Effect of machine compliance on mold deflection during injection and packing of thermoplastic parts.

INTRODUCTION

A major issue in manufacturing precise plastic parts through injection molding is the deflection of the mold. In fact, for ultra-precise parts, such as fiber optic connectors, a final part deformation of a few microns is enough to scrap the part. Clamping and cavity pressures during the filling and packing phases can cause the mold to deflect and distort significantly from its intended configuration. Mold deflection can lead to over-packing, resulting in parts with dimensions greater than the original mold cavity dimensions [1]. Misalignment of the mold platens across the parting plane often results in out-of-tolerance conditions. Ideally, the mold does not deform under pressure and maintains the original cavity dimensions throughout the injection cycle. In reality, both the mold and the injection-molding machine are compliant and will deform upon being loaded. The machine is inherently designed to minimize deflection, but some deflection is unavoidable and is, in some respects, even desirable. If the mold and machine were not compliant, high levels of stress could develop in the mold during the injection cycle. Such stress could cause increased mold and machine wear over the life of the mold [2].

In addition to its effect on part precision, mold deflection is a very important consideration for secondary processes such as in-mold coating (IMC) [3, 4]. With the IMC process, a thin coating, formulated to either enhance the properties or to improve the aesthetics of the underlying substrate, is injected over the surface of the thermoplastic substrate prior to the ejection of the part from the mold. The compressibility and shrinkage of the substrate allow space for the coating to flow. Mold deflection occurs not only during the injection of the substrate, but also during the injection of the coating. Therefore, understanding how a given mold will distort during injection of both thermoplastic and coating is important for completely modeling the in-mold coating process for thermoplastic parts.

Chen et al. [5] studied the influence of injection-molding process parameters, including injection speed, melt and mold temperature, filling/packing switchover, and packing pressure, on mold separation for thin-wall moldings under different clamping pressures. A finite element model of the mold using ANSYS [TM] with injection pressures from MoldFlow[TM] was developed to predict mold separation. The model showed a general correlation with measured values, but underpredicted mold separation values when compared with experimentally measured mold separations, with predicted values up to an order of magnitude lower than measured values.

Significant experimental research has been conducted in the area of mold deflection. Leo and Cuvelliez [1] investigated the effect of various process parameters on a thin plate with a width of 40 mm and length of 150 mm. The part was equipped with a variable thickness fan gate. Over-packing of the part occurred at moderate packing pressures (~60 MPa), causing a residual pressure to exist in the mold cavity after the injection and packing cycles were completed. Mold elasticity was determined to be the dominant factor controlling over-packing.

Boitout [6] identified three primary modes of elastic deformation in injection molding. The first mode is the mold opening at the parting plane, which is typically caused by insufficient clamping pressure. The second mode is the compression of the steel mold under injection and packing pressure; and the third mode is the bending of the mold halves due to mold cavity pressure. Theoretical calculations of local mold deflection have been solved by Delaunay et al. [7] using a simple thermoelastic calculation of over-packed polymer plates. Through this work, it was found that the percentage of negative shrinkage, i.e., overfilling, increased with packing pressure. Further, the pressure history inside the mold cavity was altered by mold deflection.

Die casting, which is similar to injection molding in that a molten metal is injected into a metal cavity, has been the focus of substantial mold deflection work [8-10]. For the die casting simulations, both uncoupled transient thermal and structural simulations were completed. These studies differ from similar injection-molding studies in that the die is not modeled as a stand-alone component with approximate boundary conditions, but rather it is modeled as a component within the die casting machine. This larger model is necessary because it was found that the compliance of the machine significantly affects the distortion and relative motion of the two die plates. Indeed, inclusion of machine compliance was required to achieve correlation between experimental findings and analytical predictions. Mold-only models of the injection-molding process found in the literature also tend to underpredict deflections. This study therefore includes the effect of machine compliance on in-process injection-mold behavior.

