Sponsored By

In this bimonthly column, Glenn Beall of Glenn Beall Plastics Ltd. (Libertyville, IL) shares his special perspective on issues important to design engineers and the molding industry.

Glenn Beall

February 1, 2000

9 Min Read
By Design, Part design 107: Draft angles

In this bimonthly column, Glenn Beall of Glenn Beall Plastics Ltd. (Libertyville, IL) shares his special perspective on issues important to design engineers and the molding industry.

The previous two articles in this series traced the transition from 2-D to 3-D injection molded parts. Continuing in that vein, this article reviews the important subject of draft angles, or molding tapers. Molding draft angles can be defined as tapers on those surfaces of a molded part that slide across a mold's cores and cavities as the part is being demolded.

Draft angles create a conflict of interest. Molders like draft angles-the larger, the better. Moldmakers dislike having to machine these angles on all surfaces of the cores and cavities. To the product designer, draft angles are an annoyance. They complicate the designing of a part while providing no functional benefit to the ultimate customer. They also make all injection molded parts look like pyramids that will not stack straight or line up with each other.

Still, there are many good reasons for incorporating draft angles into the design of an injection molded part. But designers can ignore all of these exhortations for more draft as long as they remember that draft angles reduce part cost.

All through the 1990s, the manufacturers of durable products put a priority on reducing the costs of the products they market. Draft angles are one of the tricks of the trade that designers can use to reduce the cost of injection molded parts.

Mold Shrinkage and Draft Angles
The justification for draft angles comes from the nature of the injection molding process and the ever present nemesis of mold shrinkage. Injection molding is a high-pressure process. These high pressures force the plastic into intimate contact with all surfaces of a mold's cores and cavities. This high-pressure packing of the cavities makes it difficult to demold a part.

In some cases, shrinkage of the plastic material will pull the part away from the cavity, making the demolding easier. In other instances, shrinkage causes the plastic material to tightly grip the cores that form the inside surfaces of a molded part.

The round disk and the rectangular plate shown in Figure 1 have no depressions or projections. These are basically 2-D parts. Simple parts of this type are molded in cavities that do not contain core pins. During the cooling portion of the molding cycle, these parts are free to shrink away from their cavities. The force required to eject 2-D parts is minimal.

The rectangular plate in Figure 1 could be rolled up to create a tube. A cylinder, closed on one end, could be produced by placing the round disk on one end of the tube. The two 2-D parts would have then combined to create a 3-D part, which would be produced in a mold containing both a cavity and a core.

The two parts shown in cross section in Figure 2 are basically cylinders closed on one end. From a molding perspective these are two very different parts. The part on the left was designed with straight side walls and sharp corners. This would be an easy part to design. The core and cavity required for molding this part would be low in cost. On the negative side, the sharp corners create molded-in stress, as discussed in the December 1999 installment of this series. The lack of draft angles increases the cost of molding this part.

The radiused corners and the molding draft angles on the part on the right will produce a stronger part on a shorter molding cycle, with less molded-in stress. On the negative side, this part will be more difficult to design and the mold cost will be slightly higher.

Figure 3 depicts these same two parts being ejected from a mold. The nondrafted part on the left has been partially demolded, but it is still in intimate contact with both the cavity and the core pin. The drafted part on the right has been demolded the same amount, but it is no longer in contact with the cavity or the core pin. It is obvious that a higher ejection force will be required to demold the nondrafted part. An increase in ejection force results in a longer molding cycle and a higher part cost.

Reducing Part Cost
During the cooling portion of the injection molding cycle, the plastic material changes from a thick, viscous liquid to a semisolid and finally a completely solid part. The rate of cooling will be dictated by the thickness of the part, the thermal conductivity of the plastic, and the cooling capabilities of the mold.

The degree to which the part must be cooled will be determined by how long it takes the part to regain strength enough to accept the force of ejection and retain its shape. Molding draft angles reduce the force required to demold a part, and these lower ejection forces can result in reduced cycle times.

There is no such thing as an average cooling time. If there was, it would be in the range of 70 to 80 percent of the total cycle time. Molding draft angles reduce the force required to demold a part and that, in turn, minimizes the cooling portion of the molding cycle. In other words, draft angles reduce part costs.

Other Draft-related Problems
Referring to the nondrafted half of Figure 3, a vacuum will be created as the part is pulled out of the cavity. That vacuum can cause the top of the part to be domed upward.

