Double-sided incremental forming (DSIF) is a subcategory of general incremental sheet forming (ISF), and uses tools above and below a sheet of metal to squeeze and bend the material into freeform geometries. Due to the relatively slow nature of the DSIF process and the necessity to capture through-thickness mechanics, typical finite element simulations require weeks or even months to finish. In this study, an explicit finite element simulation framework was developed in LS-DYNA using fully integrated shell elements in an effort to lower the typical simulation time while still capturing the mechanics of DSIF. The tool speed, mesh size, element type, and amount of mass scaling were each varied in order to achieve a fast simulation with minimal sacrifice regarding accuracy. Using 8 CPUs, the finalized DSIF model simulated a funnel toolpath in just one day. Experimental strains, forces, and overall geometry were used to verify the simulation. While the simulation forces tended to be high, the trends were still well captured by the simulation model. The thickness and in-plane strains were found to be in good agreement with the experiments.
ISF is an evolving manufacturing process that utilizes generic tooling to manipulate sheet metal in an effort to produce freeform parts without the need of a die. Predefined toolpaths are used to move numerically controlled tools in such a way that a final part is manufactured due to the accumulation of many localized deformations. Because of the reduction in overhead time as well as related labor and material costs, ISF is generally recognized as a flexible and energy-efficient manufacturing process particularly well suited for highly customized, low-batch production . Additionally, it has been shown that parts formed via ISF experience a significant increase in formability when compared to conventional stamping [2,3]. Referring to Fig. 1, various methods of ISF have been developed, namely, single point incremental forming (SPIF), two-point incremental forming (TPIF), and DSIF.
SPIF utilizes one forming tool to deform a peripherally clamped sheet of metal into the desired shape. However, SPIF tends to suffer due to global deformation effects, such as sheet bending outside the forming region, and often requires the use of a geometry-dependent backplate to improve the resultant geometric accuracy. There have been various attempts [4–6] to compensate for the often observed inaccuracy regarding the part geometry; however, they tend to require prior calibration procedures and trial runs before the production of a successful part. TPIF was developed at approximately the same time as SPIF  and demonstrates higher process control at the expense of requiring additional tooling. An excellent example of the success of TPIF is given by the AMINO Corporation, which developed their first prototype machine in 1996 . However, there was an apparent need to increase the geometric accuracy relative to SPIF, while simultaneously retaining the tooling flexibility. This notion led to the implementation of DSIF [9,10], which takes advantage of a secondary tool to provide local support rather than a partial die. Additionally, the through-the-thickness pressure imposed by the opposing tools has been shown to further increase formability in the sheet relative to SPIF [11,12]. However, the loss of tool contact and complexity in toolpath design can make DSIF a difficult process to implement in practice. One general framework to better understand the DSIF process is to develop and analyze simulation models by means of finite element analysis (FEA). These computational tools are pivotal toward better understanding the underlying mechanics of DSIF, which can then provide the necessary insight toward creating new and effective toolpath strategies.
Formability and Mechanics.
Before delving deeper into the existing simulation studies, it is insightful to have a better understanding on the observed mechanics of ISF through an experimental perspective with analytical justification. The definition of formability in ISF is not distinct, but is often characterized by the failure strains of a formed cone, or funnel part, and then also noting the maximum wall angle that was achieved before fracture occurred.
Jeswiet et al.  formed cones for various materials and thicknesses, and found that a maximum wall angle, or draw angle, is usually in the range of 60 deg and 70 deg for many steels and aluminums. Some researchers, such as Jackson and Allwood  and Lu et al. , have attempted to quantify the mechanics of ISF using predominantly experimental techniques. For SPIF, there is evidence that through-the-thickness shear, as well as stretching and shear in the plane of the toolpath, are prominent deformation mechanisms. Furthermore, the in-plane strains near the fracture zone of a part are found to be considerably larger than what is predicted as unstable by necking via a forming limit curve (FLC).