EXPERIMENTAL

The part tooling used in this research is an experimental flat plate mold, which is 1.905 mm thick and measures 152.4 [mm.sup.2] as shown in Fig. 1. The part is made from GE Plastics Cycoloy MC1300, an ABS/Polycarbonate blend. There is a 5.08-mm wide flange that has a thickness of 0.635 mm around the perimeter of the part. A tab is located along the top end of the part to permit injection of the coating after molding.

[FIGURE 1 OMITTED]

The molding process conditions were adjusted to obtain a complete, fully packed part. A shot size of 68.5 [cm.sup.3] was required to completely fill the part. The plastic was injected at 274[degrees]C, while the mold surface temperature was maintained at 90[degrees]C using four heater plates attached to the mold. A velocity of 73 mm/s was specified for the filling phase. The switchover from filling to packing occurred when the screw reached a position of 16.51 mm, which took ~1.3 s.

The first packing stage terminated at 1.6 s of the cycle time, 0.3 s after the filling is complete. A pressure of 21.87 MPa was specified for the first stage of packing. The second packing stage at a pressure of 32.81 MPa lasted 7.0 s.

A series of experiments were conducted on a Sumitomo 50-metric ton hydraulic injection-molding machine (SH50M) to verify the structural model created in ABAQUS[TM]. The strain induced by the flat plate mold in this machine was experimentally determined using strain gage rosettes to measure strain on the mold during an injection cycle. These experimental in-plane strain results were compared with the model results at three different points in the process: mold clamping load only, end of polymer fill, and maximum packing pressure. Strain gage rosettes 1, 2, and 4 were mounted in the locations where the maximum strain was anticipated, while rosette 3 was mounted on the modular base to help determine its deformed shape. A resolution of approximately three microstrains was obtained during data collection. Figure 2 shows the location of the strain gage rosettes on the movable half of the mold and modular mold base unit. In addition to the strain gage rosettes, a linear variable differential transformer (LVDT) was used to measure the screw position during the injection process. Finally, a combined pressure/temperature sensor was utilized inside the movable portion of the mold to verify conditions inside the mold cavity. The sensor was a Kistler Type 6190, which was specifically designed for dynamic temperature and pressure measurements inside mold cavities. The sensor is capable of measuring pressures up to 200 MPa and temperatures up to 450[degrees]C. The face of the sensor inside the mold is 4 mm in diameter. The tip of the sensor is located 63.5 mm above the sprue along the centerline, as denoted in Fig. 1.

[FIGURE 2 OMITTED]

The parameters used for the verification experiments were identical to those used as input for the simulations. To ensure identical operating conditions for each experimental run, the mold and plasticizer temperature were allowed to recover for 15 min after each shot. A hand-held thermocouple was used to verify uniform mold surface temperature before each shot. Ten consecutive runs were conducted for each rosette, with data recorded for each rosette individually.

SIMULATIONS

Clamping pressure and cavity pressure constitute the loading on the mold and the injection-molding machine throughout the molding process. The cavity pressure for the mold deflection analysis was predicted using a coupled flow-thermal model in MoldFlow. This pressure was then imported into ABAQUS, where it was applied to the mold faces for the quasi-static deflection analysis.

