Using modified quadratic tris and tets in contact problems 1

[nmk321]

I am modeling contact with irregular geometry and therefore deem it necessary to use modified triangle elements for my 2D axisymmetric analysis, and modified tetrahedrals for my 3D analysis, as per the ABAQUS user manual recommendation. However, I understand that stresses are inaccurately predicted at the surface with these elements:

Excerpts from section 22.1.1 of the Abaqus Analysis User's Manual (v6.7):

"In areas of high stress gradients, stresses extrapolated from the integration points to the nodes are not as accurate for the modified elements as for similar second-order triangles and tetrahedra in Abaqus/Standard. In cases where more accurate surface stresses are needed, the surface can be coated with membrane elements that have a significantly lower stiffness than the underlying material. The stresses in these membrane elements will then reflect more accurately the surface stress and can be used for output purposes."

[...]

"Surface stresses can be output in contact analyses by requesting element output (either extrapolated to the nodes or extrapolated to the nodes and averaged) to the results or data file, by querying the surface nodes in the Visualization module of Abaqus/CAE, or by requesting element output (extrapolated to the nodes) to the output database. These stresses are extrapolated from the integration points. In the case of modified triangles or tetrahedra, they can be inaccurate in areas of high stress gradients. In cases where more accurate surface stresses are needed, the surface can be coated with very thin membrane elements that have stiffness comparable to the underlying material. The stresses on these membrane elements will then reflect the surface stress more accurately."

(emphasis mine)

So if I add membrane elements, shall I make their stiffness similar to or much less than the stiffness of the triangle or tetrahedral elements? I'd appreciate any guidance in this matter from those who have dealt with using membrane elements on modified quadratic tris or tets.

Thank you,
Nathan

 

[johnhors]

Nathan,

In your first excerpt:-

"membrane elements that have a significantly lower stiffness than the underlying material"

in your second excerpt:-

"very thin membrane elements that have stiffness comparable to the underlying material"

The fact that the second excerpt adds "very thin" and then probably assumes you use the same Young's modulus means you will still have elements with a much lower stiffness than the underlying material. Perhaps stiffness in the second excerpt should have read modulus instead.


Before doing this procedure, you should be aware that membrane elements have incompatible displacement and shape functions with solid elements, or in other words its a bad idea to mix different element types in this fashion, as it breaks one of the golden rules FEA, that is FEA theory is based on the "continuum" being represented by discrete points. Incompatible elements introduce dis-continuities.

Or look at it another way, stress is derived from strain which itself is derived from the displacements. Thus if the stress results aren't good, how can you expect the displacements to be good? After all this method is basically imposing a displacement field (from the dodgy solid elements) on the shell elements from which it calculates stresses.

I think the bottom line is, "how can a coating of membrane elements magically improve poor results from a solid model" ? If this is true then shouldn't all solid models be smeared with a coating of thin membrane elements?

 

[nmk321]

Thank you for your thoughts, johnhors. Your reply has spurred my interest in the subject of mixing different element types. As I am relatively new to finite element modeling, I've been doing some reading (in these forums, textbooks, journal papers) regarding the matter, and I can't quite seem to find a solid argument against mixing different element types. Aside from your comments, the best I could find is in a journal article: "there are concerns with the validity of combining shell and solid elements" (paraphrased). I gather that elements having different DOFs can be combined as long as their nodes are tied together properly using multi-point constraints. Yet, I do not have any indiction from my readings on how combining different element types deteriorates the accuracy of a solution. Does anyone know of good resources that explain the basis of how combining different element types affects the accuracy of the results?

Thank you,
Nathan

 

[johnhors]

Nathan,

Consider a simple linear eight node brick element with all six sides square and all edges of length one. To apply a unit pressure to any one side, the pressure has to be equated into equivalent nodal forces, which are as you might think are simply 0.25 at each of the four corners. Now consider a parabolic twenty node brick element instead which has midside nodes placed along each edge. Each side or face of the brick element now has eight nodes (four at the corners and four at the centre of each edge). In this case a unit pressure on the face does not equate to 0.125 at each node, but the equivalent set of nodal forces for a uniform pressure is now one third at each mid side node in the direction of the applied pressure and minus one twelfth at each corner node ( 4 * 1/3 – 4 * 1/12 = 1 ) . Without going deep into FEA theory of displacement functions you just have to accept that’s the way the mathematics works out. Now for a smooth flow of stress (pressure) from one element to the next in a model the nodal forces have to be like for like. Most solvers will happily let you mix element types and formulations, however where the differing elements are connected together it is impossible to maintain a smooth flow of stress between them. In a stress contour plot this can manifest itself in the form of false peaks and troughs.

Going back to your original enquiry about coating contact surfaces with membrane elements, there is one very important aspect that has been overlooked here. Where bodies contact this induces compressive stresses in the solids normal to their surfaces. This compressive stress is the dominant stress component. The membrane elements will completely ignore this compressive stress and only report back in plane surface stresses. Thus to claim that membrane elements provide “more accurate surface stresses” is nonsense.

John

http://www.roshaz.com

 

[PachoIngetec]

Nathan and John,

I am not an expert in FEA modeling, but I have been dealing with contact modeling the last year. Instead of using a membrane element like you were discussing, but about using solid elements, very slender element with a lower stiffness to represent the contact between the two surfaces.

But do you think of that? Is it a good idea?

 

[johnhors]

If your slender element has the same Young's modulus as the rest of the solid then I can't see the point in doing that. Slender solid elements will introduce elements with poor aspect ratios, that is not going to help mattters. Abaqus has plenty of controls for hard, soft, exponential stiffness contact controls and so on to play around with, so you should keep elements as well shaped as possible.