Emmens and van den Boogard  performed an extensive study on the proposed failure mechanisms in SPIF and remarked that a conventional FLC is only valid if (1) the strain path is straight within the principal strain space, (2) the deformation is dominantly caused by membrane forces, (3) through-the-thickness shear is negligible, and (4) plane strain exists. While these conditions are often reasonably met in traditional stamping processes, all four of these conditions are violated in ISF suggesting that FLC predictions may not be appropriate for ISF. Silva et al. [16–18] developed a membrane analysis for SPIF which incorporated ductile damage mechanics to estimate the state of stress under different forming conditions and to predict fracture. In recent work, Martins et al.  furthered this damage mechanics framework to create an analytical fracture locus in strain space for anisotropic materials under plane stress conditions. While there is still some debate, there is strong evidence that the formability of a part is limited by the fracture FLC rather than the FLC, and that localized necking does not occur prior to fracture.
A substantial amount of research has been pursued related to the effects in mainly SPIF from varying the tool diameter, incremental depth, sheet thickness, forming speed, and part curvature [20–29]. In short, the general trends suggest that a decrease in tool diameter or an increase in sheet thickness will lead to an increase in the maximum achievable forming angle of a part. Additionally, if the incremental depth, ΔZ, is reasonably small (i.e., ∼1 mm or less), the achievable forming angle is not significantly altered. Typically, the most sensitive factors toward influencing the formability, geometric accuracy, and surface finish are the tool diameter, incremental depth, material type, and thickness.
In addition to the various setups seen in ISF, there have also been a considerable number of toolpath techniques to overcome many of the initial challenges seen in ISF, specifically geometric accuracy and maximum achievable wall angle. Changing the toolpath, or forming strategy, can significantly affect the success of a formed part, which implies that there is a strong relationship between a given toolpath and the resultant mechanics of the process. Accumulated-DSIF (ADSIF) will be discussed to highlight some of the effects of varying the forming strategy.
A recent toolpath strategy termed ADSIF, or ADSIF, is worth noting due to the relatively equal distribution of material thickness and natural prevention of loss of tool contact with the sheet . In ADSIF, the two forming tools are maintained within a plane that is initially equal to that of the peripherally clamped sheet metal. Starting from the innermost profile of the desired part, the tools traverse radially outward. In essence, ADSIF is an in-to-out toolpath technique whereas conventional DSIF is out-to-in. One key advantage of this technique is that the material being locally deformed is virgin material and thus, the sheet thickness entering the tools remains approximately constant. As noted by Ren et al. , the nature of the process mechanics and required force related to bending and compressing the virgin material between the tools combined with machine compliance makes it difficult to achieve wall angles much higher than 50o. Additionally, controlling the geometric accuracy of the process can be difficult, though this can be minimized by means of exploring and modeling the parameter space as shown by Ndip-Agbor et al. . Alternatively, Zhang et al.  demonstrated that Mixed DSIF can be used in an effort to combine the benefits of both ADSIF and DSIF. Inspired by the mechanics observed in multipass strategies, Mixed DSIF first forms the desired part via ADSIF, and then reforms the part using a conventional DSIF toolpath to improve the geometric accuracy.
Simulation Studies of ISF.
Finite element methods have been extensively utilized in order to better understand the fundamental mechanics that differentiate the various ISF setups and toolpath techniques. A thorough investigation of the forming forces and sensitivity of simulation parameters for SPIF was performed by Henrard et al. . The most significant factors affecting the simulation's accuracy in terms of predicted forces were determined to be the type of finite element, the constitutive law, and the identification procedure used to calibrate the material parameters. Similarly, it was concluded that a fine mesh consisting of solid elements gave the most accurate force predictions.
Malhotra et al. [35,36] concluded that solid element models produced more reliable results regarding sheet thinning in SPIF, and then calibrated a simulation model which depended on damage mechanics in an effort to predict fracture. It was observed that both through-the-thickness shear and local bending around the tool take on a prominent role when predicting fracture. However, Hirt et al.  had great success in using shell elements to predict the sheet thickness distribution in SPIF. Additionally, Seong et al.  investigated the mechanics of SPIF using shell elements in order to understand why necking is suppressed in SPIF and revealed that a necking instability under bending conditions can only occur if high tension is also applied in the stress state.
