If you have ever been tasked with designing a plastic part, you undoubtedly have hit some snags on the way to getting the part into production. In school, you learn that injection molding allows for almost limitless creativity (and it’s true that injection molding does allow for a remarkable amount of design flexibility, while also being cost effective). However, in the real world, it can seem like getting a part into production requires a never ending cycle of changes to allow for injection molding process. Use these five tips to get your part into plastic faster!
Watch Out For Wall Thickness
Not unlike the 3 rules of real estate (location, location, location), If there were three rules of plastic part design, it would be, “wall thickness, wall thickness, wall thickness.” It is hard to over emphasize the importance of proper wall thickness. Wall thickness issues can be divided into two basic categories, nominal wall thickness and unequal wall thickness. Choosing the correct nominal wall thickness is critical to getting good parts. If your wall thickness is too thick, you will be wasting material, press time, and likely will have cosmetic and structural issues. If your part is too thin, you may need to use a larger, more expensive press, risk tool damage, and have cosmetic and structural issues.
What Thickness Is The Correct Thickness?
Unfortunately, there is not a ‘one size fits all’ answer, however there are a few guidelines: First, determine the minimum wall thickness that will meet your design requirements, then check with the material supplier to see if they have any specific thickness guidelines for the specific material you are interested in. If there is no information available, or if you have not selected a specific material, you should be in the ballpark, with a wall thickness from .04 to .150* with most plastic materials.
*The primary process-related factors that will make the wall thickness thinner or thicker are material type (easier flowing plastics can allow for thinner walls), and flow length (the distance the material needs to flow from the nozzle to the furthest corner of the part.) Longer flow lengths may require thicker walls.
What To Do If You Have Unequal Wall Thickness
If there is no way to eliminate the unequal wall thickness, the basic guideline is to make as gradual of a transition from thick to thin as possible. Typically, a transition length of at least 3 X the change in wall thickness will reduce the appearance of cosmetic issues, but a more gradual transition is always better. It is also important to look out for less obvious thick sections. One way to help determine if you have a thick section, is to imagine trying to fit a circle or sphere into the cross section of the part. If you are able to fit a circle that is more than 10% larger than your nominal wall thickness, you are likely looking at a thick section that should be addressed. Below are a few common examples, with their associated fixes. Rib to wall ratios should be between 40% and 60%. However, adding fillets to the base of the rib must also be taken into consideration. The image above the first two ribs are both 60% of the wall thickness, however the second rib also has a generous fillet, resulting in a thicker area than if the rib to wall ratio had been 1 to 1. When an outside radius is not matched to the inside radius (shown on left) the result can be a thick section at the corner of the part. Add the wall thickness to the inside radius to get an outside radius that will maintain the wall thickness. When a boss is too close to a side wall, the result will be thick sections where the boss merges with the side wall (shown on left). One solution, is to move the boss away from the side wall, and then attach with an appropriately sized rib for strength.
Undercuts, are regions of a part that if not corrected will prevent the mold from opening. Often these are created by holes or snap features. While many of these features can be created using various tool actions (secondary tool movements), they will greatly contribute to the tool complexity and cost. One way to avoid an undercut, is to put a hole in from the opposite side of the part to allow the undercut to be formed without adding an action. The highlighted snap surfaces are not able to be pulled out of the mold (image left). Adding a through hole allows the opposite side of the mold to create the underside surfaces of the snap.
Add Draft, Or At Least Plan For It
Draft must be added to the walls of all injection molded parts. Without draft, parts will stick in the mold. While there a many factors that affect how much draft is needed, 1 degree is a good starting point. However, more draft is always better. And don’t forget to draft your internal features (like ribs and bosses).
Part without draft (left) and part with draft (right).
While the need for draft is relatively simple to understand, one area that is often overlooked (until it is too late) is mismatch of mating parts, caused by draft. Often, it is relatively easy to account for draft in the beginning of a design, but part mismatch can cause a major issue if left to the end of a design.
Mating edge (blue) is mismatched due to draft not being taken into account.
Plan For Gating
The runner and gating system is most often designed by the molder or toolmaker, however this does not mean that the need for gating can be ignored by the part designer. Understanding where gates should be placed, and allowing for the resulting blemish (typically an area under .1” by .1”) is important. Ideally gates would be placed at the geometric center of the part. This will allow for the shortest overall flow length (distance the plastic must flow from the gate to the outer most point of the part). If more than one gate is needed, the gates should be placed to both reduce the flow length, and must take into account the knit line created by plastic from each gate meeting. Ideally a part designer will account for the blemish caused by the gate and knit lines by designing the part in such a way that any blemish is on a non-cosmetic surface.
The proposed gate location (blue) is located on a surface that will be covered by a label.
Plastic Parts “Move”, Expect It & Plan For It
Plastic allows for nearly infinite shape possibilities, but plastic injection molded parts cannot be expected to maintain the same tolerance as a machined piece of metal. This is especially important to remember when prototypes are created using machining, or existing designs are moved to plastic from metal. A good rule of thumb for a typical plastic part tolerance is +- .005” for the first inch of length, then add an addition .001 per inch up to 6 inches and add .003 after that. For example a 12.5” linear dimension would have a tolerance of +-.028. (There are many considerations when determining the correct tolerancing on a specific dimension, and this is intended only as a general guide) In addition to basic tolerancing, it is also important to understand that plastic parts will warp and bow. However, unlike metal parts, plastic parts can more easily be forced into place. For this reason, it is often a good idea to create a shiplap or “style” grove around all mating parts (as opposed to a flat butt joint), because any mismatch between the parts will be hidden from the eye.
Groove added to reduce appearance of mismatch due to warping, tolerance, and draft.
While these are just basic guidelines, they should greatly reduce the amount of back and forth required to get your parts into production. Sometimes, there are places in a design that these guidelines must be broken, or situations that are beyond the scope of basic rules. In these cases, mold filling simulation can provide quick feedback about what issues still need to be addressed, long before the design is sent out for molding.