equivalent to your forces in a similar way to applying a hydrostatic pressure distribution.   

What corus said is correct and should produce a moment - this method will work perfectly well ***according to the way in which you describe your model**. A pressure normal to the (axial) surface of a tube will produce a moment (m) equivalent to m=PAl, where P is the applied pressure, A is the area over which it is applied and l the perpendicular length between the applied centroid of pressure to the centroid of the support. Also be aware of the fact that applying a pressure in this way will also give you shear, whereas a pure moment will not - is this how you expect your load to be applied? We could do with a drawing of your model to see exactly what's going on. Is it like this:

        P R E S S U R E
     |-------------------|<- fixed translations 
     |-------------------|<- fixed translations


global axes

Y
|
|
|----- Z


pressure applied in -ve Y direction?

If the pressure is applied around the whole circumference then it won't produce a moment. What I was referring to was applying a pressure along a narrow strip down one side of the tube. As drej implies, it's unclear as to what the loading is.

I described the load in the first poster, but I am sorry that it was not clear. Now I quote it in the first poster:
"The cross section of the tube lies in the X-Y plane. I added a moment at one node at the free end of the tube with value of CM3. "

In ABAQUS CAE, CM3 refers to the value of the moment in the third direction, i.e. Z direction. So I meant the load was applied in the term of torsion, and the moment should be in the X-Y plane.

|
.
|------------
             |-->>M(torsion moment in the direction 
|------------            according to right-hand system)


global coordinate system
Y
|
|
|----- Z

In this case, any pressure normal to the outside surface of the tube produces no moment to Z-axis, and this moment is what I expect.

去VIEW里面看,通常node set ErrNodeBCInactiveDof被自动定义成一个集合,这样可以在VISUALIATION中很容易看到.
问题原因有几中,如在某节点的某个自由度被限制的情况下,还施加了边界条件,就会导致这样的情况,检查边界条件,和那些问题节点的自由度情况,特别注意如*EQUATION,*MPC等容易被忽略的命令.

阅读 评论 收藏 转载 喜欢 打印举报
已投稿到:
  • 评论加载中,请稍候...
发评论

       

    验证码: 请点击后输入验证码 收听验证码

    发评论

    以上网友发言只代表其个人观点,不代表新浪网的观点或立场。

      

    新浪BLOG意见反馈留言板 不良信息反馈 电话:4006900000 提示音后按1键(按当地市话标准计费) 欢迎批评指正

    新浪简介 | About Sina | 广告服务 | 联系我们 | 招聘信息 | 网站律师 | SINA English | 会员注册 | 产品答疑

    新浪公司 版权所有