Addressing multipass ISF, Liu et al.  simulated TPIF using reduced integration shell elements whereas Duflou et al.  modeled multipass SPIF with second order shell elements. Further yet, both multipass studies found that their respective simulations gave reasonable trends in strain evolution when compared to their respective multipass experiments.
Concerning ADSIF, Smith et al.  performed a full-scale simulation using 8 solid brick elements through the thickness, which took approximately 30 days to complete on 56 processors. A total of 24 simplified ADSIF simulations were carried out by Ren et al. , and although the models were reduced in size, over four months of simulation time were necessary for all of the simulations to complete.
While this is not a complete list of the work done in the field, it highlights some of the key challenges that ISF simulations are currently faced with: (1) common methods to simplify simulation models, such as utilizing axisymmetric boundary conditions, often prevent the ease of simulating general toolpaths, (2) the choice of element and implementation of numerical methods (e.g., mass scaling, mesh density, etc.) likely produce errors which are not easily quantified or comparable with experiments, (3) and most importantly in many cases, the required simulation wall time is significantly longer compared to experimentation time needed, making the utilization of simulation process design impractical.
In order to effectively improve the success of current ISF strategies, it is necessary to develop a detailed understanding of the fundamental mechanics for a given ISF setup and/or toolpath strategy. Thus, there is a need for a general simulation model that can capture the mechanics of ISF on a timely basis. Furthermore, to the authors' knowledge, there have not been published results related to simulations of conventional DSIF, and it should not be assumed that the mechanics from ADSIF simulations are necessarily the same as those from the DSIF process. Finally, it is not known from the literature how sensitive a given simulation solution is to varying numerical parameters, such as mesh density, mass scaling, or tool velocity.
The objective of this work is to accurately and practically simulate the DSIF process by means of finite element methods. To clarify, it is desired to be able to simulate the DSIF process using a standard 8 CPU computer within 48 hrs for general toolpaths of a typical part size of 200 × 200 mm. Careful attention is also placed on justifying the accuracy of the simulation model in order to determine how well the model truly captures the actual DSIF process. Some preliminary analysis of the fundamental mechanics that are observed from the simulation will also be discussed.
To determine the accuracy of a given simulation, it was first necessary to develop and characterize a DSIF part in an effort to establish a baseline for comparison purposes. As already described, toolpath parameters are related to a part's strain history and forming forces. Therefore, a short discussion will be introduced on how the tool gap was calculated using a Modified Sine Law. Then, emphasis is made on the requirement to use laser-marking in order to produce a uniform circle-grid onto the sheet metal for strain analysis. A custom-built DSIF machine at Northwestern University was used to carry out the experiments using a funnel as the desired geometry. Only aluminum 5754-O (1 mm thick) was considered in this study. The forming forces, overall geometry, thickness distribution, and surface strains were measured for comparison purposes with the simulation study.
Tool Gap in DSIF.
where A, B, C, and D are fitting constants and were defined to be A = 2.152 × 10−6, B = −3.146 × 10−4, C = 3.147 × 10−3, and D = 0.9933, noting that the wall angle is represented in degrees.
Aluminum alloy 5754-O (1 mm thick) was used in this study, and based on prior tests, it has been determined that this batch of material is prone to failure at approximately 70% thinning through the thickness. Therefore, Eq. (2) was developed  so that the tool gap, defined to be equal to the predicted thickness, was given by the Sine Law up to a wall angle of about 50 deg, at which point Eq. 2 begins to asymptote to 0.3 mm (i.e., 70% thinning) in order to prevent the tools from over squeezing. The form in which the function asymptotes closely resembles a conventional third-order smooth step. It will be seen, however, that the maximum wall angle achieved in experimentation was 66 deg which implies a difference in tool gap of only 0.06 mm, as predicted between Eqs. (1) and (2). Thus, Eq. (2) is more advantageous in multipass experiments where nearly vertical walls can occur.
