Injection-Molded Polyester Medical Devices: Preventing Failure through the Proper Design of Parts and Molds

Medical Plastics and Biomaterials Magazine | MPB Article Index

Originally published September1997

PART DESIGN

Medical part quality depends on factors that include part design, resin selection, the quality and design of the molding tool, and processing conditions. Design and molding considerations, in turn, depend on the type of resin to be molded. The following general guidelines and examples are given to aid in the proper design of parts and

Precision parts such as injection-molded winged luers are among the many medical products made from polyester resins. Photo: Eastman Chemical Co.

molds for medical-grade polyesters. (The polyester resins referred to in this article were Eastar polyesters/ copolyesters and Eastalloy polymers, produced by Eastman Chemical Co., Kingsport, TN). By understanding how part design affects injection molding, tooling, and production costs, part designers and engineers can significantly reduce mold complexity. By understanding how tool design affects the processability of polyester resins, they can avoid complications during molding.

PART DESIGN PRINCIPLES

The goal of the medical part designer should be to provide a part that combines maximum functionality with minimum complexity. The following principles are useful for the designer to keep in mind when designing a part that will incorporate any thermoplastic resin. As simple as these principles are, many are often overlooked, resulting in increased mold costs, a defective final product, or premature part failure.

Wall Thickness. The most basic principle of plastic part design is that uniform wall thickness should be maintained wherever possible. Thin sections are weak structurally and difficult to fill; they can restrict flow and require increased injection pressure. Thick sections are easier to fill but difficult to cool and pack out; they are subject to increased shrinkage, and may cause sink marks, voids, and high levels of molded-in stress. When thickness variations are unavoidable, they should be designed with a gradual transition, which will help reduce the level of molded-in stress at the transition region.

Corners are often problem areas because of nonuniform thickness. If the outer radius is too small, a thick section is created in the corner; this increased thickness then causes cooling and warpage problems. If the outer radius is too large, the corner will be thinner than its adjoining walls. Besides being weak structurally, the change in thickness can serve as a flow restrictor. The best approach is to have the inner and outer radii originating from the same point, ensuring a uniform wall thickness through the corner. A good rule of thumb is to have the inner radius value 1Ž2 the wall thickness, and the outer radius 11Ž2 times the wall thickness.

Stress Concentration and Sharp Corners. Stress concentrations are areas that by the nature of their design tend to concentrate or magnify the stress level within a part. Figure 1 shows how the stress concentration factor in an inside corner will increase rapidly as the radius decreases. A good rule of thumb is to specify a minimum radius of 1/4 the wall thickness. Sharp corners should be avoided in critical stress locations such as inside corners, and at the base of ribs, bosses, and snap-fit latches.

Figure 1. The curve gives an indication of the relationship among stress, wall thickness, and corner radius for plastic parts. (Figure courtesy of SPI Plastics Engineering Handbook, 5th ed, p 323.)

Designing for Proper Ejection. Once a part is molded, ejecting it from the tool without damaging it or the tool is important. Zero degree draft is not recommended, as it can cause a part to remain in the mold, locking it up. It can also increase the cost of the mold significantly due to the additional mechanisms required for ejection.

For proper ejection, a draft of 1° per side is typical. Less than 1° is suggested only in cases where adequate cooling is supplied, the cores are short, the part walls are thick so as not to shrink tightly to the core, or sleeve ejectors are used. Sometimes side pulls can be employed on the outside of a cylindrical part so that low draft on the inside core can be easier to release. If texturing is incorporated in the mold, between 1° and 1.5° of draft for each 0.025 mm (0.001 in.) of texture depth should be added.

PART DESIGN FOR ASSEMBLY

There are many instances in which medical devices require assembling. Solvents and adhesives can often be used successfully in assembly, but such bonding agents are not acceptable for every application.

Ultrasonic welding can also be performed effectively with polyester materials, if certain design considerations are observed. Shear-type joints--which produce strong, hermetic seals--should be used. The advantages of shear joints over energy directors are that joint strengths can be doubled, crack-propagation behavior is reduced, loads are more evenly distributed during use, and joint flash can be controlled. In some limited situations, energy directors may work satisfactorily with polyesters; in most situations, however, the assembly will not retain enough toughness for the application.

General guidelines for successful shear-joint design include (1) interference of between 0.20 to 0.30 mm (0.008 to 0.012 in.) between the mating parts; (2) weld depths of 11Ž4 times the nominal wall thickness for maximum joint strength; and (3) a minimum radius of 0.76 mm (0.030 in.) to minimize stress risers that may crack via flex-fatigue during welding.

TOOL-DESIGN PRINCIPLES

For any molding process, proper tool design is an essential part of a quality operation. A well-designed, well-built tool made from durable materials and incorporating good cooling and venting will last longer and require fewer repairs than a tool of lesser quality. It will also increase the quality of the finished parts, decrease scrap, and shorten cycle time.