The specifications for the Sumitomo SH50M as well as the parameters outlined above were entered in the Mold-Flow analysis. Two instances during the injection cycle are of particular interest. The first instance is the end of polymer fill, which occurs at 1.3 s in the cycle. The pressure gradient within the mold is very high at the end of polymer fill with zero pressure at the flow front and a peak pressure inside the mold cavity 28.70 MPa. The second point of interest is the time at which the maximum packing pressure is observed and the maximum clamping force is required. From the mold simulations, this occurs 2.66 s after the cycle has begun. The maximum mold deflection is expected at this point. Unlike the pressure at the end of polymer fill, the pressure distribution at the maximum packing pressure is more uniform within the mold cavity. The peak pressure inside the mold cavity at this time is 28.76 MPa and occurs during the second stage of packing. Figure 3 shows the calculated pressure distributions inside the mold cavity at the end of filling (Fig. 3a) and maximum packing (Fig. 3b) conditions. The calculated pressures at the sensor are compared with the experimentally measured pressures in Fig. 4. The vertical dashed lines correspond to the two time periods of interest. The pressure sensor in the mold shows a pressure that makes a smooth transition from the filling phase to the packing phase. The actual injection unit shows an overdamped response with no overshoot. When the experimental response time for the Sumitomo's injection unit is used in MoldFlow, a pressure overshoot is predicted which deviates from what is observed by the pressure sensor. At the two points of interest, however, close correlation between pressure prediction and measurement are obtained.

[FIGURE 3 OMITTED]

Two different structural models were used to predict the mold deflections: a mold-only model, and a model of the mold within the injection-molding machine. In the first model, many machine components were replaced with boundary conditions to minimize the simulation size, which in turn reduced the computational time. Figure 5 shows the five components used for this model: the ejector platen, the modular mold base on the ejector side, the movable mold half, the fixed mold half, and the modular mold base on the sprue side.

[FIGURE 4 OMITTED]

The boundary conditions for the mold-only model are illustrated in Fig. 6. The back face of the modular mold base on the fixed side was constrained in all directions to simulate the effect of the fixed platen that was not included in the model. The tie rods were modeled as a displacement constraint on the ejector platen in the in-plane directions. The ejector platen is free to translate along the tie rods. Contact was defined between the mold halves and between the movable mold half and its mold base. Tied contact was specified between the mold base and the ejector platen at the locations of the clamps mounting the base to the platen. Clamping pressure and mold cavity pressure were the two traction boundary conditions applied to the ABAQUS model. Because of the symmetry of the components, the displacement boundary conditions, and the cavity and clamping pressures, a half symmetry model was utilized in the structural simulations. The "S" on the boundaries of the model in Fig. 6 denotes the symmetry surfaces on which all displacement in the 1-direction was constrained to zero.

[FIGURE 5 OMITTED]

[FIGURE 6 OMITTED]

The mold-only model simulations underestimated the actual strain in the mold during an injection cycle. Therefore, a second model, illustrated in Fig. 7, was constructed to more accurately re-create the structural rigidity of mold and machine. In this model, the fixed platen, the four tie rods, the hydraulic cylinder, and the cylinder support were added to the mold-only model.

The stationary platen was included to model properly the support of the fixed mold half. Since the stationary platen and its supporting tie rods on the back face of the platen are asymmetric, the plane of symmetry no longer could be used for this model. Tie rods which link the two platens and the cylinder support were modeled to determine the overall machine distortion. The clamping system was modeled through the hydraulic cylinder and cylinder support. These components were modeled to predict the effect of machine compliance on mold deflection.

The weight of the oil reservoir, located at the back of the cylinder support, was modeled as a point load at the reservoir's center of gravity. The filled reservoir's weight (~2000 N) is transferred to the back of cylinder via a distributed coupling constraint, which applies the load at a reference node located at a distance of 295 mm from the back face of cylinder support. A node set was specified for the nodes on the face of the cylinder support where the force and moment resulting from the reservoir would be acting. This constraint couples the motion of the nodes in the node set to the motion of the reference node.

[FIGURE 7 OMITTED]

The structural effects of the injection unit behind the stationary platen were replaced by boundary conditions. During polymer injection, the injection unit moves forward into the opening of the stationary platen. The structural effect of this moving injection unit is to support the stationary platen during the injection cycle. The injection unit was modeled as a displacement constraint along the longitudinal axis of the machine at the circular location where the injection unit comes into contact with the stationary platen during an injection cycle. In addition, the two asymmetrically placed tie rods connected to the back of the stationary platen were modeled as fixed boundary conditions in the longitudinal axis of the machine.

