Patent Application
20060050987
The present invention relates generally to deformation analysis and, more particularly, to finite element mesh processes used in deformation analysis.
The process of finite element analysis that deals with large deformation usually produces distorted elements at the later stages of the analysis. These distorted elements lead to several problems; inaccurate results, slow convergence and premature analysis termination. Metal-forming processes are the most common applications involved with large deformation analysis; they include forging, extrusion, rolling, deep drawing, and so on. An example of such large deformation analysis is illustrated in
There are two conventional techniques for addressing this problem, the adaptive remeshing and the Arbitrary Lagrangian-Eulerian (ALE) techniques. Both techniques, however, have drawbacks.
Adaptive remeshing is a technique which replaces an over-distorted mesh with a better-conditioned mesh when the error approximation of analysis exceeds the tolerance, or the maximum error value allowed. The newly-created mesh may not necessarily have the same topology as the original mesh, and the number of nodes and elements of the new mesh may differ from the original mesh. Therefore, state variables and history-dependent variables must also be transferred from the original to the new mesh. State variables include nodal displacements and variables of the contact algorithm. History-dependent variables are the stress tensor, strain tensor, plastic strain tensor, etc. The adaptive remeshing technique usually completely remeshes the part at every certain number of steps in the analysis. The disadvantage of this method is its high computational cost, especially during the procedure for determining the error estimator and mapping variables from an old to a new mesh. More importantly, computational costs increase considerably for analysis of complicated geometries.
The Arbitrary Lagrangian-Eulerian (ALE) method is another technique for addressing the problem of large deformation in finite element analysis. This method combines the features of pure Lagrangian analysis and Eulerian analysis—two common types of finite element analysis. In pure Lagrangian analysis, a mesh follows the material deformation during analysis; the mesh is connected to the material throughout the finite element calculation. Since the mesh and the material are connected, severe distortion of the mesh can cause difficulty in the finite element calculation. It is here that adaptive remeshing must be applied to improve the shape quality of the mesh in order to continue the analysis. ALE was developed to reduce the repetition of complete remeshing. Essentially, ALE is a Lagrangian analysis that takes advantage of the advection techniques of Eulerian analysis. In the ALE method, the mesh is neither connected to the material nor fixed to a spatial coordinate system. Rather, it is prescribed in an arbitrary manner. During the analysis, the mesh elements deform according to the Lagrangian method. However, instead of repositioning the nodes at their original position and performing advection, as in the Eulerian method, the nodes are placed at other positions to obtain optimal mesh quality. The mesh nodes have velocity associated with them in order to obtain the updated mesh. Mesh velocity plays an important role in the ALE method as it reduces the analysis error and prevents mesh distortion. Another important characteristic of this method is that it changes the location of the nodes in the existing mesh, instead of creating a completely new mesh, like the adaptive remeshing method, and it maintains the same (or similar) mesh topology throughout the analysis. However, because of its complexity, the computation cost is much more expensive than using pure Lagrangian analysis. There are also other limitations in ALE analysis. In many cases the mesh suffers considerable distortion and the same mesh topology cannot be maintained for the entire analysis. In such cases, complete adaptive remeshing is still required. Another drawback of ALE is that the state-variables remapping step is much more complicated than in the Lagrangian method.
In one general aspect, the present invention is directed to systems and computer-assisted methods for using inverse pre-deformation to generate a deformed (non-uniform) input mesh for deformation analysis. Using this technique, the elements of the deformed input mesh are pre-deformed into shapes that are, for example, approximately inverse to the elements produced by conventional Lagrangian analysis using a uniform input mesh. As a result, the number of inverted and ill-shaped elements generated when using the deformed input mesh can be reduced at the later stage of the analysis when compared to conventional Lagrangian analysis using a uniform input mesh.