Mold Cooling. Good cooling is absolutely critical in molds that are designed to run polyester resins. Such resins are likely to stick to hot (>49°C (120°F)) surfaces in the mold. Good cooling design and practices will reduce cycle times, prevent sticking, and aid in part ejection.

Figure 2 shows a suggested layout of drilled cooling lines in the mold. The cooling line spacing should be 21Ž2 to 3 times the diameter between lines, and 11Ž2 to 2 times the diameter away from the surface of the part. Uniform placement of cooling lines, as illustrated in the figure, will help ensure that the part is cooled equally and adequately.

Figure 2. Suggested layout of drilled cooling lines in a mold.

Proper cooling is especially important in mold cores. The processing window and part performance can be greatly enhanced by following good core-cooling principles. Although it may be initially more expensive to place proper cooling in the cores of a tool, it pays off in the long run every time a part is made. There are many methods of achieving proper core cooling: baffles, bubblers, high-conductive alloys, and circular cooling channels around cavity and core inserts. The specific cooling method is not important as long as it is capable of providing good, uniform temperatures throughout the core geometry.

Baffle Configuration. Figure 3, which shows a typical water baffle, illustrates some considerations in core cooling. The water flows all the way into the core, ensuring uniform, complete heat removal. It is critical to bring water to the end of the core pin to allow optimum cooling at the innermost section of the core region.

Figure 3. Typical water-baffle configuration.

When cutting a baffle coolant drop, designers should make it larger in diameter than the feeder tube in order to prevent a flow obstruction from occurring. The cross-sectional area of each side of the drop channel should equal the area of the feeder tube. In a typical baffle tube assembly, a water channel is drilled into the area to be cooled. An intersecting water channel provides water flow that is diverted up one side of the baffle and down the other.

Sprue Design. Because polyester-based resins tend to stick to hot mold steel (>49°C (120°F)), some specific design guidelines are suggested for sprues. In many cases, a thick sprue is the hottest and most difficult area of the tool to cool.

Many molders are successfully using the type of high-conductivity sprue bushing shown in Figure 4. Made from a high-conductivity copper alloy, the bushing contains a hardened 420-stainless-steel nozzle seat to insulate it from nozzle heat and to provide wear resistance. This construction is effective in reducing sprue sticking, increasing sprue rigidity, and cutting cycle time. With this sprue bushing, a standard sprue taper of 4.2 cm/m (0.5 in./ft) has been found to be acceptable for good heat transfer. Installation of these sprue bushings in new molds--or when modifying existing molds to process polyesters--is strongly suggested.

Figure 4. Cross section of popular high-conductivity sprue bushing.

A maximum sprue length of 82.5 mm (3.25 in.) is suggested. To aid ejection, the sprue should be polished in the draw direction. A generous radius should be included at the junction of the sprue and runner system to avoid breakage during ejection. An ejector pin, rather than an air poppet valve, should be placed under the sprue puller, since an air poppet could cause a hot spot and impede cooling.

Upper and lower cooling-line circuits are suggested around the sprue to aid in cooling (see Figure 5). The sprue bushing should be assembled with a slight 0.005-mm (0.2 mil) interference fit to ensure good heat transfer from the bushing into the mold plate.

Figure 5. Sprue design featuring upper and lower cooling-line circuits and slight interference fit for cooling/heat transfer.

Runner Design. Runner systems should be flow-optimized. They should be large enough to deliver the resin to the gate with a low pressure drop and minimal shearing, but small enough to avoid excessive regrind. The most common errors in runner designs are oversizing and inclusion of sharp corners.

Common runner-design guidelines for other engineering polymers also apply to polyesters. A cold-runner system should be designed for smooth, fully balanced material flow. Generously radiused transitions are suggested to reduce resin hang-up and shearing. Cold slug wells are useful in trapping frozen material at the flow front, and should be sized 11Ž2 times larger than the diameters of the runners they are attached to. Runners should always be vented generously.

Regarding runner geometry, trapezoidal and rectangular runner systems are not optimum, since most of the material flow takes place in the circular cross sections indicated by dark shading in Figure 6, and the rest of the runner configuration is not used efficiently. Round runners are best, because they deliver the melt to the cavity with the least amount of dead space. However, they require machining both halves of the mold across the parting line. Typically, a compromise is reached with the half-round approach. A draft angle of 5° on the flat sides of the runner is suggested to ensure good ejection. The bottom of the runner should be fully radiused.

Figure 6. Runner design options. Flow efficiency increases as the cross section approaches a circular shape.

Gate Size and Location. When possible, designers should gate into the thickest section of the part. Several problems can occur if a part is gated in a thin section. These problems include high material shear, which can cause degradation; increased injection pressures; and difficulty in packing out the thicker sections.

For small medical parts, such as luers or needle hubs, gates should be from 0.762 to 1.27 mm (0.030 to 0.050 in.) in diameter. Larger gates may be required for bigger parts. For polyester resins, tunnel gates are commonly used.

If polyesters are to be molded in tools designed for other resins, it may be advantageous to change the gate size to account for differences in viscosity. In general, polyester-based resins may require larger gate sizes than some other resins with lower viscosities. Typically, gate diameters for efficient processing should be 1Ž2 to 2Ž3 times the wall thickness of the part.