Both models used eight node linear brick elements with incompatible modes and a linear elastic, homogeneous, isotropic material for each part in the assembly. The mold is made of P20 tool steel, while the mold bases are made of cold-rolled low carbon steel. The tie rods are made of high carbon steel, and the platens and cylinder support are made from cast iron. All the components except the platens were modeled using the properties of steel with an elastic modulus of 206 GPa, a Poisson's ratio of 0.3, and a density of 7.87 kg/[mm.sup.3]. Since the exact composition and processing of the cast iron is not known, there is some uncertainty in specifying the material properties. A second analysis using a lower value of the elastic modulus for the cast iron was conducted to determine sensitivity of the simulation results to a variation in cast iron material properties. The predicted mold deflection values did not vary significantly with the change in modulus, and therefore, a midrange elastic modulus of 140 GPa, Poisson's ratio of 0.3, and a density of 7.2 kg/[mm.sup.3] were specified for this analysis [2].

The penalty method was utilized to model all part-to-part interactions. All interactions were small sliding steel-on-steel with an unlubricated interface. A static friction coefficient of 0.5 was used for the contact between the unlubricated steel components. A sensitivity analysis determined that the specific value of the coefficient had little effect on the final solution results.

Contact pairs were used to define mechanical interactions between the surfaces of the deformable parts of the molding machine. The contact pairs of the mold-only model were expanded to include contact between the ejector platen and the ejector mold base, the fixed mold half and its mold base, the mold base on the sprue side and the stationary platen, the cylinder support and the hydraulic cylinder, the ejector platen and the tie rods. In addition, each end of each tie rod was held in place using tied contact with the cylinder support and with the stationary platen. Tied contact was also used to clamp the sprue side mold base to the stationary platen.

[FIGURE 8 OMITTED]

A thermal simulation of the mold was not conducted because of the mold being uniformly heated to 90[degrees]C, which reduces the temperature differential between the mold and polymer during injection. A flash heating of the mold occurs during the injection cycle, but the heat quickly dissipates throughout the mold. It was assumed that the strain due to pressure loading would be far more significant than the thermally induced strain.

RESULTS

Data were collected from each rosette for 10 shots (parts). There was very little variation in the experimental strain between each shot. Figures 8-11 show representative data collected from each rosette during an injection cycle. Each chart has the three gage readings in each rosette. Additionally, the screw position throughout the cycle is shown to indicate the progression of the cycle. Because of the limitations of the data acquisition system, a resolution of approximately three microstrain was obtained during data collection.

[FIGURE 9 OMITTED]

[FIGURE 10 OMITTED]

The data have three distinct regions for each injection cycle. The first region contains a constant strain level when the mold closes and the clamping pressure is applied. The steep increase in strain is characteristic of the injection of polymer into the mold cavity. The final region is the packing phase; this is the region in which the strain reaches its maximum value. The strain is lessened as the part shrinks in the cavity, but the strain is not completely eliminated until the mold opens for part ejection. This residual strain, which exists after the packing pressure is removed, is most likely caused by overpacking of the part [2].

Structural simulations using both models were completed for three different loading scenarios for the mold. The first simulation solved the mold deflection with only the clamping force applied. Mold cavity pressures, obtained from MoldFlow, were included in the remaining two simulations. The cavity pressures at the end of polymer filling and at the time of maximum packing pressure, in addition to the clamping force, were used to determine the structural deformation at those instances.

[FIGURE 11 OMITTED]

[FIGURE 12 OMITTED]

The deformed shape of the loaded mold and machine is of interest. Figure 12 illustrates the bending of the movable mold half due to injection pressures. The figure also shows the loss of contact the mold base unit undergoes with the ejector platen, indicating that the clamps, which attach the mold base unit to the platen, are unable to prevent the bending of the back of the mold base unit. The loss of contact means larger displacements of the mold base unit and a corresponding increase in strain values of rosette 4.