According to various embodiments, the method may include the step of performing a partial analysis (referred to as a “pre-analysis”) on the object subject to the deformation analysis to generate a deformed boundary for the object from an undeformed boundary for the object. Next, the method may include the step of generating the deformed input mesh for the object based on the geometric and strain information from the pre-analysis step. Next, the node locations from the deformed mesh are mapped to the undeformed boundary for the object so that a full analysis can be performed on the undeformed boundary of the object using the deformed input mesh.
In various implementations, bubble analysis may be used to generate the deformed input mesh from the information generated in the pre-analysis step. Also, the pre-analysis step may be performed, for example, until the elements experience sever distortion or until a certain percentage (e.g., between 50% and 80%) of a complete analysis is performed. Further, the inverse pre-deformation process can be used for both two and three dimensional problems. For two dimensional problems, inverse bilinear mapping may be used to map the node locations of the deformed mesh to the undeformed boundary of the object. For three dimensional problems, barycentric interpolation may be used for the mapping step.
Since the deformed input mesh may be generated using the deformed boundary of the object from an intermediate stage of the pre-analysis, the shape quality of the resulting mesh (following the complete analysis using the deformed input mesh) tends to improve until the maximum point is reached around the stage at which the boundary is taken. Then, the shape quality may degrade. Therefore, the inverse pre-deformation process may be also be utilized in an iterative manner. That is, for example, the results of the analysis from the first deformed input mesh may be used to generate a second deformed input mesh for further analysis, and so on. Thus, in cases where the geometry of the problem is complicated, performing the inverse pre-deformation technique just once may not provide sufficient results. Subsequent iterations may, therefore, be performed until the desired results are obtained.
Various embodiments of the present invention are described herein by way of example with reference to the following figures, wherein:
a-b illustrate an example of a large deformation analysis using a conventional finite element analysis;
a-c show the finite element analysis results of the original mesh, the first iteration pre-deformed mesh and the third iteration pre-deformed mesh, respectively, for the test problem;
a-d illustrate the elements with radius ratio greater than 50 at step 18 for the original and pre-deformed meshes, respectively, for the test problem;
a-e illustrate an overview of the two-dimensional inverse-predeformation process according to various embodiments of the present invention;
a-c illustrate an example of the bubble mesh process for a two-dimensional problem according to various embodiments of the present invention; and
Various embodiments of the present invention are directed to systems and computer-assisted methods for finite element analysis that employ inverse pre-deformation to generate, in one embodiment, a deformed input mesh for multi-dimensional Lagrangian deformation analysis. The inverse pre-deformation produces a pre-deformed mesh whose element shapes are, for example, approximately inverse from the shapes into which they will be deformed during the analysis. Accordingly, the new deformation analysis, run on the pre-deformed input mesh, can reduce the chance of inverted elements at later stages of the analysis and decrease the possibility of premature analysis termination. The inverse pre-deformation is applicable for both two-dimensional and three-dimensional problems.
The inverse pre-deformation module 16, as described further below, may generate, based on a partial analysis by the finite element analysis module 14 (a “pre-analysis”), a deformed input mesh to be used by the finite element analysis module 14 in a subsequent analysis of the object. The elements of the deformed mesh are, in various embodiments, approximately opposite of those produced by the pre-analysis. As a result, the number of ill-shaped and inverted elements can be reduced at later stages of the analysis. The output data from the computer system 12 may include boundary shape and stress information for the deformed object.
The modules 14 and 16 may be implemented as software code to be executed by a processor of the computer system 12 using any suitable computer instruction type. The software code may be stored as a series of instructions or commands, or as a program, on a computer readable medium. The input data may be stored in a database (not shown) associated with the computer system 12 or may be retrieved from a file. The output data may also be stored in a database and/or in a file. Graphical displays of the output data may also be generated and displayed to a user of the computer system 12.