There have been investigations by Meier et al.  and Lu et al.  that attempted to relate formability and the relative angle between the top and bottom tools. While there is some evidence that increased formability can be achieved with various shift angles, a simple method was chosen in this study where the local, normal vector on the desired surface was used to orientate the tool centers.
Desired Geometry and Laser Marking.
A common practice to measure surface strains in the forming industry is to use electro-etching. This was trialed with various etching agents and amperage exposures, but in general, the etched circle patterns did not reliably survive the DSIF process due to both contact rubbing and large forming pressures. Then, a laser marking setup (Fig. 2) was trialed in an effort to locally mark the surface of the metal without affecting the global material properties. An 8 ps, 532 nm (2nd harmonic) pulsed Nd:YV04 laser with 0.6 mm beam diameter was used to locally anneal the top surface of the sheet while preventing the creation of a microchannel. This laser has an average power ranging from 0.03 to 1.1 W with a max peak power greater than 1012 W/cm2.
A funnel geometry, as illustrated by Fig. 3, was chosen for the DSIF study due to its abundance in the literature and axisymmetric simplicity in design. Using the described laser setup, a pattern featuring 2 mm circles was then manufactured on the surface of the virgin sheet. The DSIF process for the funnel toolpath was carried out using sheets with and without the circle grid, and it was confirmed that the laser markings had negligible effects on both the resultant geometry and the forming forces. The circle grid will be shown later in Fig. 6, noting that the part is axisymmetric and thus does not require strain measurements to be taken everywhere.
Aluminum 5754-O, 1 mm thick, was chosen for all of the forming experiments. Tensile tests in the rolling direction (0 deg), diagonal direction (45 deg), and transverse direction (90 deg) were performed. The hardening curves were measured using digital image correlation and are given by Fig. 4. Additionally, the elastic properties can be fully defined by the Young's modulus and Poisson ratio and were measured to be 68.0 GPa and 0.32, respectively. Additionally, the r-values at 15% true strain were found to be approximately r0 = 0.75, r45 = 0.79, and r90 = 0.82.
The DSIF machine at Northwestern University (Fig. 5) utilizes a DELTA-TAU controller to move the independent X-, Y-, and Z-axes for both top and bottom tools. Piezoelectric load cells are placed in series with the forming tools allowing the measurement of both transverse and axial loads. The total forming area within the clamped region is 200 × 200 mm, and no backing plate was used during the forming process. Precision tools with a spherical diameter of 9.53 mm [3/8 in.] were chosen and multipurpose lubricant/grease infused with fluoropolymers (i.e., Teflon) was used between the tools and the sheet. Spiral toolpaths with a fixed incremental depth, or pitch, of 0.2 mm were developed in-house. The resultant funnel part is shown in Fig. 6.
As illustrated by Fig. 6, the bottom tool lost contact partway through the DSIF process, which implies that the part was actually finished using SPIF. This phenomenon has been noted before by Malhotra et al.  and is difficult to correct for without either an accurate thickness prediction of the formed part or in-situ force control loop that modifies the toolpath in order to maintain contact. In this study, it is our focus to develop a simulation framework for DSIF in accordance with experimental data, whatever that be, rather than implement modified DSIF toolpath techniques.
To measure the in-plane strains, a stereo-vision camera system was devised similar to what is used by Correlated Solutions VIC3D and their digital image correlation techniques. So long as the surface deformations of circle-grid are homogeneous, then the length of the semi-axes of the formed ellipses can be used to estimate the in-plane strains. Using a characterized, undeformed circle, this method was found to have a standard error of approximately true strain. The measured strains, and additionally the forming forces, are shown in Sec. 4 where comparisons are made between experiment and simulations.
