automatic remeshing with hexahedral elements - Semantic Scholar

AUTOMATIC REMESHING WITH HEXAHEDRAL ELEMENTS: PROBLEMS, SOLUTIONS AND APPLICATIONS Peter Kraft Femutec GmbH, Hamburg, Germany. [email protected]

ABSTRACT The design process of a mesh generation tool for automatic remeshing of hexahedral element meshes is shown as well as its application to the field of simulating metal forming processes. Automatic hexahedral remeshing is very important allowing an economic analyses of processes with large deformation. Although the industry demands robust tools for automatic hexahedral remeshing, previously there were no tools available that have been accepted by the commercial users. An attempt has been made to close that gap. Besides the selection of the most promising meshing technique – the octree-based meshing technique – solutions for other problems that are related to automatic hexahedral remeshing are discussed. Their implementation is presented as well as examples of industrial applications.

Keywords: HexMesh, automatic remeshing, hexahedral elements, octree, metal forming 1. INTRODUCTION The metal forming industry has widely accepted finite element simulation as an efficient tool for designing or analyzing their manufacturing processes [1]. The simulation of 2D processes is already a standard procedure in the development (research) departments of the metal forming industry [2][3]. The available software products have become more robust and comfortable. As a consequence, the graphical user interfaces which display the workpieces, tools and simulations results allow not only scientific experts but more and more design and construction engineers the application of finite element analysis. The field of applications for finite element analysis has entered the design (construction) departments. This is an important development which places several demands on the finite element software. The usage of the software packages needs to be simplified, since construction engineers are in general not FEM experts. And the simulations need to be more economical since money is less easily spent in the design departments than in the scientific departments. This is one reason why the simulation of real 3D processes has not yet taken that step. Even if the analysis technique and the software packages can handle 3D problems nearly as successfully as they can deal

with 2D problems, the cost of simulations for 3D processes is far beyond that for 2D processes. While a 2D analysis can be performed on a standard workstation, the computational power which is required for 3D analysis demands computers with far more memory and more (or faster) processors to perform the simulations in acceptable computation times. In addition the time the user needs for creating and supervising the simulation for a 3D analysis is far higher. Weingarten wrote in [4]: “Furthermore, it is important to remember that, because automatic hexahedral meshers contain so many limitations they are really semi-automatic at best, using hex elements may be more time-consuming than using 10-node tet elements, which take the advantage of the speed of fully automatic meshing.” The industry is not willing to accept these large costs to provide the man power for 3D simulation in that situation. The objective of this paper is to show the design process for a robust automatic mesh generation tool for remeshing hexahedral finite element meshes, its implementation and its performance in the industrial world. Various authors have been undertaking research in this field but most of the research results have not made the jump from the scientific (academic) environment to industrial applications. One reason is the lack of robustness. Another is the larger number of limitations in many cases. The research has been focused

on developing the main meshing strategies, but smaller problems that need to be solved for robust remeshing have often not been discussed. This paper focuses on (which includes the examples shown) the metal forming industry. The simulation of forming processes using a Lagrangian approach requires many remeshing steps, so the demand for an automatic remeshing tool is very high. The proposing of a new meshing strategy or a new application for remeshing is not the purpose of this paper. Instead it means to present – like a guideline – the design of a remeshing tool that works robustly and automatically. The result is proven by the acceptance of the industry.

1.1 Overview Various techniques for generating 3D finite element meshes have been proposed in the last few years. The selection of the most promising method for remeshing hexahedral element meshes is discussed. A short review of the existing techniques with respect to the remeshing is given, before the reasons that lead to choosing the octree technique are presented. The third section is focused on diverse problems that occur with remeshing, which are not basically part of the mesh generation itself. These interesting topics are often not mentioned in the literature since they are not directly related to the meshing algorithms, but they still need to be solved. The fourth section presents the implementation of the remeshing tool based on the design issues mentioned in this paper. It is the program HexMesh which is – for example – integrated in the finite element software package MARC/AutoForge [22]. MARC/AutoForge is widely used within the metal forming industry. The implementation of solutions for the problems that have been shown in the third section are presented here and additional features that allow advantages for the analysis of special manufacturing processes are mentioned. Simple meshing examples end this section. Finally, the application of the meshing tool is demonstrated on some typical problems of the automotive industry. They illustrate the use of the finite element simulation and the mesh generation in practical applications. It should also give the reader an impression of the state-of-the-art of simulation of forging processes in the industry.

