|
DFMPro helps designers check for industry standard DFM practices for injection molding
right inside the CAD environment. This helps produce parts economically at a better
quality and shorter lead time. Users can validate the designs to check for uniform
wall thickness, recommended rib parameters, appropriate draft angles on core and
cavity surfaces, undercuts, thin steel conditions on mold and many other common
rules.
|
|
|
|
DFMPro provides flexibility to configure the available injection molding rules.
It also provides the ability to add new design rules requiring very basic programming
knowledge.
|
|
Design Guidelines for Injection Molding
|
|
Given below are certain standard guidelines which can be referred to while designing
parts for injection molding. But it is important to note that the guidelines are
general. Depending on particular requirements of a part, it may not always be possible
to follow all the guidelines.
|
|
Guidelines for Ribs
|
|
Rib features help in strengthening the molded part without adding to wall thickness.
In some cases, they can also act as decorative features. Ribs also provide alignment
in mating parts or provide stopping surfaces for assemblies.
|
|
- The fillet at the root of the rib should have a radius which is 0.25 to 0.50 times
the nominal wall thickness. Such a fillet helps in reducing the stress concentration
in the region where the rib joins the main wall. A smaller fillet will not prove
useful whereas a larger fillet will increase the thickness in that region possibly
causing sink marks.
- The base of the rib should have a width approximately 0.5 to 0.6 times the adjacent
nominal wall thickness. A thinner rib will need a greater height causing problems
during filling, ejection and also may buckle under load. Very thin parts (<=
1mm) should have ribs equal to part thickness. Thick ribs can affect fill pattern
of the mold and cause sink marks. For thicker ribs, core out the rib from the back
to maintain uniform wall thickness.
- Ribs should ideally not have a height over 3 times the nominal wall thickness to
avoid stress, venting, filling and ejection problems. It is better to have more
ribs in preference to taller ribs. Ribs which have excessive height or width will
need strengthening by using reinforcing ribs or gussets
- Ribs must ideally be placed in the drawing direction and
have drafts of around 0.5 to 1 degree per side for ease of ejection. Excessive
drafts can cause filling problems in tall ribs and also cause excessive thickness
reduction. They are also most advantageous if placed along the length of the region
under bending.
|
|
- Parallel ribs must not be too close together since the gap between the ribs is produced
by an upstanding core in the mould. If this core becomes too thin, then it becomes
very difficult to cool. Usually, this gap should be at least two times the nominal
wall thickness.
|
|
Guidelines for Drafts
|
|
Draft angle design is an important factor in designing with certain materials more
than others. The mold finish, resin, part geometry, and mold ejection system determine
the amount of draft needed. With materials having higher shrinkage, parts tend to
shrink onto the core leading to higher contact pressure and friction.
|
|
|
- Appropriate draft angles applied on inside and outside surfaces of part in the direction
of draw will help ejection of part from mold thus reducing cycle time and improving
productivity. Draft angle of 0.25 to 2 degrees is generally recommended per side.
If the depth of draw is higher, higher draft angles are recommended.
- If the surface is textured, additional draft is necessary to avoid drag marks and
scuffing of part surface. Per 0.01 mm depth of texture, generally additionally 0.4
degree additional draft may be required.
- Ejector pins are generally used to assist ejection. If a part doesn’t have
enough contact area for ejector pins, additional draft may be required on part surfaces
to avoid distortion during ejection.
- Ribs must ideally be placed in the drawing direction and have drafts of around 0.5
to 1 degree per side for ease of ejection. Excessive drafts can cause filling problems
in tall ribs and also cause excessive thickness reduction. They are also most advantageous
if placed along the length of the region under bending
- In case drafts are not permitted, cam or slide action may be needed.
|
|
Guidelines for Bosses
|
Boss, a basic design element in plastics, is typically cylindrical and used as a
mounting fixture, location point, reinforcement feature or spacer. Requirements
for draft angle and comer radiuses with respect to bosses match those for ribs.
The design of a boss may vary depending on its functionality. Bosses are more often
than not buttressed by supporting rib or gussets a little lower in height. Flat
ribs may also connect the boss to side walls thus assisting in improving rigidity
while maintaining uniform wall thickness.
|
|
- Generally, boss diameter at the top should be 2-2.5 times the hole diameter. Thickness
of the boss should be within 0.5 to 0.75 times the nominal wall thickness. The thickness
of the boss may have to be increased depending on the stresses created by inserts
/ screws; accompanied by creation of sink marks.
- A lead-in chamfer may be provided for ease of assembly. For screw-type bosses, counter
bores reduce stress at the open end. For such bosses, the diameters of the boss,
hole and counter bore in addition to the depth of the counter bore depend on the
material. In case the hole is blind, its depth must be sufficient (core pin must
penetrate nominal wall partially) to minimize sink marks. The bottom of the blind
hole (head of core pin) must have a generous radius to avoid stresses.
- Height of the boss is generally restricted to 3 times nominal wall thickness to
reduce cycle times. ( Core pins may take longer to cool for taller bosses)
- A fillet is of around 0.25-0.5 times nominal wall thickness is introduced at the
base of the boss to reduce stresses – higher radii may create sink marks.
Tip of the boss is also rounded to reduce stresses.
- A draft of around 0.5 degrees may be applied on the boss for ease of ejection.
- Heights of ribs and gussets supporting the boss are restricted to 0.9 times the
height of the boss.
|
|
Guidelines for Holes
|
|
Designing a hole in a injection molded part requires stress minimization considerations.
Holes are generally created using core pins.
|
|
- Distance of a hole from the side wall as well from the edge of another hole should
be at least 2T where T is the nominal wall thickness.
- To avoid deflection of core pins due to molding pressures, depth of blind holes
is restricted to 2-4 times diameter. Another option to design through holes wherein
core pins can be supported on both sides. For through holes having higher depth
diameter ratios, cores can become fragile and break due to the operating pressures
and high temperatures. In such cases, higher tapers or steps may be employed.
- Holes parallel to axis of parting lines are easier to create; side action cores
are avoided.
- Drafts are provided on holes for ease of ejection.
- Holes created by core pins lead to knit marks. If nit marks have to be avoided,
alternate designs are needed.
- Edges and corners of holes and other depressions are preferred to have a radius
(preferably 0.5 times wall thickness)
|
|
Guidelines for Corners
|
|
The mold for manufacturing the part is generally machined from steel. Creating a
radius in the mold is easier than creating a sharp corner. Hence the part must generally
have rounded corners where needed to facilitate radius on the mold.
|
|
|
- Sharp corners may also have to be replaced with appropriate to maintain uniform
wall thickness
- Sharp corners, upon material shrinkage, may also cause high stresses and hence may
have to be appropriately filleted or rounded.
- Radiused corners also assist smooth flow of material and part ejection.
- Radius specifications for the complete part must be avoided to prevent unnecessary
increase in mold cost.
|
|
Guidelines for Wall Thickness
|
|
Plastic materials are bad conductors of heat; hence thicker sections take a longer
time to cool compared to thin regions. Such differential cooling rates can cause
problems like warping, distortion, voids and sink marks. To avoid such issues, plastics
parts must have uniform wall thickness (with minimal variations). Transitions between
thick and thin regions, if any, must be smooth. To add strength to the model in
spite of the reduced material mass, features like ribs and bosses are used.
|
|
|
|
Note:The guidelines and related parameters mentioned above are only indicative and
may change depending material, process and applications.
|
|
|