A ROMER Absolute Arm with an integrated laser scanner was used to develop dense point clouds of the top and bottom surfaces of the formed parts. Computer-aided design (CAD) surfaces were then fitted to these point clouds using the software suite, Geomagic Design X, thus allowing the surfaces to be compared against the desired part. Using thickness measurements from a micrometer, it was determined that a given point on the resultant CAD geometry originating from the point cloud data could have a 3D positional standard error as high as mm. The fitted CAD surface, as well as the evaluated thickness distribution from the measured surfaces, are illustrated in Fig. 7.
The force and strain measurements gathered from the funnel experiment were used as a guide toward the development of the desired, practical simulation model. To begin with, a full-scale simulation of DSIF using solid elements was considered. Reduced-integration shell elements with thickness-stretch were then trialed and compared, resulting in the eventual realization and success of full-integration shell elements. All of the FEAs were performed with explicit time integration using the LS-DYNA R7.0 solver. Due to the many small deformation increments in DSIF and the ease in scaling for parallel processing, explicit time integration was chosen. In developing the model, an isotropic elastic–plastic model (i.e., J2-plasticity) calibrated to the Voce law shown in Fig. 4 was considered. The Hill's 1948 anisotropic yield criterion was tested and found to have only a small effect when compared to J2-plasticity for this particular material on both the forming forces and resultant strains. Consideration of an anisotropic model designed for aluminum alloys with kinematic hardening to more precisely capture the real material behavior is currently being pursued as future work. The static and dynamic friction coefficients were kept small (∼0.01) due to the assumption that the tools were well-lubricated. For all of the simulations, the tools were modeled as rigid bodies. Unless specifically mentioned, the same toolpath parameters used in the experiment were also used in the simulation.
Although it is instinctive to use a radial mesh for an axisymmetric part, it is the goal of this research to develop a DSIF model to simulate toolpaths without the need of changing the mesh shape (i.e., the simulation of a toolpath should ideally be mesh-independent). Hence, uniform meshes were chosen for all of the following simulations. To simplify matters, the surrounding boundary of the sheet was assumed to be fixed, which is based on the observation that sheet draw-in is not significant in ISF contrary to conventional stamping. When considering reduced integration elements, the Flanagan-Belytschko stiffness-based hourglass control formulation  was used to reduce any zero-energy deformation modes. Additionally, each simulation uses elements with six integration points through the thickness, or in the case of linear solid elements, six elements through the thickness. In an effort to be succinct, the strain comparisons between the experiment and simulation are only shown for the best-case simulation (see Sec. 4).
Reduced-Integration Shell Elements.
To begin, the preliminary results are discussed for the two simulation cases corresponding to the full-scale domain (200 × 200 mm) using (1) reduced integration solid elements and (2) reduced integration shell elements; specifically LS-DYNA's solid element ID 1 and shell element ID 25. The chosen shell element from LS-DYNA's library provides a through-the-thickness degree-of-freedom which is necessary in order to capture the triaxial stress and strain states expected in DSIF. Additionally, the shell element was formulated using Mindlin–Reissner plate theory . A continuous thickness distribution between neighboring shell elements is enforced in the simulation and the contact surface about the shell elements moves in accordance to these thickness changes.
Corresponding to these initial simulations, a tool speed of 1000 mm/s was used in combination with mass scaling so as to bring the stable time step up to 5 × 10−6 s. The element length was uniformly set to 1.0 × 1.0 mm within the center of the forming region resulting in a total of 38,416 shell elements and 230,496 solid elements. While it was expected that the element density may be too coarse to capture the correct stresses, the simulations still provide an excellent comparison between the differences in the solutions between the shell elements and the solid elements. A mesh size study is performed subsequently. The principal (i.e., major) true strains of the resultant simulations are compared in Fig. 8.