1.2 Remeshing The term remeshing is used for a mesh generation process that generates a new finite element mesh out of an existing mesh. Normally a solid model or a surface model is the input for a mesh generation process. The exchange of an exiting finite element mesh with a new one can be caused by several factors. The change of the element class or the change of the mesh density for example. But, most often, remeshing is necessary because the element quality of an existing mesh is no longer sufficient for the analysis. Simulation of a process with large deformation of the finite element mesh causes a loss of mesh quality. If the initial finite element mesh is being deformed during a simulation, the deformation of that mesh

can be so strong that the simulation error which occurs due to the distortion of the elements is no longer acceptable. At this stage a new mesh is created that replaces the old, distorted mesh. The new mesh should have better elements but fill the same volume as the old one. This is what will reffered to as remeshing, the generation of a new finite element mesh that replaces an old mesh. Both meshes should fill the same volume and have the same contact areas to tools or symmetry planes. The analysis data that describe the current state of the object are than transferred onto the new mesh in the following rezoning step. The rezoning is seen as part of the analysis and not of the meshing, so it is not discussed here.

1.3 Non supervised remeshing Typical metal forming simulations need between 20 and 100 remeshing steps during their simulation ([5][6]). The necessity for remeshing depends on the way the simulation proceeds. Since it is not possible to predict the flow of the material we can not predict the time when a finite element mesh needs to be remeshed. The total time of a simulation can extend to several days or even weeks. It is not possible or at least not economical to supervise the simulation and do the remeshing manually whenever it is needed. The remeshing should be made automatically without any user interaction during the simulation. This does not mean that an automatic remesh tool needs to mesh every possible object without setting any parameter a priori. Even if most parameters that are necessary for the meshing (for example, the desired element size) can be calculated automatically we can expect the user to figure out the optimal values of all necessary parameter. But once these parameters are set the whole simulation – including all remesh runs – should run without any user interaction.

1.4 Hexahedral elements The two main classes of elements used in 3D finite element analysis are tetrahedral elements and hexahedral elements. The question of which class of element is to be preferred for an analysis is widely discussed. A comparison of the performance between both elements can be found in [7] and [8]. But, whenever a simulation of elastic-plastic material behavior is made, it is necessary to use at least quadratic tetrahedral elements or linear hexahedral elements. This is due to the “Brezzi-Babuska condition”. The use of quadratic elements, however, does have some disadvantages. The number of degrees of freedom for the simulation is higher and the contact conditions are far more complex. This makes the analysis very expensive [9]. A second point is frequently not mentioned when comparing tetrahedral and hexahedral elements: tetrahedral elements cause critical errors if they get distorted, while hexahedral elements still produce acceptable results, even when they are already distorted. In a certain way tetrahedral elements are a kind of degenerated hexahedral elements. Most test examples used to compare the element classes are quite simple because they need to be compared with theoretical results, so they often do not have any distorted elements. That is one aspect why this very important issue (for the forming industry) is seldom mentioned.

1.5 Other terms In this paragraph the meaning of some terminology used in this paper is explained: •

•

•

•

• • •

Object: Traditionally the object whose manufacture is simulated, the workpiece, has the strongest deformation. It is also most often the object which is to be remeshed. Modern simulation can cope with multiple deformable bodies, which will allow the simulation of composite workpieces. The term object will reference the body which is actually to be remeshed, regardless of whether it is the workpiece, one component of the workpiece or a tool. Also the term tool refers in general to any body that is not being remeshed. Contact body: In general every tool (die) or workpiece is a contact body. In this paper it refers to all objects of the analysis that are in contact with the workpiece, like tools, symmetry planes or even the workpiece itself (self contact). Remesh run: A remesh run is the simple procedure of remeshing the object once. This may includes edge detection, multiple meshing attempts, contact checking, volume control, parameter adaptation and various other things. Initial mesh: This is the start mesh of the analysis. It may have been created manually, extended from a previous 2D meshing stage, created with a normal meshing program or imported somehow to the analysis. Old mesh: The mesh that came from the analysis. It is to be remeshed, the input for the remeshing tool. New mesh: The output of the remeshing tool, the newly created mesh. Tied nodes: A node is tied if some constraints exists that defines its position relative to other nodes (multi point constrains).

