Complexity vs. Manufacturability

Materials Supplement - Supplement

Plastic Product Design Principles that Eliminate Uncertainty, Ensure Manufacturability

March 7, 2013

The rapid development of modern 3D CAD systems has facilitated the evolution of product design, and as a result, a move to more organic forms and ever-increasing geometry complexity. Just think about the change in design from the conventional box shaped vacuum cleaner to the modern Dyson. The aim of this column is to focus on design fundamentals and the impact they have on the manufacturing and production processes.


Consistent Wall Thickness

Design engineers need to try to maintain a consistent wall thickness throughout the entire model. Any major change in part thickness can cause major molding issues such internal voids, surface sink marks, unpredictable shrink rates, and ultimately, longer cycle times. If a wall thickness change is necessary, it should be a smooth transition to ensure ease of material flow preventing critical stress points, which may cause part failure during product testing and result in an updated part design or additional tooling costs. Detecting manufacturability issues at the design stage will prevent costly reworking and save valuable time during later production stages.
 



Rib Design

When creating rib patterns, it is important to remember that ribs are only there to increase part rigidity and aesthetic reasons should not compromise them. Design engineers typically follow standard guidelines for rib design. If possible, engineers should avoid a combination of thin and thick ribs. Some of the most common design guidelines are:

  • Rib thickness should be 60% to 80% of the nominal wall thickness.
  • Maximum rib height should not exceed 3x the nominal wall thick- ness; to increase product rigidity, it is better to increase the number of ribs rather than the rib height.
  • Minimum spacing between ribs should be 2x the nominal wall thickness.
  • Fillet radii applied to ribs should be no greater than 50% of the rib thickness.
  • Extra thick ribs should be cored out.
  • Cross ribbed patterns are preferred (if the design allows), as they offer reater loading permutations and ensure uniform stress distribution.


Bosses

Bosses are a fundamental component in plastic part design as they offer strengthening properties and provide alignment during assembly. Similar to rib design, it is important to consider the wall thickness when designing bosses. The design guidelines listed below will help avoid surface imperfections such as internal voids, surface sink marks, and unpredictable shrink rates.

  • The boss thickness should be 60% of the nominal wall thickness; if the part thickness is greater than 4mm, reduction of the boss thick- ness can be to 40% of the nominal wall thickness.
  • The boss height should not exceed 2.5x the diameter of the hole in the boss.
  • Corner bosses integral to side walls will result in excess material accu- mulation.
  • Tall ribs on a boss help material flow and venting, reducing the chances of air traps.
  • Gussets distribute the load applied during screw/insert insertion) to a wider area, reducing failure at the boss/wall junction.

The fillet radii should be applied at the base of a rib or boss to allow better stress distribution. High stress concentrations peaks occur if no fillets are applied, often leading to cracking and part failure. Please note, however, that if the fillet radii applied is too large, excess material accumulation can occur, which may lead to voids or sink marks during the molding cycle. This same principle is also true where a rib or boss meets the edge of the component.

Fortunately, CAD systems are beginning to introduce analysis tools to calculate and display the thickness of a CAD model and help identify potential problem zones. Typically, two methods are available – the first is based on the largest sphere that can be placed within the model without intersecting any other face; the second is the more traditional shooting ray method, which shoots a ray through the model along the surface normal until it hits a second face.


Draft Angle

Well understood but often ignored during the design stage is the need to add a draft angle to a model. While this may seem like a trivial task, if the addition of the taper is not at the right point within the history tree (if applicable), or if there is the subsequent addition of complex fillets, this task becomes a great deal more complex.

Draft angle is an important feature that allows extraction of a molded part from a mold cavity without issue. The high pressures of injection molding and material contraction means that it is often difficult to remove the part. While it is possible to mold parts with zero draft (or even negative draft) using side cores, lifters, or two-stage ejection, these features dramatically influence the complexity and cost of the tool.