It is immediately clear from Fig. 8, that the strains from the solid elements simulation are not axisymmetric. Additionally, the resultant shape of the funnel is not similar to what was observed in the real DSIF experiment. The solid elements experienced different stress-states when they underwent tension compared to shear, even with the use of hourglass controls. Therefore, utilizing solid elements with the desired amount of mass-scaling may actually be mesh-dependent. Quantitatively, over 4 × 104 times the initial mass of the sheet was added in order to provide a stable time step 5 × 10−6 s for the solid element simulation. It would appear that simply too much mass was added to the solid element simulation due to the small element lengths through the thickness, and this caused the material to be severely dampened and exhibit erroneous results. On the contrary, the shell element simulation demonstrates a more axisymmetric solution. Furthermore, both simulations were computed on 24 CPUs and the shell element simulation finished in approximately 72 hrs while the solid element simulation required twice that. Therefore, all further attempts to better the simulation model with regards to speed and accuracy were done using shell elements as the fundamental element technology.
To be clear, though, previous simulation studies of ADSIF and SPIF have been investigated using solid elements with what appear to contain excellent results so long as adequate time was given to complete a simulation using less mass scaling. To achieve accurate results with solid elements, it seems that a wall time on the order of weeks using 24 CPUs or more is required. The choice to use shell elements in this study is due to the need to dramatically decrease the CPU wall time of the DSIF simulation while still maintaining a good approximation of the DSIF process.
Upon closer inspection of the shell element simulation, however, the forming forces exhibited different trends when compared to the experiments (Fig. 9). Note that the simulation time, not to be confused with CPU wall time, is smaller due to increased tool velocity and that the experimental timescale has been scaled accordingly. Force oscillations in the solid element simulation were observed due to the lack of mesh independence causing dramatically different stresses to be experienced around the profile of the funnel. In the shell element simulation, the bottom tool lost contact with the sheet prematurely whereas the solid element simulation exhibits overall too large of values for the forces. It is assumed that the loss of contact with the bottom tool in the shell element simulation also resulted in a loss of through-the-thickness pressure, which would have helped to stabilize the material to resist thinning. The lack of this stabilization eventually led to elements that were so thin and easily deformable that the simulation became unstable resulting in the observed force oscillations present near the end of the simulation.
To improve the accuracy of the simulation, different mesh densities were tested to examine whether the simulation could better capture through-the-thickness effects with the reduced integration shell elements (Fig. 10). To aid in the reduction of time to complete these computationally expensive simulations, the spatial domain was reduced in size to 150 × 150 mm. It is assumed that the elastic bending that is occurring outside of the forming area does not play a strong role in the forming process and therefore can be neglected. This is not likely a reasonable simplification if one is seeking springback effects since elastic recovery is the primary stress reliever during springback. Thus, the following simulations are primarily concerned with the effects of significant material deformation and are not directed toward precise predictions of part geometry since the simulation of springback is beyond the scope of this study.
The choice of using a 150 × 150 mm reduced scale model seems justified since the forming forces, and consequently the resultant thicknesses, were similar to those of the full scale model (Fig. 10). However, it is apparent that the bottom tool continues to lose contact far too early in the simulation, despite a significantly more refined mesh. Varying the mass scaling and/or increasing the global mass damping did help to better the validity of the simulation but significant differences were still observed when compared to the experiment. Because of premature thinning, it is clear that the reduced integration element was not adequately capturing the through thickness effects of the DSIF process. It was hypothesized that the approximations made using reduced Gaussian integration were too coarse and that using the full number of integration points would lead to more accurate strain increments. This led to the decision to use fully integrated elements with thickness stretch (LS-DYNA's shell element ID 26).
Full-Integration Shell Elements.
After changing the shell element formulation to a fully integrated scheme, it is quick to notice from Fig. 11 that the final part geometry has improved and does not resemble a truncated cone as before. Nonetheless, another mesh study using fully integrated shell elements was performed and the force results are illustrated in Fig. 12. When using fully integrated shell elements, the bottom tool's force profile is much closer to what is observed during experimentation. Additionally, the simulation changed very little after refinement suggesting that the solution is close to converging. A total of 14 simulations were completed using the fully integrated shell elements to see the effects of varying other numerical parameters such as mass scaling, contact penalty stiffness, and so forth. There were only small differences in the resultant solutions; nonetheless, the details are briefly discussed.