2. SELECTING THE APPROPRIATE HEXAHEDRAL MESHING TECHNIQUE

2.1 General important points of the input data The first part of the input data which is given to the remesh tool is the old mesh, i.e. the coordinates of its nodes and the connectivity of its elements. The surface of the workpiece which encloses the old mesh can be generated from it. It is based on discrete three or four node patches (depending on the elements the old mesh contained). So we have neither a global description nor are higher order surface elements (NURBS surfaces, ...) available. One could think of using the same surface patches from the old mesh as surface patches for the new mesh. But this has one disadvantages: the old surface patches may already have been distorted, so the new mesh will still contain elements of a poor shape, i.e. the elements which belong to the distorted surface patches. The second point is the type of workpiece we expect to deal with. Traditionally the start objects are simple geometric volumes, like cylinders or bricks, the final objects are most often components for the automotive industry like hubs,

connecting rods, cog wheels. They all tend to be massive, without very small details or thin walls. The third point I want to mention is the fact that besides the well defined geometry of the initial and the final object, we have to cope with any kind of intermediate shapes. This means that it might be possible to extract surface feature like planes, spherical parts, parallel walls etc. from the well defined shapes. But this part is far more complex for the intermediate objects where edges are slowly smoothed out and the curvature of the surface might change everywhere.

2.2 Choosing the best meshing techniques The most important part of a remesh tool is the meshing technique on which it is based. Various different techniques have been published in the last years. A survey of mesh generation technology was presented by Owen [10] who also maintains a survey of meshing software [11]. A reflection of the grid generation in this century is presented by Thompson in [12]. Sabin has presented some criteria for comparison of automatic mesh generation methods [13]. In 1988 K. Ho-Le presented a classification scheme [14] for mesh generation methods that can still be used. He pointed out that the girdbased approach is the only one that can cope with hexahedral (brick) elements. But more recent developments, like the octree-based or skeleton-based methods have not been investigated by K. Ho-Le. This paper limits the investigation of different meshing techniques to the subset of the existing meshing techniques. Even if some of the methods discussed below can not deal completely with hexahedral meshing they might be combined with other methods. Very important for the choice of the right meshing technique is that it shows a good robustness in the manual meshing. Otherwise the automatic meshing would be even more difficult. Due to the high complexity of analyzing the global shape of the object, all methods that need this global information, like the conformal mapping approach, domain or geometry decomposition approaches do not seem to be robust enough. All methods that predefine certain boundary conditions seem to be too complex for automatic remeshing. This means that a paving/advancing front approach is withdrawn since the creation of a hexahedral mesh that is compatible with a surface mesh is too complex, even if the existence of such a mesh can be guaranteed [15].

2.3 Octree based meshing, the best solution The only viable techniques are the grid-based and the octreebased meshing. The grid-based technique can be seen as a special case of the octree-based technique. Whenever an octree is split to the same level for all octree elements, a grid is constructed. The main advantage of the octree-based meshing technique is that it does not need any complex geometric information about the input surface. No geometric properties need to be detected such as corner points for a conformal mapping or medial axises. A second advantage is that the generation of a new surface mesh is not necessary since the octree-based method always creates its own surface quad mesh. Details about the octree-based meshing can be

found in [18] or [20]. Robert Schneiders has already successfully used octree-based meshing for hexahedral remeshing, so its principle possibility has already been proved. If the grid-based method is used its implementation is straight forward, but the octree-based techniques needs transition elements between octree elements of different size (level), which could cause problems for some analysis programs. Even if Schneiders has proposed the existents of template element sets that allow conformal transitions between different octree levels, this design will not use such templates.

3. ADDITIONAL REQUIREMENTS FOR THE REMESHING Unfortunately the meshing is not the only objective a remesh tool has to fulfill. Some of the important pre and post remeshing steps that need to be carried out are presented here:

3.1 Edge detection Even if the meshing is truly the most demanding part, the resulting mesh will not satisfy the user as long as the edges and corners of the workpiece are not represented correctly in the resulting mesh. We can not assume that the edges of the workpiece are already known by the meshing tool since the input of the mesher consists only of the discrete surface description. A preprocessing step has to determine the edges of the workpiece and forward that information to the mesher. If the initial surface has been created manually and edge information has been added to it or if the initial surface description contains edge information (trimming curves of NURBS surfaces, for example) this data can be passed to the mesher while creating the initial mesh. But, the subsequent remeshing does not have this kind of information. It would be possible to store the initial edge information and pass it to the remesher. That means, however, that we will have edges at the same location on the workpiece during the whole simulation. In real processes, edges are quite often smoothed out or new edges are being created. The manufacturing of a hub out of a cube, as shown in Figure 1, is an example. The initial cube has twelve edges, while the final geometry has the eight vertical edges, which are all in different positions to those of the initial mesh. The edges on the top and bottom of the cube have been smoothed out completely.

