Design rules for plastic injection

Design rules for plastic injection molding.

Plastic injection molding allows us to form relatively complex shapes. As a result, a well designed plastic part serves multiple functions.

Once the injection mold is produced, these parts can be reproduced at a very low cost. However,  changes to the mold design at later stages of development can be very expensive. Therefore, achieving the best results on the first time is essential. It is important as a product designer to follow the design guidelines in order to avoid the most common defects in injection molding.

Use a constant wall thickness.

It is important to use a constant wall thickness to avoid sections that are thicker than other areas in the part. This is essential as walls with a section too thick lead to warping of the part as the molten plastic cools down.

When there is no other option than to design sections of different thickness, make the transition as smooth as possible using a chamfer or round. In this way the material will flow more fluently inside the cavity. This ensures that the whole mold will be fully filled.

constant wall thickness plastic product design
plastic design smooth transitions

Using a wall thickness between 1.2 mm and 3 mm is correct for most materials. Below you find an overview of recommended wall thicknesses of commonly used injection molding materials:

MaterialRecommended wall thickness [mm]Recommended wall thickness [inches]
Polypropylene (PP)0.8 – 3.8 mm0.03” – 0.15”
ABS1.2 – 3.5 mm0.045” – 0.14”
Polyethylene (PE)0.8 – 3.0 mm0.03” – 0.12”
Polystyrene (PS)1.0 – 4.0 mm0.04” – 0.155”
Polyurethane (PUR)2.0 – 20.0 mm0.08” – 0.785”
Nylon (PA 6)0.8 – 3.0 mm0.03” – 0.12”
Polycarbonate (PC)1.0 – 4.0 mm0.04” – 0.16”
PC/ABS1.2 – 3.5 mm0.045” – 0.14”
POM (Delrin)0.8 – 3.0 mm0.03” – 0.12”
PEEK1.0 – 3.0 mm0.04” – 0.12”
Silicone1.0 – 10.0 mm0.04” – 0.40”

For best results:

Use a uniform wall thickness within the recommended values

When different thickness are required, smoothen the transition using a chamfer or fillet with length that is 3x the difference in thickness

Hollow out thick sections.

Among the design rules for plastic injection it is important to hollow out thick sections. Thick sections have a negative effect on the final result. More specific the lead to different defects, including warping and sinking. It is essential to limit the maximum thickness of any section of your design to the recommended values by hollowing out the wall or feature.

Design structures with ribs of equal strength and stiffness but reduced wall thickness. This in order to improve the strength of hollow areas. A correctly designed part is shown below:

plastic design hollow out

Use ribs to improve the stiffness of horizontal areas without increasing their thickness. Remember though, that the wall thickness limitations still apply. Designing thicker rids than the recommended rib thickness can result in sink marks.

plastic design ribs and walls

For best results:

Hollow out thick sections and use ribs to improve the strength and stiffness of the part

Design ribs with max. thickness equal to 0.5x the wall thickness

Design ribs with max. height equal to 3x the wall thickness

Add smooth transitions.

Recommended: 3 × wall thickness difference

Sometimes sections with different wall thicknesses cannot be avoided. When this is the case, use chamfers or fillets to make the transition as smooth as possible.
Similarly, the base of vertical features (like ribs, bosses, snap-fits) must also always be rounded.

smooth transitions plastic product design

Round all edges.

The uniform wall thickness limitation also applies to edges and corners: the transition must be as smooth as possible to ensure good material flow.
For interior edges, use a radius of at least 0.5 x the wall thickness. For exterior edges, add a radius equal to the interior radius plus the wall thickness. This way you ensure that the thickness of the walls is constant everywhere (even at the corners).
Adding to this, sharp corners result in stress concentrations which can result in weaker parts.

rounded corners plastic product design
plastic design rounded corners

For best results:

Add a fillet equal to 0.5x the wall thickness to internal corners

Add a fillet equal to 1.5x the wall thickness to external corners

Add draft angles.

Among all the design rules for plastic injection, draft angles is one of the most important. In order to make the ejection of the part from the mold easier,  draft angles must be added to all vertical walls. Walls without a draft angle will have drag marks on their surface, because of to the high friction with the mold during ejection.

A minimum draft angle of 2° is recommended. However, smaller angles are better than nothing in some cases. The taller the feature, the larger the draft angles should be. Use draft angles up to 50° if necessary.

draft angles plastic product design

A good rule of thumb is to increase the draft angle by one degree for every 25 mm. For example, add a draft angle of 3o degrees to a feature that is 75 mm tall. Larger draft angle should be used if the part has a textured surface finish. As a rule of thumb, add 1o to 2o extra degrees to the results of the above calculations.

Remember that draft angles are also necessary for ribs. Be aware though that adding an angle will reduce the thickness of the top of the rib, so make sure that your design complies with the recommended minimum wall thickness.

plastic design draft angles

For best results:

Add a minimum draft angle of 2o degrees to all vertical walls

For features taller than 50 mm, increase the draft angle by one degree every 25 mm

For parts with textured surface finish, increase the draft angle by 1-2o extra degrees

How to handle undercuts.

