General
Input on the best molding method for the design concept should be sought
early in the design process so the part shape can be optimized
accordingly. This will ultimately reduce material and manufacturing
costs. Akron Porcelain & Plastics can offer significant material and
processing information to assist the product designer.
As with other
plastic materials, good thermoset plastic part design requires
consideration of a number of aspects: tolerances, shrinkage, wall
thickness, draft angles, radii, fillets, ribs, bosses, holes, threads,
inserts, etc. The following suggestions are fundamental practices to
follow when designing a thermoset molded part.
Tolerances
It is best to always design with generous tolerances in mind since
extreme dimensional accuracy can be difficult and expensive. The main
contributors to dimensional variation in the molding process are: mold
dimensions, molding shrinkage, post-shrinkage, warpage, and machine
process variations.
Typical molding tolerances for properly designed parts are plus or minus 0.003" per inch, and are increased by an additional plus or minus 0.005" when measuring across the mold parting line.
Material
Shrinkage
Each molded part has a characteristic shrinkage defined as the
difference between the dimensions of the mold and the molded part when
measured at room temperature. Shrinkage varies, ranging from 0.001" to
0.015" per inch depending on the specific material, flow grade, molding
method and process parameters. Non-uniform cross sections will result in
varying shrinkage within the same part and should be avoided.
Wall Sections
Uniform wall sections are important. Thick wall sections require
increased cycle time in order to fully cure the material, so sectional
thickness should be minimized without sacrificing strength. If possible
thick sections should be thinned or cored out with a pin or blade to
reduce part weight and cycle. Sink marks do not occur with thermoset
materials, but uneven sections can cause warping and shrinkage variation
due to uneven cooling. Generally, nominal wall sections range from
0.050" to 0.125", but thicker sections are achievable. Sections in other
areas of the part should be within 25% of the nominal wall section.
Sudden changes in wall section should be avoided.
Thin sections, edges and sharp corners can result in breakage problems during the secondary deflashing operations required with thermosets. Thin sections can also cause flow problems and weld lines possibly resulting in warping, breakage, and electrical failure.
Draft Angles
Draft should be provided on all vertical mold surfaces for proper part
release. A draft angle of one degree per side is sufficient on side wall
sections, and two to three degrees are desirable on deep barriers and
bosses.
Radii and
Fillets
Adequate radii and fillets eliminate stress concentrations, improve
flow, reduce cracking and improve overall strength with very little
additional weight and cost. Minimum radii for all inside and outside
corners are typically 25% to 75% of nominal wall thickness with a
minimum radius of 1/64".
Ribs
Ribs increase rigidity and strength without changing the nominal wall
thickness. Typical ribs are half as thick as the nominal wall section,
and should not be any closer together than twice the nominal wall
section. Sufficient rigidity is achieved with rib heights that are three
times the rib thickness. Free standing ribs should be avoided since they
are prone to breakage. Since sink marks do not occur in thermoset
materials, ribs, bosses, etc. can be added where needed to enhance the
design.
Bosses
Bosses should be located in the corners of the molded part and be no
more than twice the diameter in height. If additional height is
necessary, ribs are recommended at the base of the boss for added
strength. Three degree draft angles and a generous radius at the base of
the boss will aid part release and strength. Hollow bosses should have
wall sections at least equal to the inside diameter.
Holes
Through holes are easier to produce because the mold core pins can be
supported from both ends. Blind holes are formed by pins supported from
one end only, and these pins must be strong enough to withstand molding
forces. When designing compression molds, core pins should not be more
than 2 ½ times the diameter in length or pin breakage will be a problem.
With 0.062" diameter pins the pin length should not exceed the diameter.
In applications where pins must be longer, designing the core pins with half the length in each side of the mold, with 0.002" to 0.005" clearance between the tips when the mold is fully closed, is recommended. To account for any mismatch, one pin should be slightly larger in diameter than the opposite pin. As a general rule, edges of holes should be at least twice the nominal wall section from part edges or other holes.