3.2 Contact / penetration checking The object that is to be remeshed is often in contact with other objects of the simulation, such as symmetry planes or tools. This means that some of the nodes of the object are lying on (within a certain contact tolerance) the surface of these contact bodies. Since only the nodes of the object determine the contact, the surface patches of the object may penetrate the contact body (if it is locally convex) or there might be a gap between the contact body and the surface patch of the object (if it is locally concave). While the number of elements for the deformable bodies is kept as small as possible, to minimize the simulation time, the complexity of the description of the contact bodies is chosen in a such way that the shape of the body is represented correctly. This means they have either an analytic surface description or a representation of discrete elements with a good accuracy, i.e. much more elements compared to the object. Figure 2 illustrates these. The remesh tool needs to locate new surface nodes it has generated on the surface of the contact body instead of projecting them onto the surface of the old mesh if the latter position would be in contact. The possible places for new nodes 54 or 55 in Figure 2 are not acceptable. Nodes need to be placed onto the positions 50 or 51 instead. The element edge between node 15 and 16 is penetrating the curved surface of the tool, while the element edges between nodes 25, 20 and 29 produce a gap. So, for a surface node it is first necessary to calculate its position on the surface of the old mesh. Then this position needs to be checked for penetration into or contact with the contact bodies, and finally a new position on the surface of the contact body has to be calculated (in the case of contact).

Figure 2. Penetration or loss of contact

Figure 1. Smoothing out existing edges and creation of new edges: a) initial 6 sided cube b) 10 sided result

This is very difficult for two reasons: the projection onto the surfaces and the contact checking are very time consuming operations. Depending on the description of the surfaces higher order equations need to be solved. So, here, numerical methods and heuristic assumptions have to be applied. This can lead to errors in cases where the contact algorithm of the analysis works differently or uses a different contact tolerance. As a consequence the nodes which are in contact, from the remeshing point of view, are not in contact for the analysis (or vise versa).

3.3 Volume difference It is quite obvious that the volume of the object should not change during the remeshing. Since the old mesh and the new mesh do not share the same surface mesh (in the general case) a difference in the volume of the two meshes might occur. This difference appears in two situations. The first situation depends on the penetration (or gap) of the surface patches of the old mesh with contact bodies. Since the nodes of the new mesh are not projected onto the old mesh but onto the contact bodies (as mentioned above) a difference in the volume occurs here. These volume differences are actually created by the analysis. The second situation that causes volume differences are curved surface areas of the object. If a convex surface is remeshed and the nodes of the new mesh lie exactly on the surface of the old mesh a loss of volume will occur because the linear surface patches of the new mesh will lie completely within the old mesh (vice versa for concave surface areas). Figure 3a is demonstrating this. Every new remesh run creates a circular polygon that has a smaller radius than the previous one had, even though all nodes of the new mesh are in contact with the old mesh.

surface patches exist, the smaller is the difference of the volume between the original object and the model. This leads to the fact that the volume of the object depends on the number of its elements. This implies that a change of the element size (or number) during the remeshing has to result in a difference in the volume between the new and the old mesh (that is a contradiction to the first sentence of this subsection). These facts need to be taken into account when the volume is controlled during the remeshing.

3.4 Parameter adaptation The state of the workpiece is changed with every increment of the finite element simulation. So it is changed especially between the remeshing runs. A remeshing tool needs to take that into account and should change its mesh parameters. The size of the generated elements should be adapted to the actual state of the workpiece. Smaller elements are required in areas which are interesting for the simulation. This could be contact areas, areas with manufacturing defects on the real workpieces, areas that have a fast flow of material or strong deformations. While the number of elements can be reduced when areas which move out of interest for the simulation are meshed with larger elements. The change of the geometry of the workpiece may require an adaptation of the element size as well. The developing of a flash, for example, causes a reduction of the element size in the flash area. An example for this is shown in Figure 15 and Figure 16. The adaptation of the element size can be implemented automatically or manually. A mesh density function can be employed to calculate the optimal element size for every remesh run. These functions need to analyze the geometry and the simulation stage (i.e. local stress, contact, deformation, etc. ). A manual adaptation of the parameters can be achieved when the simulation allows different remesh criteria during the analysis. This can be used to allow the user to set the mesh parameters in advanced differently for different stages.