The asymmetric placement of tie rods on the back of the stationary platen causes a global twisting of the molding machine, especially the tie rods (Fig. 13). The effect of this twisting can be seen in the predicted variation in the ejected part thickness variation. The net variations for the mold, illustrated in Fig. 14, indicate a maximum variation of 0.067 mm at the center of the mold, which is expected, as the injection pressures applied have a maximum magnitude at the center of the mold. The deflections of the mold, however, are nonuniform, with one side deflecting more than the other, in addition to the larger deflections along the vertical centerline than the edges. This indicates that the machine undergoes twisting as well as the expected bending. The largest thickness variation occurred at the maximum packing pressure where the mold pressures are highest and the mold deflects the most. A maximum of 0.067 mm part thickness variation was predicted at the center, and a maximum of 0.041 mm part thickness variation was predicted around the perimeter of the flange. When compared with 1.905 mm designed part center thickness and the 0.635 mm designed flange thickness, this results in an ejected part 3.51% thicker than designed at the center and 6.45% thicker at the flange.

[FIGURE 13 OMITTED]

[FIGURE 14 OMITTED]

A comparison between experimental and predicted strain is shown in Fig. 15-18. When comparing the experimental strain with the strain predicted by ABAQUS, a few general trends were identified. First, both structural models accurately predict the relative magnitude of the strain throughout the injection cycle. For example, the strain due to clamping is less than the strain at the end of fill, which in turn is less than the strain at maximum packing. However, it is clear from these figures that the mold-only model underpredicts the measured strain at each location. The mold and machine model, although closer than the mold-only model, also underpredicts the experimentally determined normal strain in transverse or mold bending direction of rosettes 1 and 2. For rosettes 3 and 4 located on the ejector mold base unit, however, predicted results matched well with the experimental results and improved much over the mold-only model. Comparing experimental and predicted strain results of these rosettes on the mold base unit, it can be concluded that the machine compliance has been simulated correctly.

[FIGURE 15 OMITTED]

[FIGURE 16 OMITTED]

The amount by which the strain in the mold is underpredicted is far larger than what one could reasonably expect from thermal effects alone. Further, the difference between experimental and analytical is approximately constant and exists for all three loading conditions. For this reason, it is believed that the difference in the strain is largely due to a local effect such as mold misalignment, particularly in the IMC tab region of the mold. (See Fig. 19)

[FIGURE 17 OMITTED]

[FIGURE 18 OMITTED]

CONCLUSIONS

This study addresses injection-mold deflection and the role of the compliance of the injection-molding machine on these deflections. This work included the development and verification of the finite element model of an experimental flat plate mold in a Sumitomo SHM50 injection-molding machine. A comprehensive nonlinear finite element model of the injection-molding machine comprising the platens, mold halves, master unit dies, hydraulic cylinder support, hydraulic cylinder, and tie rods was constructed to include most of the factors that affect mold deflections and strains. Three separate load cases namely, clamping load only, end of polymer fill, and maximum packing pressure as related to injection-molding process were analyzed to determine the strain and mold deflections. The predictive capability of the simulation model was verified by comparing the strains from the simulation model with the experimental measurements. The maximum mold deflection for the experimental mold used for this work occurred during the maximum packing pressure of the part as anticipated for this geometry. However, the maximum deflection could occur during filling with different process parameters and part geometry.

This work has shown through experimental correlation of the strain results on the ejector mold base unit and improved predictions of the movable mold half strains that machine compliance has been correctly modeled. This machine compliance causes twisting of the global machine model and bending of the mold halves. This deformation affects the overall quality of the part and must be quantified. The predicted strain results for the mold and machine model confirm that machine compliance has a considerable influence on mold deflections. Significant reductions in mold openings were predicted for the mold and machine model for all the load cases when compared with the predicted mold openings in the mold-only model. Variation in part thickness indicated that mold deflection can be significant and can vary with location within the mold because of compliance effects.