Although no exact formula exists for defining the correct draft angle for a certain part, many factors have an impact on the optimum value. Generally, thin-walled parts that undergo high-pressure injection molding need more draft as the material is forced in, which results in a tighter grip on the cavity. Equally, parts subjected to lower-pressure molding can have less draft.

For smooth surfaces, the general recommendation is for a minimum of 0.5° draft per side, although experience has shown that a draft angle of 1° per side provides easy ejection for most surfaces. Textured surfaces are slightly different as the non-uniform texture will drag and scuff, ruining the required effect if the draft angle is not sufficient. As a general guideline, designers need to allow for a minimum of 1.5° per 0.025mm depth of texture in addition to the normal draft amount.

It is important to consider the depth of the draw. As the draft’s distance becomes greater, ejection becomes easier and the geometry also becomes thicker. As we have already learned, those types of dramatic changes in model thickness may cause internal voids, surface sink marks, and unpredictable warpage. As an example, a draft angle of 1° over a drop of 100mm would increase part thickness by 1.75mm per side.

Although at the product design stage, the molding polymer may not be known, this can have an effect of the required draft angle. For example, materials with fillers (glass-filled) tend to have a reduced shrinkage value and, therefore, will not move away from the cavity wall. In this case, greater draft angles are required.

Holes are easy to produce in molded parts with typical creation using core pins. However, blind holes with zero draft often create a vacuum effect at the top of the core pin during ejection (more prone to parts with a polished finish). In this case, a small draft angle will break the seal and improve ejection. Ultimately, the easier it is to remove the part from the mold the fewer the number of ejector pins required.


Part Radii, Part Text

A significant number of plastic parts fail due to sharp corners or insufficient radius. Sharp corners create localized stress concentrations, which will promote crack initiation and cause premature part failure. The addition of fillet radii to all sharp corners will not only reduce stresses, but also improve plastic flow. As a general rule, at corners, the inside radius is 0.5x material thickness and the outside radius should be 1x material thickness plus the part thickness – a larger radius should be used if the part design allows it.

Text should be embossed up on the model, as this is a cavity on the mold, and therefore, easier to machine and easier to polish. For ease of cutting and visibility, bold San Serif fonts are preferred.



Undercuts, Design, Gate Position

Most undercuts cannot strip from the mold, therefore requiring additional mechanisms in the mold to move certain components prior to ejection. This is typically performed using slides, cams, lifters, or collapsible cores – all adding costs to the mold design. Clever part design or minor design concessions often can eliminate complex mechanisms for undercuts.

It is often preferred to gate onto the thickest section of the component to reduce the possibility of sinking due to insufficient material packing. Fixing the gate location ultimately determines the filling behavior, weld lines, shrinkage, warpage, and surface quality of the molded part. Weld lines are lines where two plastic flow fronts meet and form a relatively weak bond. These are the areas most likely to fail when the part is under stress. Complex moldings will always contain weld lines and if they cannot be reduced then they should be moved to non-critical areas of the component. To achieve this, the gate location is typically moved, or if the design allows, flow leaders or flow restrictors are added to change the part wall thickness.

Flow Leader – Thickened sections (no more than 25% of nominal part thickness) to help drive the plastic flow front. It is typically used for filling or packing issues in areas furthest away from gate location or used to balance the filling of non-symmetrical parts.

Flow Restrictor – Small areas of reduced thickness (no more than 33% of nominal part thickness) that help control the plastic flow front; typically used to control the filling pattern and manage weld lines and air trap locations.


Conclusion

We have briefly studied eight plastic product design principles. While each of the points are generic and are not applicable to every scenario, they are certainly a solid base from where to start your next design. Therefore, next time you shell out a model or drop in some strengthening ribs, do not forget to consider the impact these decisions have on the production cycle. In the engineering world, for a project to be successful, it is a continual compromise between product design and production feasibility.
 

 


Vero USA Inc.

Wixom, MI
www.verosoftware.com