4. HEXMESH, AN IMPLEMENTATION

Figure 3. Volume control a) 2D example for volume loss due to remeshing b) linear representation of a sphere c) remesh of the linear sphere d) remesh of a cubic representation of the sphere in b) It has been shown that subsequent remeshing can cause a loss of volume of more than 10% in realistic simulations [16]. This is not acceptable for industrial applications. A further problem is the difference of the volume between the original object and the finite element mesh which is caused by the representation of the real object with discrete linear finite elements. The size of the volume difference depends on the quality of the surface representation which is depends on the size (i.e. number) of the surface patches and the curvature of the object. This means as more (smaller)

Forced by the needs of the forging industry FEMUTEC [17] has started the development of a hexahedral remeshing tool at the end of 1995. The objective was to create a robust, fully automatic meshing tool that proves its good performance in the industrial sector. The various points mentioned in the two sections above have driven most design decisions of development, called HexMesh. It was first published at the end of 1996 and integrated in the finite element software MARC/AutoForge [22].

4.1 Meshing technique The meshing technique implemented in the first releases was a grid-based meshing similar to the one which was published by Robert Schneiders in 1994 [18]. The grid-based method does have the advantage that it only needs local geometric information of the object during the grid building and projection step. It is also quite simple to implement and allows a short development cycle. Even though the remeshing is robust and the program has been accepted by the industry,

the underlying meshing technique has been changed to overcome the disadvantages of the grid-based meshing. The primary disadvantage is the high number of elements that are created. Aspects of different meshing strategies (see [19]) have been implemented and the main technique moved to octree-based meshing. The same decision has been taken by other research groups that work on related topics [20]. A conformal mapping technique is employed to scale elements in certain intervals of the coordinate system. This allows the meshing of small regions (flashes, for example) with elements that have a different aspect ratio. An example is shown in Figure 16, where the flash region of the connecting rod is meshed with smaller elements. The octree technique has been modified such that the difference in the size of neighboring octree elements can be, at maximum, one level. All octree elements are directly converted into finite elements. The transitions between elements of different levels are realized with tied nodes. Since these tied nodes cause problems on the surface of the object a special transition layer is implemented to allow conformal transitions without tied nodes on the surface (Figure 10 shows an example). The projection algorithm is allowed to create degenerated hexahedral elements, five sided wedge elements, to represent the edges of the object better. This can be suppressed if a pure hexahedral mesh is needed, but is has been shown that the analysis performs better with having a few wedge elements than a pure hexahedral mesh, which has in general a greater number of distorted elements (see next paragraph).

4.2 Additional features Some additional advanced features have been implemented to allow more flexibility during the remeshing or to solve the problems mentioned in the previous sections. The following list describes some of the additional features: Relax: instead of the creation of a new hexahedral mesh, the topology of the old mesh is not changed. Smoothing and relaxing operations reposition the nodes of the old mesh to achieve a better mesh quality. This feature is useful in case the number of elements should not be changed (especially not enlarged). Template mesh: the new mesh can be read from a template mesh. The connectivity of the template mesh is used to mesh the object. The template can describe either the whole mesh or just the kernel (the interior elements created by the grid or octree) of the object. This feature can be used if the shape of the mesh can easily be calculated or if the space of the object is known. Higher order surface representation: the linear surface patches of the old mesh are converted into higher order surface elements (Coons patches [21]). This mechanism reduces the volume loss, as mentioned in 3.3, to a minimum. Figure 3 shows an example: the resulting mesh of the sphere in Figure 3b is shown for the linear surface representation in Figure 3c and for the higher order surface representation in Figure 3d. Details can be found in [16].