The primary goal of the pre-analysis is to predict deformation behavior and collect necessary information, e.g., deformed boundary information and equivalent strain, which will be used in the later pre-deformation steps. Thus, according to various embodiments, the pre-analysis step can be carried out until, for example, 50%-80% of a complete analysis is performed, or until severe distortion of the finite elements starts occurring. Furthermore, two mesh data sets may be maintained in this step; the initial undeformed mesh (referred to as “Mesh 1”), and the deformed mesh (referred to as “Mesh 2”). However, to facilitate the node mapping process in a later step, each quadratic tetrahedral element in Mesh 1 and Mesh 2 may be subdivided into eight linear tetrahedral elements, according to various embodiments.
Referring back to
When generating a tetrahedral mesh at step 22, the element sizes should be properly determined. Ideally, smaller elements are desirable around the high-curvature corner regions of the deformed object, where the elements tend to experience more distortion. For this reason, a tetrahedron mesher that can control the element sizes precisely is preferable. Bubble Mesh can achieve this by utilizing the equivalent strain information collected from the pre-analysis step to control the mesh sizes over the whole domain through the grid-based tensor function. In order to do this, a background grid may first be defined over the domain, where the grid size is properly determined for each problem. Mesh sizes are then stored at the grid nodes corresponding to the values of the equivalent strain. Smaller element sizes are specified where the equivalent strain values are higher such as around the high-curvature corners. For the internal point of a grid cell, Bubble Mesh calculates the mesh size by linear interpolation of the values at four grid nodes. Bubble Mesh packs the sphere bubbles closely inside the boundary of the deformed blank using sizes specified in the tensor function to control the size of the bubbles. The mesh nodes are placed at the centers of the bubbles and are then connected by, for example, Delaunay triangulation and tetrahedrization, to generate the tetrahedral mesh.
Referring again back to
Barycentric interpolation is a form of tetrahedral interpolation, and barycentric coordinates are the numbers corresponding to the weights placed at the vertices of a tetrahedron. These numbers can be used to determine the location of the center of mass of the tetrahedron corresponding to the weights put on its vertices. Let Vi (i=1,2,3,4) be the vertices of tetrahedron T. Any point P in three-dimensional space can be expressed as
P=θ1V1+θ2V2+θ3V3+θ4V4, (1)
where θi's are the barycentric coordinates for point P, and
θ1+θ2+θ3+θ4=1. (2)
And point P is inside the tetrahedron if
θi>0 i=1,2,3,4. (3)
In this analysis, point P is a mesh node of Mesh 3, and tetrahedron T is a tetrahedral element of Mesh 2. Thus, Vi and P are known variables in Eqn. (1), and the barycentric coordinates θi's are the numbers to be determined. Since the Eqn. (1) can be decomposed into three sub-equations for x, y, and z coordinates, along with Eqn. (2), there are four equations to be solved for the four barycentric coordinates. Nevertheless, as Mesh 2 is searched for each element that each Mesh 3 node lies inside, the calculated values of barycentric coordinates associated with that node and the element that is found are maintained.
Recall that the initial undeformed mesh (Mesh 1) is deformed into Mesh 2, and both meshes have the same topology. In addition, the element of Mesh 2 that each Mesh 3 node lies inside is also known. Therefore, each of these Mesh 3 nodes can be mapped onto Mesh 1 using Eqn. (1), where θi's and Vi are now the known variables, and P is the location of the node to be determined on the undeformed boundary. By mapping all the Mesh 3 nodes onto Mesh 1, the result is a pre-deformed mesh, such as shown in
Referring again back to
Further, as shown in
The following provides an example of the pre-inverse deformation process for a three-dimensional deformable block. The model consists of a sinusoidal rigid die and a 20 mm by 10 mm by 20 mm deformable blank. The bottom of the blank is constrained in the y-direction, and symmetry boundary conditions are applied at the x=0 and z=10 planes. The die has a sinusoidal shape with amplitude and period of 5 and 10 mm, respectively. The material of the blank is steel and modeled as a von Mises elastic-plastic material with a Young's modulus of 200 GPa, an initial yield stress of 100 MPa, and a constant hardening slope of 300 MPa. The Poisson's ratio is 0.3 and the density is 7800 kg/m3. The die is moved downward vertically at a velocity of 2000 mm/sec and is constrained in all other degrees of freedom.