HOT-RUNNER SYSTEMS

Hot-runner systems are becoming more common in applications that require the use of polyester materials. When designed properly, these systems can eliminate sprue and runner regrind, mold with lower pressures, and reduce cycle times.

Hot-runner systems should be designed up-front using reputable vendors who have experience with polyester resins. Good hot-runner systems will not have holdup spots in the manifold or gate areas. They will also be designed to avoid sharp corners, extremely small gates, and other high-shear areas. In general, polyesters are more sensitive to shear and thermal conditions than many other resins, and the hot-runner system should be selected with this difference in mind.

Excellent thermal control and good cooling at the gate location are critical for molding polyesters. The mold should be designed so that heat is quickly removed from the gate, since, if the gate does not cool properly, drooling, sticking, or stringing may occur. Steel that is heated as part of the hot drop should not directly contact the part, but should be insulated from the cooled portion of the mold.

For hot-drop gate cooling, separate cooling loops with individual flow and temperature controls are advisable. The additional control is very useful in debugging and optimizing gate appearance and performance. If possible, a water-jacketed insert should be used to remove heat from the gate area.

Hot Drops. Hot "probe" systems, like the one shown on the left of Figure 7, are very common. These sometimes work quite well for processing polyesters, and sometimes don't. Though results with this type of equipment are difficult to predict, generally the more crystallizable types of polyesters do not function well in these systems.

Figure 7. Varieties of hot-drop runner systems: a "probe" system (top), a system in which the melt is completely enclosed in a heated tube (center), and a valve-gate system (bottom).

Polyesters have better molding success using a drop that has the melt completely enclosed in a heated tube, as illustrated in the center image of Figure 7. In this design, the drop is insulated from the gate opening and mold. With such a system, the plastic in the hot drop is 100% melted, resulting in lower pressures and reduced degradation or crystallinity. The gate area still requires excellent cooling.

If at all possible, a valve-gate system should be used. This setup has several advantages: the melt channel is externally heated, and the mechanical valve gate ensures good gate appearance, even when a large gate diameter is used. In non-valve-gated systems, the gate size is often kept very small to reduce gate vestige, which can mean higher material shear through the gate and increased pressure to fill the part. With valve-gated systems, these problems can be avoided.

CONCLUSION

When creating medical devices, designers should maintain a relatively uniform wall thickness throughout the part to ensure quality filling and part performance. A radius should be applied to all sharp corners of the part wherever possible to reduce the likelihood of premature failure due to stress concentration. A minimum draft angle of 1° per side is suggested to help slide the part off the mold during ejection.

Additional consideration should be given to part design when ultrasonic assembly is required. Shear-joint designs are preferred over energy directors when part fabrication requires the welding of polyester resins. These joints provide stronger welds, reduce crack propagation, and facilitate a more evenly distributed load during end use.

Quality mold cooling is of utmost importance in the design of tools for molding polyester resins. Maintaining a mold surface temperature of 38° to 49°C (100° to 120°F) is necessary to prevent material from sticking to the hot mold surface and causing ejection problems. Adequate use of cooling channels, baffles, bubblers, or high-conductivity metals throughout the mold is suggested.

The gate of the part should be located in its thickest section whenever possible. Because of their higher viscosity, polyesters may require larger gate sizes if they are molded in tools designed for other resins. If the mold design includes a hot-runner system, drops that completely enclose the melt in a heated tube have been particularly successful with polyesters, with valve-gated systems performing the best.

By following these general guidelines, design engineers can be successful in achieving proper part and tool design for injection-molded polyester medical devices.

BIBLIOGRAPHY

Dowler B, "Thermoplastic Polyesters" in "Guide to Medical Plastics," Med Dev Diag Indust, 16(4):54­56, 1994.

Dowler B, "Tool Surface Enhancements: The Extra Edge in Injection Molding?", Inj Mold, supplement, November 1993.

Eastman Polymers Design Guide for the Medical Industry, PPM-104A, Kingsport, TN, Eastman Chemical Co., 1995.

Medical publications on Eastman Chemical Co.'s Internet Web site (http://www.eastman.com/ppbo/medical/online/contents.shtml).

Processing Guide for the Medical Industry, PPM-4, Kingsport, TN, Eastman Chemical Co., 1993.

Proper Tool Design for Eastar and Eastalloy Amorphous Polymers, PP-7A, Kingsport, TN, Eastman Chemical Co., 1995.

Vance M, and Dowler B, "Using Thermoplastic Polyesters in Medical Devices," Med Plast Biomat, 2(2):20­32, 1995.

Melanie L. Jones is a technical service representative at Eastman Chemical Co. (Kingsport, TN). Her principal service areas deal with part and tool design for injection-molded medical applications, medical chemical-resistance testing, and secondary operations for amorphous copolyesters.

Copyright ©1997 Medical Plastics and Biomaterials

Return to the MPB article index