Edge detection: HexMesh has three different mechanisms that perform the edge detection. Next to the standard detection of edges due to geometric features, the boundary of a contact area can be defined as an edge. This is especially helpful at symmetry planes, since nodes that are in contact with a symmetry plane are never allowed to be detached from it. So the border of the contact area of a symmetry plane needs to be seen as an edge. HexMesh also has the possibility to store edge information so that a new detection can keep all edges that have previously been detected. Edge representation: HexMesh supports four different methods for representing detected edges of the old mesh on the new mesh. Every edge is mapped onto a connected chain of surface patch edges of the new mesh. If two neighboring edges of a single patch are members of that chain, they are replaced by its diagonal. Otherwise, that patch may have a very large angle (~180 degree) between those edges. This can lead to small gaps on the surface if the particular patch is curved (i.e. the diagonal does not lay on the patch parameterization). Since that gap is just an optical problem and the analysis may still perform well, HexMesh can leave the gap as it is, as the first method. Secondly, the element of the patch can be split into two wedge elements. This solution looks good, performs well, but does not produce a pure hexahedral mesh. A third method introduces a split algorithm that removes the wedge elements. The resulting mesh is pure hexahedral, but some more distorted elements are inserted (Figure 7). Finally, an additional chain of elements can be inserted along convex edges to enhance their representation (Figure 6). Orientation control: to achieve a higher independence of the meshing from the orientation of the object in the coordinate space, a rotation of the axis system can be employed to find the optimal position of the object in the coordinate space. Volume control: the volume of the new mesh can be adapted to the volume of the old mesh. A loss or gain of volume is balanced with the higher order representation (as mentioned above) and with local changes of the surface of the element.

4.3 Hexahedral meshing examples The examples shown in this paragraph do not result from commercial simulation of metal forming. They are simple benchmarks which illustrate the overall capabilities of the presented meshing tool. The surface description which is used as input for the remesh tool does not necessarily need to be a volume mesh (as it is for the remeshing), it could also be the 2D surface of an object. So HexMesh can, of course, be used to create initial meshes.

The next example, Figure 5, shows some different techniques of enhancing edges. The first mesh (Figure 5a, left) is the standard mesh that uses wedge elements to allow a good edge representation, Figure 5b shows the detail of that mesh. A second technique to enhance edges can be seen in Figure 7. An additional layer of elements has been put along sharp edges. Figure 6 shows the pure hexahedral mesh. The consequence is more, smaller and more distorted elements.

Figure 4. Cut through the mesh of a bone with an artificial cavity Figure 4 shows a sectional view of an upper leg bone (femur). The mesh generation of such examples is very easy for any mesher since no sharp edges occur. Only the element size of the elements have to be small enough to fit into the small wall around the cavity (here, artificial). The mesh uses two different element sizes on the surface and two additional element sizes of larger elements in the interior. Figure 6. Enhanced edge representation

Figure 7. Pure hexahedral mesh Figure 5. A simple example: a) standard mesh b) detail view

Figure 10. A small detail meshed with smaller elements Figure 8. A grid-based mesh Figure 8 is the mesh of a benchmark found on the internet. It is meshed using the grid-based strategy, i.e. all elements have the same level (size). Even if the mesh looks very good it would be very expensive to perform nonlinear analysis of this example (approx. 60.000 elements). The use of different element levels can result in a reduction of the number of elements.

5. APPLICATIONS Since the first commercial version has been shipped in 1997 several major metal forming companies have used HexMesh (in combination with MARC/Autoforge [22]). The application of HexMesh to real industrial problems, as shown in this section should demonstrate that it is well accepted by the industry. Since most of the simulations FEMUTEC are involved in are confidential, we are glad that we have been allowed to show the following three examples of real life industrial simulations.

5.1 Hub

Figure 9. A mesh with a small detail The application of different element size is shown in Figure 9. Here a small detail, a dent, is meshed with smaller elements. Figure 10 shows that section in detail. While the element mesh has a conformal surface mesh the interior mesh contains tied nodes.

The simulation of the hub shown in this paragraph is the multi stage (two stages) manufacturing of a six-cornered hub. A detailed description of a similar simulation is published in [23]. To illustrate the material deformation, images of four different increments of the simulation are shown. Figure 11 shows the initial mesh at the beginning of the first stage. The initial mesh is a simple cylinder. While taking advantage of the symmetry the simulation was limited to a 90 degree part. Since the hub is six-cornered, a 60 degree part would have been sufficient but the interest of the simulation was the force between the workpiece and the tools. The 90 degree part covered one corner and one side completely which made the simulation more reliable for the customer. The first stage of the process produces an intermediate object. This intermediate object has a better shape for the manufacturing of the final part. One of the main applications of the finite element simulation for the metal forming industry is design of the intermediate stages of multi stage processes. An optimal shape of the intermediate object can reduce the necessary temperature and force. Figure 12 shows the end of the first stage. The simulation of the first stage is very simple. The deformation of the finite element meshes is not very large and no sharp edges or corners are created.