Threads
Threads may be molded or tapped. Fine threads of 32 threads per inch
should be avoided. Molded pilot holes with chamfered edges are
recommended for secondary tapping operations. Thread cutting
self-tapping screws also work well and eliminate the need for molded or
tapped threads. Do not use thread forming screws.
Parting Line
Flash
Due to volatile gasses generated during the molding process, low melt
viscosity and other processing conditions, parting line flash is
inherent in the thermoset molding process. Even newly built molds
generate flash that must be removed from the part with a secondary
process. Some typical methods are: batch de-flashing, belt fed
de-flashing, and hand finishing. When possible, the part should be
designed with generous radii and fillets so the most economical method,
batch de-flashing, can be employed. Other de-flashing methods will
increase part cost. If cosmetics are highly critical, hand or
specialized de-flashing may be required.
Inserts
Molded-in inserts should be used only when there are no acceptable
alternatives. Brass and aluminum have thermal expansion properties most
compatible with thermoset plastics. Thin wall inserts with sharp corners
should be avoided. Diamond knurling usually provides the best anchorage,
although single grooved inserts free of sharp edges also work well.
Knurled inserts can be pressed in immediately after molding, preferably within three minutes of molding, to take advantage of part shrinkage. The hole for the insert is based on insert size and normal material shrinkage. Hole diameters for small inserts should be 0.001" to 0.002" smaller than the insert outside diameter. Larger inserts will require additional anchorage. When working with thin wall sections, apply 50% of the normal shrinkage when determining the hole diameter so as to prevent cracking. The wall section around the insert should be 0.8 times the insert diameter for 0.5" diameter or less inserts, and 1.5 times the insert diameter for larger inserts.
Quick Prototype
Sample Parts
Once the chemical, physical and electrical properties are defined, it is
best to construct a 3-D CAD file and possibly fabricate a quick
prototype to fully evaluate the part. It will then be easy to identify
areas that need further attention. For example, knife edges on the part
are often overlooked during the early design phase and can result in
chipping. Likewise, knife edges in the mold itself are prone to wear and
damage ultimately causing extra tool maintenance. Akron Porcelain &
Plastics can provide quick prototype SLA and SLS parts so the design
concept can be properly evaluated.
Prototype Molds
When working with a new application it is best to construct a prototype
mold to evaluate the performance of the part design prior to
constructing a multi-cavity production mold. In many cases the prototype
mold cores and cavities can be used in the multi-cavity production mold
as well to help minimize development costs. To replicate the ultimate
production part properties, the prototype mold should be designed to
operate under the same processing conditions as the production mold.
Summary of General Design Guidelines for Thermoset Plastics:
Molded Part
Tolerances: +/- 0.003" per inch, additional +/- 0.005" when
measuring across the mold parting line.
Material Shrinkage: 0.001" to 0.015" per inch depending on the
grade of thermoset material.
Typical Nominal Wall Thickness: 0.050" to 0.125" with less than
25% variation
Draft Angles: one degree/side on side wall sections, two to three
degrees/side on deep barriers and bosses.
Radii and Fillets: 25% to 75% of nominal wall section, minimum of
1/64" radius.
Rib Thickness: 50% of nominal wall section
Rib Height: Three times rib thickness
Boss Height: Less than two times the outside diameter of boss
Boss Draft Angle: Three degrees
Hollow Boss Wall Section: Two times inside diameter of boss
Hole Depth: 2.5 times hole diameter (when compression molding)
Hole Edge Locations: Twice the nominal wall section from part
edges or other holes.
Hole Diameter for Inserts: 0.001" to 0.002" less than insert
diameter for small inserts, increase slightly for larger inserts.
Hole Wall Thickness for Inserts: 0.8 times insert diameter for
0.5" diameter or less inserts, 1.5 times insert diameter for larger
inserts.
Insert Type and Material: Diamond knurled brass or aluminum.