First, the tool's velocity was chosen to vary between 500, 1000, and 1500 mm/s, though, negligible differences were observed in the simulation solution regarding forming forces or resultant strains. So long as the tools are modeled as rigid elements, the internal energy dominates due to plastic deformation rather than the localized kinetic energy induced by toolpath displacements. Including a shear correction factor of 5/6 within the Mindlin–Reissner constitutive equations, as suggested by the LS-DYNA theory manual, did very little to alter the solution, as well. Occasionally, second order terms are required in a simulation to accurately capture large, rotational displacements. However, negligible changes were observed after including second order terms from the *CONTROL_ACCURACY card block. The penalty stiffness for the contact algorithm was reduced in half relative to the default value and some changes in the trend of the force profile were observed. However, the magnitude of the forces and location of where the bottom tool lost contact was nearly unaltered. Doubling the penalty stiffness had a similar outcome.
It was found, though, that after increasing the mass scaling to achieve a time step of 1 × 10−5 s from 1 × 10−6 s, there was approximately a 10% increase in the maximum error regarding the forming forces when compared to Fig. 12. However, it was assumed that these differences did not alter the solution significantly considering that an order of magnitude of additional mass was added.
Upon completing the aforementioned simulations, it was concluded that the simulation solution using the 0.75 mm mesh is the approximately converged solution of the simulation. The chosen parameters for the converged shell element model are summarized by Table 1. In short, the 0.75 mm fully integrated shell element mesh used a wall time of only 23 hrs when using 8 CPUs, a tool speed of 1500 mm/s, and a time step of 1 × 10−5 s.
Results and Discussion
The forming forces given by Fig. 12 for the fully integrated shell elements are only in fair agreement with those observed in the experiment. The general trend of the forces is well-captured while the magnitude of the simulation forces is off by as high as 250 N. One of the reasons that could cause this difference is due to the fact that the machine compliance is not accounted for in the simulation, which creates a difference between the desired toolpath and the actual toolpath used in the experiment. Because of the machine compliance, it is likely that the experimental setup does not enforce as high of a squeezing pressure as would be expected with perfectly rigid tools. Although the reduced scale domain of the simulation significantly helps to reduce computational costs, this assumption also may induce some amount of error in the location of where the bottom tool loses contact. The supporting tool, or bottom tool, lost contact with the part at a depth of 22.7 mm and 19.5 mm for the experiment and simulation, respectively. Despite some of these disagreements, the overall mechanics of the process are still captured, as will be shown in the forthcoming strain comparisons.
Since forming forces are only one aspect to characterize the accuracy of the simulation, further investigations were pursued using the fully integrated shell element simulation described by Table 1. Figures 13 and 14 illustrate geometric and strain comparisons between the experiment and simulation. The primary goal of the simulation is to capture the plastic strains during the DSIF process and that springback is not the focus. Nonetheless, to present a fairer geometric comparison between the simulation and the experimental data, an implicit load step after the DSIF simulation was performed so as to estimate springback. As performed in standard practice , three separate nodes in the model had some or all of their translational degrees of freedom fixed in order to fully constrain the part.
In Fig. 13, the trends in the simulation geometry, such as the maximum wall angle as well as where necking occurs, agree well with what is observed in the experiment. Nonetheless, the simulation cross section is still lower than the experiment's profile. This is partially due to the fact that the simulation domain, and hence the elastic domain, is reduced in size which reduces the amount of springback. As will be discussed, factors such as damage and kinematic hardening were neglected from the constitutive law so as to simplify the comparisons between different models. These constitutive assumptions, however, do have an additional effect on the accuracy of the springback analysis. Shown in Fig. 14, nonetheless, the plastic strains have been estimated quite well by the simulation model.