An internal vacuum will also be created as the part is ejected from the straight core pin. This can cause the top of the part to dome inward. Flexing the top of the part can result in a deformed top panel and molded-in stress at the junction of the top and the side walls. The drafted part creates a clearance between the core and cavity and the molded part. This clearance becomes a vent that releases the vacuum.

The combination of sharp corners and no draft angle can also result in drag marks or scratches on the side walls of the part. These scratch marks are created by the nondrafted part rubbing against the sharp corners on the core and cavity. The mold on the right in Figure 3 has no sharp corners, and the draft angle creates a clearance between the part and the core and cavity.

The high ejection forces required for nondrafted 3-D parts can cause an increase in molded-in stress and deformation. This is especially true with ejector pin type molds that do not apply uniformly distributed ejection force to the part.

An Adequate Draft Angle
There is no single draft angle that is adequate for all injection molded parts. Each individual part has its own unique draft requirements. Large parts require more draft than small parts. Thin-walled parts that are molded at high pressures require more draft than parts molded at lower injection pressures.

As the plastic material cools, it shrinks and pulls away from cavities while gripping the core pins. Theoretically, core pins require more draft than cavities. The amount that a plastic material shrinks must be considered in selecting a suitable draft angle.

Large draft angles and a smooth polish are required for parts molded in strong, brittle, abrasive, and sticky materials. Smaller draft angles can be used on soft, ductile, and slippery materials. For example, self-lubricating nylon gears and bearings would be easier to mold with draft angles, but they can be molded with zero draft. Some materials cannot be molded without draft.

The ideal draft angle, from a cost and manufacturability perspective, is the largest angle that will not distract from the consumer's acceptance of the product. The minimum allowable draft angle is more difficult to define. The hands-on experience gained by plastic material suppliers and molders makes them the ultimate experts on the minimal acceptable draft.

In most cases, 1° per side will be adequate, but 2 or 5° per side would be better. If the design cannot tolerate 1°, then specify 1/2° per side. A minimal draft angle, such as 1/4° or even .002 inch/inch/side, is better than no draft angle at all.

Specifying Draft Angles
While designing a part, the engineer may not know the location of the mold's parting line. Without that information, it is impossible to determine whether the part should have plus or minus draft angles. There is also confusion as to how much is required. This lack of knowledge has resulted in the common practice of drawing the part without draft angles and specifying the draft as a drawing note, such as "allowable draft 1°." This technique simplifies the part design process, but it is an undesirable draft angle specification that leads to misinterpretation.

The four different parts shown in Figure 4 could have been made from the same drawing with the note designating an allowable draft of 1°. Part A has a -1°/side draft angle. Another moldmaker might have interpreted that note to be an included angle of 1° or -1/2°/side, as depicted in Part B. Part C has a +1°/side draft on the outside and a -1°/side draft on the inside. This part has a thicker wall that will require more plastic material and a longer molding cycle.

The moldmaker that produced the mold for Part D interpreted the word "allowable" to mean that draft was optional, and parts from his mold have no draft angles at all. The sad part of this story is that all four of these different parts are within the drawing draft angle specification. Molding draft angles are too important to the successful molding of a part to be relegated to a simple drawing note.

With 2-D drawings, each dimension that is to be drafted should have its own draft specification. That specification must indicate the amount of the draft per side, and whether it is plus or minus draft. Parts being designed as 3-D solid models for electronic transfer must have the draft included in the database. If draft is not included, time will be lost, as there cannot be a seamless transfer of the data through the cutter path program and on into CNC machining of the cores and cavities.

Experienced designers are aware of the importance of molding draft angles. Most designers try to specify draft angles on at least the side walls of a part that are perpendicular to the mold's parting line. Many designers will, however, overlook drafting the other details on a part. For example, the part shown in Figure 5 should also have draft angles on the mounting flanges, gusset, and hole. The standing rib, hollow bosses, louvers, and other holes will all benefit from being drafted.

Any draft is better than none. The important cost saving benefits of draft angles will, however, be lost by a half-done job. Failing to provide a draft angle on the long side-acting core pin that forms the hole in the threaded projection in Figure 5 would be a serious mistake. The force required to pull that core pin could be the one thing that requires a longer cooling cycle.

Sign up for the PlasticsToday NewsFeed newsletter.

You May Also Like