ansys中求解时出现这个错误：negative radius on element 1，这是什么错误？

ljttlf

ansys中求解时出现这个错误：negative radius on element 1，这是什么错误？怎么改正阿？

wangsnike

我的也是，请高手指教。negative radius 负半径指的是什么？请问是否与网格划分有关，还是与element位置有关。。。

hitvip

srosset (Electrical) 12 Apr 05 3:21  
Hello,
I am doing coupled field electrostatics/structural analysis.
It means that I calculate an electrostatic force, then the displacement of the structure due to this force. After that I do a mesh morphing to calculate the new electrical field and electrostatic force, and so on until convergence occurs. I am doing this on a circular plate, so I used axisymmetrical modeling. I have large deflection, but for relatively small strain.
My problem arises with high tensions (i.e. large displacement) after some iterations, I can do the mesh morphing, but I can';t solve the electrostatic problem anymore and I get this error message : "Negative Radius on Element XXX" (XXX being the number of an element situated on the axis of revolution of my rectangle (the rectangle, by rotation around the Y axis, creates a circular plate))
What I don';t understand is that the element is not highly deformed and looks fine. I';ve tried to look in the help files for this error message, but the only reference I can find about "Negative Radius" is in the time bisection paragraph of the automatic time stepping chapter :
5 An illegal element distortion is detected (e.g., negative radius in an axisymmetric analysis)
But I don';t see what is wrong with my element. It has move a lot from its original point (it';s at the center of the plate), but is not distorted. I tried to unmesh the area and remesh it, but if I control the new mesh, I do have the same error coming.
Does anyone know what is causing this problem and how I could solve it?
Thanks in advance for your replies.


Eng-Tips Forums is Member Supported. Click Here to donate.
Drej (Mechanical) 12 Apr 05 4:36  
Weird.
Is your model constrained correctly? I';m thinking rigid body motion and that possibly one (or more) of your elements is/are displacing outside the "allowed zone" in axisymmetric XY space? Make sure your triad is plotted at the origin (/triad,orig) then change displacement scaling to 1:1 (/dscal,1,1) and then pldisp. Have you tried running with/without NLGEOM as well?
Cheers,
-- drej --

srosset (Electrical) 12 Apr 05 11:39  
There is one thing I might have done wrong : I haven';t set a SYMM boundary condition on the Y=0 line, for I thought it was implicit, due to the fact I defined the element with the axisymmetrical keyopt. I';ve tried with and without it with small actuation voltage and as I didn';t notice any differencs, I removed it. It is not clearly stated in the helpfiles if this condition is needed, optional or useless for axisymmetrical geometries.
If I take a close look to the border element near Y=0, I can indeed see that they have a slight negative move on the x axis, which is indeed illegal, but what can I do against it?
Thanks for your help.

user76 (Mechanical) 1 Jun 05 12:54  
I just had this same error message while running an axisymmetric structural analysis (linear, small-deformations).  Turns out I had to put all my elements/nodes and lower items in the +x-axis.  Apparently when my elements were in the -x-axis, Ansys didn';t like it and gave this error for every element in my model.

srosset (Electrical) 1 Jun 05 13:11  
What you describe is different from my problem, but is normal. I would suggest you read the help file for a more complete explanation, but in short, in an axisymmetric analysis, the Y axis (x=0) is defined as the axis of rotation of the model. It is therefore impossible to have any node with a negative x component. But you cannot place your model wherever you want on the x axis : for exeample if you draw a rectangle with corners at (0,0) and (10,1), it would represent a circular membrane of radius 10 and thickness 1. If you shift your keypoints of 10 along the x axis to (10,0) and (20,1) your model now represent a circular membrane of radius 20 and thickness 1 with a hole in its center of radius 10.
This shows that x component of the keypoints cannot be chosen randomly.
Hope this helps.

zg0609

用ANSYS分析轴对称问题时,单元X方向的坐标值必须是大于零的值.将模型重新调整一下就可以了.

caat

谢谢  今天遇到这个问题 谢谢