The thickness distribution obtained from the simulation is compared to the experimental data, with the minimum value in excellent agreement (Fig. 14). Additionally, the major true strains of the simulation agree very well with those measured in the experiment. The largest difference in the thickness distribution appears to be in the range of 20 and 25 mm from the center of the part. This is also close to where the bottom tool lost contact for the simulation, which was slightly premature when compared to the experiment. As aforementioned, machine compliance was not modeled in the simulation and may contribute to some of these deviations. Additionally, a more comprehensive material model than isotropic J2-plasticity, or Hill's 1948, would likely further improve the agreement in the simulation. Incorporating a mechanics- or a materials-based failure model would benefit the accuracy at necking leading to fracture . Recent damage models and fracture studies performed by Martins et al.  and Xue et al.  have noted that fracture may be dependent on both pressure and Lode angle. The effect of implementing a weakening function dependent on an internal variable, namely damage, has been shown to more accurately capture strain evolution postnecking. Therefore, it is also reasonable to assume that the isotropic J2-plasticity model used in this simulation study is not adequate enough to completely predict the postnecking behavior seen at a radial distance of approximately 14 mm. More comprehensive constitutive models are being explored in future work. However, what is emphasized here is the novel simulation framework which can still approximately capture the 3D mechanics of DSIF while requiring significantly less simulation wall time.
Some preliminary conclusions can still be made from the DSIF simulation results. Regarding the thickness prediction, recall that the modified sine law was chosen and that this estimated value also defined the tool gap. For completeness, experiments were also performed using the conventional Sine law only to note that the bottom tool still lost contact with the sheet at some point in the forming process. Since contact was lost before completing the part, it is clear that the Sine Law, which is based solely on the wall angle, is too simplistic a choice in defining the tool gap for general DSIF features. This is not surprising since many of the kinematic assumptions made in the sine law are violated. In particular, the hydrostatic pressure through the thickness appears to create local material stabilization, and when the tool contact is lost, the material exhibits a necking phenomenon. This is best seen in Fig. 14 where a distinct change of slope is observed in the thickness profile after necking (i.e., 14 mm radial distance 25 mm). As stated before, there is substantial experimental evidence that SPIF tends to fail prior to the onset of necking. However, it does appear that if a DSIF toolpath fails because of a loss in tool contact, then a localized neck can occur. With a faster simulation model, it may be feasible in the future to use FEA as a framework toward better thickness prediction models and hence more successful DSIF toolpaths.
A simulation framework that can simulate the ISF process, namely, DSIF, was developed without the necessity of weeks or even months of computational time. The accuracy of the resultant simulation was verified using experiments and was found, to be good, particularly regarding the principal plastic strains.
In the experiment, an axisymmetric funnel part was formed in 1 mm AA5754-O sheet metal and carefully characterized by means of force, thickness, in-plane strain, and overall geometry. Then, a reduced-scale finite element simulation model was developed in LS-DYNA which utilized fully integrated shell elements with a thickness degree of freedom. Simulation parameters (e.g., element type, mass scaling, and tool speed) were varied in order to study the sensitivity of the simulation with respect to accuracy and speed. The finalized simulation model contained 40,000 elements and was able to simulate the funnel toolpath (total length approximately 25,800 mm) in only 23 hrs using 8 CPUs.
The simulation was compared directly to the experimental measurements and found to agree well. The minimum thickness and major true strain predicted by the model differed not more than 0.05 mm and 0.11, respectively. While the forces in the simulation were generally higher (as much as 250 N) than those measured in the experiment, similar trends were observed with particular interest on the depth where the supporting tool lost contact with the part. The difference in force measurements may be partially due to the fact that machine compliance was not accounted for in the simulation. In the future, a more descriptive constitutive relation will be incorporated into the simulation, such as a damage model, in an effort to further increase the accuracy as well as to predict fracture.
Thanks are given to Mr. Marco Giovannini, Mr. Jacob Smith, Mr. Ebot Ndip-Agbor, and Miss Zixuan Zhang for their technical advice. The authors would like to acknowledge the Department of Energy (U.S. DE-EE0005764) and the National Science Foundation (GRFP DGE-1324585) for their support.