Undercuts are features to consider well when designing plastic products. The simplest mold consists of two halves. Features with undercuts (such as  external thread or the hook of snap-fit joints) may not be manufacturable with a standard mold though. This is either because the mold cannot be CNC machined or because the material is in the way of ejecting the part.

Undercuts in injection molding are features that cannot be manufactured with a simple two-part mold, because steel material is in the way while the mold opens or during ejection.

The teeth of a thread or the hook of a snap-fit joint are examples of undercuts.

Here some ideas to help you deal with undercuts:

Avoid undercuts using shutoffs.

Avoiding undercuts altogether might be the best option. Undercuts always add cost, complexity, and maintenance requirements to the mold. A clever redesign can often eliminate undercuts.

Shut-offs are a useful trick to deal with undercuts on internal regions of the part (for snap-fits) or on the sides of the part (for holes or handles).

undercuts plastic product design

Below are some examples of how you can redesign injection molded parts in order to avoid undercuts: essentially, material is removed in the area under the undercut.

plastic design undercuts solutions
plastic design undercuts solutions snap fits

Slides and cores.

We use slides when it is not possible to redesign the injection molded part to avoid undercuts.

Slide cores are inserts that slide in as the mold closes and slide out before it opens. Keep in mind that these mechanisms add cost and complexity to the mold.

Follow these guidelines when designing a side actions:

– There needs to be space for the core to move in and out. This means that the feature must be on the other side of the part.

– The side-actions must move perpendicularly. Moving at an angle other than 90° is more complicated, increasing cost and lead times.

– Don’t forget to add draft angles to your design as usual, taking in consideration the movement of the slide.

plastic injection product design undercuts with slide

Bosses or studs.

Bosses and studs are very common in injection molded parts. Moreover, they are used as points for attachment or assembly. They consist of cylindrical projections with holes designed to receive screws, threaded inserts, or other types of fastening and assembly hardware. A good way to think of a boss is as a rib that closes on itself in a circle.

Studs are used as points of attachment or fastening with the use of self-tapping screws or threaded inserts.

bosses and studs for screws plastic product design
plastic design bosses or studs

When studs are used as points of fastening, the outer diameter of the boss should be 2x the nominal diameter of the screw or insert and its inner diameter equal to the diameter of the core of the screw. The hole of the boss should extend to the base-wall level, even if the full depth is not needed for assembly, to maintain a uniform wall thickness throughout the feature. Add a chamfer for easy insertion of the screw or insert.

For best results:

Avoid designing bosses that merge into main walls

Support bosses with ribs or connect them to a main wall

For bosses with inserts, use an outer diameter equal to 2× the insert’s nominal size

Designing ribs.

When even the maximum recommended wall thickness is not enough to meet the functional requirements of a part, ribs can be used to improve its stiffness.

When designing ribs:

  • Use a thickness of 0.5 × main wall thickness
  • The height should be smaller than 3 × rib thickness
  • Use a fillet with radius greater then ¼ × rib thickness
  • Add a draft angles of at least 0.25° – 0.5°
  • Add a minimum distance between ribs and walls of 4 × rib thickness
designing ribs plastic product

plastic design snap fits


Snap-fit joints are a very simple, economical and rapid way of joining two parts without fasteners or tools. A wide range of design possibilities exists for snap-fit joints.

As a rule of thumb, the deflection of a snap-fit joint mainly depends on its length and the permissible force that can be applied on it on its width (since its thickness is more or less defined by the wall thickness of the part). Also, snap-fit joints are another example of undercuts.

In the example above, the most common snap-fit joint design (known as the cantilever snap-fit joint) is shown. As with ribs, add a draft angle to your snap-fit joints and use a minimum thickness of 0.5x the wall thickness.

For best results:

Add a draft angle to the vertical walls of your snap-fit joints

Design snap-fits with thickness greater than 0.5x the wall thickness

Adjust their width and length to control their deflection and permissible force

Text and symbols.

Text is a very common feature that can be useful for logos, labels, warnings, diagrams and instructions, saving the expense of stick-on or painted labels. Design rules for plastic injection also include text and symbols embossing.

When adding text, choose embossed text over engraved text, as it’s easier to CNC machine on the mold and thus more economical.

Also raising the text 0.5 mm above the part surface will ensure that the letters are easy to read. We recommend selecting a bold, rounded font style with uniform line thickness, with a size of 20 points or larger. Some font examples include: Century Gothic Bold, Arial and Verdana.

plastic design text and symbols

For best results:

Use embossed text (0.5 mm height) instead of engraved texted

Use a font with uniform thickness and a minimum font size of 20 points

Align the text perpendicular to the parting line

Use a height (or depth) greater than 0.5 mm