Integration point
Integration point
(OP)
What is an integration point for a finite element ? Please please give me a detail description.
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS Come Join Us!Are you an
Engineering professional? Join Eng-Tips Forums!
*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail. Posting GuidelinesJobs |
|
RE: Integration point
http
RE: Integration point
Since you asked for a detailed description consider that the stiffness of an element is:
K = integral ([b]trans . [c] . [b] dv) (over the volume of the element dv)
The question then becomes "How do I evaluate this volume integration in the most accurate manner". Selection of points to achieve this defines the "integration points".
Ed.R.
RE: Integration point
On a (somewhat) related note, folks often compare elemental strains with averaged nodal strains to determine whether their mesh is adequate. If there is a significant difference, mesh refinement is required.
RE: Integration point
You know, that's something I was thinking about today: software calculates stresses (typically) at the Gauss points of the element....but a variable in that is the displacements (which are calculated at the nodes [not the Gauss points]. So there is sort of a discontinuity there (if I am thinking about it correctly).
I guess it goes back to what you said about meshing properly.
RE: Integration point
RE: Integration point
No discontinuity. Think about a simple link element (pictured below). The finite element solution provides displacements at the nodes (based on a weak form solution to the defining differential equations). Strains are a derivative of the displacements (du/dx), so you take the difference of the nodal values calculate the strains.
If you have some sort of non-uniform loading (say an acceleration load pulling things to the right), the real-life strains are not uniform within the element.
Even if the nodal displacements were exact, which they generally aren't, the linear shape function within the element could not produce anything but a constant strain [u(x)=C1x+C2 ==> du/dx = C1]. The constant strain results will generally be more accurate in the center of the elements (integration points), and least accurate at the nodes in this case.
Of course, you can see how having a lot of elements increases your accuracy, regardless. The idea being if you make the change in strain across the element small (d2u/dx2), the results become more accurate.
2 Undeformed Link Elements
o=====o=====o--->
2 Deformed Link Elements (du/dx used to compute strains)
o=======o=======o--->
Smarter elements (higher order) have shape functions that can better approximate the deformation of the element. If, for example, you had another node in the center of your link elements, you could have a quadratic shape function, which would handle a constant acceleration load (the example given) much more accurately. That additional accuracy comes at a price, though, since higher order elements are more computationally expensive.
So, there are two schools of thought in the finite element world:
1. Use lots of lower order elements in areas with high stress gradients to obtain an accurate solution (h-method), a-la ABAQUS or ANSYS
2. Use fewer, but higher-order (smarter) elements in areas of high stress gradients to obtain an accurate solution (p-method), a-la Pro/Mechanica
The best answer is probably some combination of the two, which is likely where (I think) FE software will go in the future.
RE: Integration point
I'm not sure I am following you here. Are you saying [some] software will use an interpolated displacement [between the nodes] to get a more accurate stress at the gauss points?
RE: Integration point