Figure 11. Hub – initial stage The workpiece is quarter of a cylinder, the tools are represented as contact surfaces.

Figure 13. Hub – middle of 2nd stage

Now the tools are exchanged and the second stage of the forming process starts. The shape of the second set of tools can be seen in Figure 13. It shows the simulation in the middle of the 2nd stage. Here, the flow of the material is far larger than in the first stage. A large amount of material moves from the center (the rotation or symmetry axis) outwards to form the ring part, while in the lower part the material gets into contact with the tools and the six-cornered ring is formed.

Figure 14. Hub – end of 2nd stage

5.2 Connecting rod

Figure 12. Hub – end of 1st stage The final part is shown in Figure 14. The forging process has been finished.

The manufacturing of a connecting rod is shown in this example. Figure 15 shows the geometry of the final part. The simulation of this object took an overall time of approximately two days. It was performed on a single processor (R1000, 195 MHz) SGI workstation using 0.5 Giga byte memory. During the simulation more than 50 remesh runs were necessary to keep the mesh quality acceptable. The main goal of the simulation was to control the temperature of the workpiece and to measure the time it needed to cool down. Apart from the temperature behavior, the flow of the material was also of interest. The developing flash area had to slow down the outward flow of the material to allow the filling of the whole die.

reduce the simulation time advantage was taken of the symmetry and one tooth was simulated.

Figure 15 Connecting rod – final increment Figure 16 shows the flash region in detail. To allow a sufficient quality of the simulation of the flash the elements in the flash region needed to be thin enough that at least four elements fit over the thickness of the flash. Two methods have been applied to fulfill that condition and to keep the overall number of elements within a tractable range. First the aspect ratio of all elements had been set so that the elements were smaller in the direction of the thickness of the flash and second the area of the flash was scaled up before the remeshing and scaled back after the remeshing.

Figure 16 Connecting rod – detailed view of the flash region

5.3 Toothed wheel This example shows the simulation of the manufacturing of a toothed wheel. The simulation was made for the company Sieber Trade [24]. Figure 17 shows the solid model of the whole wheel. It consists of 61 equally formed teeth. To

Figure 17. Toothed wheel – solid model An image of the final tooth is shown in Figure 18. The aim of this simulation was not to optimize the manufacturing process but to calculate the pressure that is applied to the tools at the end of the process. The area of interest here was the head of the tooth (addendum circle). To achieve a high accuracy the contact area was meshed with far smaller elements than the remaining part of the body.

Figure 18. Toothed wheel – simulated tooth Actually, three different element sizes have been applied. The finer were introduced around the area where the development of the tooth started, as the material deformation is high in that area. Since the remaining part of the body is of less interest for the simulation, the larger elements have been used there.

6. CONCLUSIONS The major focus of scientific research in the field of hexahedral meshing is the design of main meshing strategies. However other problems that need to be solved to allow robust automatic remeshing with hexahedral elements have not been given much attention so far. This paper has presented a guideline for the design process of robust remeshing tool, closing the gap between scientific research and industrial application. Many problems that occur and possible solutions for them have been shown, so a robust hexahedral remeshing tool could be developed. The performance of that tool – called HexMesh – has been shown in commercial simulations. A wider range of applications for the finite element analysis is now open for the industry.