Three iterations of the inverse pre-deformation were run on this test problem, as shown in
The results from the analyses of the pre-deformed meshes were compared with the results from the analysis of the original mesh.
To compare shape quality of the meshes during analysis of the original mesh and pre-deformed meshes, the radius ratios are computed. The radius ratio ρ is defined as the ratio of the inradius ρin and circumradius ρout of a tetrahedron. The values of ρin and ρout can be calculated as
where a, b and c are the products of the lengths of opposite edges of a tetrahedron. The optimal value of radius ratio is 1 and a high value of radius ratio indicates an ill-shaped tetrahedron. Table 1 below shows the percentage of the total elements that have radius ratio greater than 50 at various analysis steps in the test problem.
According to Table 1, the increasing percentage of original mesh elements implies that the overall shape quality of the original mesh degrades as the analysis continues. The result of the first iteration pre-deformed mesh is obviously improved as fewer number of elements have large radius ratio. In the second and third iterations, the pre-deformed meshes start with more elements having large radius ratio, because many elements are deformed in advance to reduce the severe element distortion expected during analysis. Nevertheless, after only a few analysis steps, the shape quality of the pre-deformed meshes improves rapidly, and the pre-deformed mesh results become better than the original mesh results.
As mentioned above, the pre-deformation technique may also be used for two-dimensional problems. For a two-dimensional problem, inverse bilinear mapping may be used at step 24 to generate a quadrilateral mesh. Also, because the deformation behavior of a three-dimensional problem is usually more complicated than a two-dimensional problem, there are more chances that one iteration of the process might be enough for adequate results.
a-e illustrate an overview of the two-dimensional inverse-predeformation process. The process starts with a uniform mesh, as shown in
After optimal node locations have been located inside the pre-analysis deformed boundary, it is possible to map the new node locations back to the initial boundary (step 24 of
In inverse bilinear mapping, let (x,y) be the coordinate of the source space and (u,v) be the coordinate of the destination space.
x=auv+bu+cv+d, and (7)
y=euv+fu+gv+h, (8)
where a, b, c, d, e, f, g and h are constants. Solving for v in Equation 7, then substituting in Equation 8, the following is obtained:
(au+c)(fu+h−y)−(eu+g)(bu+d−x)=0, or
Au2+Bu+C=0. (9)
Similarly, solving for u in the Equation 8, then substituting in the Equation 7, the following is obtained:
(av+b)(gv+h−y)−(ev+f)(cv+d−x)=0, or
Dv2+Ev+F=0. (10)
Equation 9 gives two solutions and Equation 10 gives another set of two solutions.
However, since all of the master elements are non-concave, and only one unique solution is valid for the range of 0≦u≦1 and 0≦v≦1, a unique solution is obtained.
In summary, it must first be determined in the deformed boundary in which old element ei, each new node ni lays. Next the u and v vectors must be calculated to give the location of this new node ni, inside the old element ei. Then inverse bilinear mapping can be performed to map this new node from the deformed boundary to the undeformed boundary, using the calculated vector u and v, as shown in
The result of the node mapping step is a new pre-deformed mesh inside the initial boundary, as shown in
While several embodiments of the invention have been described, it should be apparent, however, that various modifications, alterations and adaptations to those embodiments may occur to persons skilled in the art with the attainment of some or all of the advantages of the invention. It is therefore intended to cover all such modifications, alterations and adaptations without departing from the scope and spirit of the present invention as defined by the appended claims.
This application claims priority under 35 U.S.C. § 119(e) to U.S. provisional patent application Ser. No. 60/607,916, filed Sep. 8, 2004, entitled “Inverse Pre-Deformation of Finite Element Mesh for Large Deformation Analysis” by Arbtip Dheeravongkit and Kenji Shimada, which is incorporated herein by reference.
| Number | Date | Country | |
|---|---|---|---|
| 60607916 | Sep 2004 | US |