[FIGURE 19 OMITTED]

The work discussed has laid the foundation for a more detailed investigation of mold deflection. Finite element analysis provides an effective means for analyzing the mold deflection, while requiring little capital investment. Future work includes the analysis of a flexible mold in the polymer injection simulation to get a more accurate starting point for the structural analyses. Polymer flow simulations generally assume rigid molds, which do not deflect during injection and packing. These ideal molds do not deform under applied force and pressure and maintain the cavity dimensions throughout the cycle. However, both the mold and injection-molding machine are compliant and will deform upon loading. Further, the effects of mold misalignment on mold stresses and strains need to be quantified. The current flat plate mold makes it difficult to measure the small variations in the part due to mold distortion and misalignment. A new mold, which features concentric cylinders on opposite sides of the parting plane, is under development to further quantify the effects of mold compliance on finished part dimensions.

In-process mold deflections can result in dimensional variation among molded parts, in some cases resulting in parts that do not meet the tight tolerance requirements common in electronic and optic components. Prediction of in-process mold deflection, therefore, is critical to all high-precision molding applications.

ACKNOWLEDGMENTS

The authors gratefully acknowledge the support of Mr. Gary Glozer of the Eastman Kodak Company and Bob Miller and Mary Hartzler of the Industrial, Welding, and Systems Engineering Department at the Ohio State University.

REFERENCES

1. V. Leo and Ch. Cuvelliez, Polym. Eng. Sci., 36, 1961 (1996).

2. B.S. Carpenter, Mold Deflection During In-Mold Coating Process--Simulation and Verification, master's thesis, The Ohio State University, Columbus, OH (2004).

3. X. Chen, N. Bhagavatula, and J.M. Castro, Model. Simul. Mater. Sci. Eng., 12(3), 267 (2004).

4. X. Chen and J.M. Castro, J. Injection Mold. Technol., 6(4), 272 (2002).

5. S. Chen, W. Liaw, P. Su, and M. Chung, Adv. Polym. Technol., 22(4), 306 (2003).

6. F. Boitout, "Calcul des Contraintes Residuelles dans les Pieces Injectees en Thermoplastiques en Utilisant une Description Surfacique de Lageometrie," Ph.D. Thesis, CEMEF, Sophia Antipolis, France (1993).

7. D. Delaunay, P. LeBot, R. Fulchiron, J.F. Luye, and G. Regnier, Polym. Eng. Sci., 40(7), 1692 (2000).

8. H. Ahuett-Garza, K. Hedge, and R.A. Miller, Die Cast. Eng., 39(2), 18 (1995).

9. H. Ahuett-Garza, K. Hedge, and R.A. Miller, Die Cast. Eng., 39(6), 22 (1995).

10. A.E. Ragab, Sensitivity Analysis of Casting Distortion and Residual Stress Prediction through Simulation Modeling and Experimental Verification, Ph.D. Thesis, The Ohio State University, Columbus, OH (2003).

Brian Carpenter 

Department of Mechanical Engineering, The Ohio State University, Columbus, Ohio 43210

Sachin Patil, Rebecca Hoffman

Department of Mechanical Engineering, Villanova University, Villanova, Pennsylvania 19085-1691

Blaine Lilly

Department of Industrial Welding and Systems Engineering, Department of Mechanical Engineering, The Ohio State University, Columbus, Ohio 43210

Jose Castro

Department of Industrial Welding and Systems Engineering, The Ohio State University, Columbus, Ohio 43210

Correspondence to: Rebecca Hoffman, Assistant Professor. Department of Mechanical Engineering, Villanova University, 800 Lancaster Avenue, Villanova, PA 19085-1681; e-mail: [e-mail]

Contract grant sponsor: The National Science Foundation: contract grant number: DMI-0217664.