REFERENCES [1]

A. Erman Tekkaya, “Stand und Entwicklungstendenzen der Umformsimulation”, Umformtechnik, pp. 44-48, (1998) [2] Hendrik Schafstall, Michael Winter and Peter Kraft, Wirtschaftliche Auslegung von Schmiedeprozessen mit MARC/AutoForge, Benutzertreffen Deutschland, MARC Software Deutschland GmbH (1997) [3] A. E. Tekkaya, “Current State and future Developments in the Simulation of Forming Processes”, 30th Plenary Meeting of the International Cold Forging Group ICFG, Den Bosch, (1997) [4] Victor I. Weingarten, “The controversy over Hex or Tet meshing”, Machine Design, April, pp. 74-78 (1994) [5] Haluk Menderes, “Simulation als wesentliches Element in CAD/CAM Systemen- Neue Trends in CAE””, Tagungsband XXIV. FEM-Kongreß, Baden-Baden, Germany, pp. 33-74 (1998) [6] Michael Winter, “Einsatz der Prozeßsimulation zur Verkürzung der Entwicklungszeit am Beispiel der Warmumformung”, Tagungsband XXIV. FEMKongreß, Baden-Baden, Germany, pp269-284 (1997) [7] Steven E. Benzley, Ernest Perry, Karl Merkley and Brett Clark, “Comparison of all Hexagonal and all tetrahedral finite element meshes for elastic and elasticplastic analysis”, Proceedings of the 4th International Meshing Roundtable, Albuquerque, pp. 179-191 (1995) [8] A. O. Cifuentes and A. Kalbag, “A performance study of tetrahedral and hexahedral elements in 3-D finite element structural analysis”, Finite Elements in Analysis and Design”, Vol. 12, pp. 313-318 (1992) [9] A. E. Tekkaya, “State-of-the-Art of Simulation of Sheet Metal Forming”, 6th SheMet Conference, University of Twente/The Netherlands, pp. 53-66 (1998) [10] Steven J. Owen, “A Survey of Unstructured Mesh Generation Technology”, Proceedings of the 7th International Meshing Roundtable, Sandia National Lab, pp. 239-267 (1998)

[11] Steven J. Owen, “Meshing Software Survey, URL: http://www.andrew.cmu.edu/user/sowen/softsurv.html (1998) [12] Joe F. Thompson, “ A Reflection on Grid Generation in the 90s: Trends, Needs, and Influences”, 5th International Conference on Numerical Grid Generation in Computational Field Simulations, Mississippi State University, pp. 1029-1110, April (1996) [13] M. Sabin, “Criteria For Comparison of Automatic Mesh Generation Methods”, Advances in Engineering Software, Vol. 13, #5/6, pp. 220-225 (1991) [14] K. Ho-Le, “Finite element mesh generation methods: a review and classification”, computer-aided design, Vol. 20(1), pp. 27-38 (1988) [15] Scott A. Mitchell, “A Characterization of the Quadrilateral Meshes of a Surface Which Admit a Compatible Hexahedral Mesh of the Enclosed Volume”, 13th Annual Symposium on Theoretical Aspects of Computer Science (STACS `96), pp. 465476 (1996) [16] Peter Kraft and Paul Pfeufer, “Jüngste Entwicklungen im Bereich Hexaeder-Vernetzung für den vollautomatischen Einsatz in der Simulationspraxis", XXIV. FEM-Kongreß, Baden-Baden (1997) [17] Femutec GmbH, Tempowerkring 9, Hamburg, Germany. Email: [email protected] [18] Robert Schneiders, “Automatic Generation of Hexahedral Finite Element Meshes”, Proceedings, 4th International Meshing Roundtable, pp. 103-114 (1995) [19] Peter Kraft, “Möglichkeiten der adaptiven Hexaedervernetzung komplexer Gebiete”, XXV. FEMKongreß, Baden Baden, pp. 419-430 (1998) [20] Weiler, et. al., “Automatic Geometry-Adaptive Generation of Quadrilateral and Hexahedral Element Meshes for FEM”, 5th International Conference on Numerical Grid Generation in Computational Field Simulations, Mississippi State University, pp. 689-697, April 1996 [21] David F. Rogers and J. Alan Adams, “Mathematical elements for computer graphics”, Mc Graw Hill (1990) [22] MARC Analysis Research Corporation, 260 Sheridan Avenue #309, Palo Alto, CA 94304, Tel.: +1/650/329 6800 [23] Peter Kraft, Hendrik Schafstall and Michael Winter, “Einsatz der Prozeßsimulation zur Auslegung dreidimensionaler Massivumformvorgänge am Beispiel der Herstellung einer Kugelnabe”, Benutzertreffen Deutschland, MARC Software Deutschland GmbH, (1996) [24] Karl Sieber GmbH & Co. KG, Fabrik für Umformwerkzeuge, Tiedenkamp 1, D 24558 HenstedtUlzburg, Germany