Premium Finishes When
Routing of acrylic has
become one the most popular methods of plastic fabrication in the sign and point-of-purchase
industries. As the accuracy of the CNC routers improves and approaches that
of CNC mills additional gains are being made into the machine building, medical
devices, and valve industries. A common quality across all of these industry
segments is the requirement for a premium finished edge on acrylic without the
need for post-routing finishing operations. Four factors in the routing operation
typically will affect the quality of the cut edge: Tooling, Programming, Machine
Condition, and Fixturing. If any one of these factors is not optimized, it will
be extremely difficult to maintain a consistent, high quality edge finish. Two
of the factors - Tooling and Programming - will be covered in this article and
the remaining two in a future article.
Tooling is a broad topic,
but there are some simple guidelines that can be used to decrease the likelihood
of failure during cutter selection. The first selection criterion for router
tooling is typically diameter. While is a common request for tooling diameters
to be in the 1/8" to ¼" range, designing the parts, fixtures, and
programs for 3/8" to ½" tooling can dramatically improve surface finishes
and consistency from job to job. A typical result from increasing cutting edge
diameter from ¼" to 3/8" can be a drop in surface finish from 40-60
RMS to 18-25 RMS. This is usually accompanied by an increased feed rate as well
as better chip extraction. The stability and flute depth offered by larger diameter
cutting tools cannot be overestimated. That said, it is important to note that
there is typically only a marginal benefit when increasing cutting edge diameters
over ½" as long as the depths of cut are not exceeding 2". The price-to-performance
ratio cannot typically support the use of 5/8" to 1" diameter cutters
in sheet stock.
After diameter, cutter
configuration is frequently the second selection criterion for tooling. As a
rule of thumb, the smaller the diameter of cutter that is being used, the more
likely it is that a spiral configuration will yield the optimum edge finish.
While straight flutes typically have good success in larger diameters (3/8"
and above), it is the spirals that excel when cutting with small diameter tooling.
Single edge spiral O-flutes (see Figure 1) typically give the best edge finishes
in ¼" and smaller tooling. When moving into the larger diameters, typically
low helix multi-fluted tools will yield the best results with some variations
depending on the manufacturing method of the acrylic (i.e. cast or extruded)
and any fillers that may have been used. It is also in these larger diameters
that the double edge straights can typically begin to perform well. Both V-flute
and O-flute configurations have been shown to work well through testing and
industry use. (see Figures 2 & 3)
A final note on tooling
is to mention the existence of numerous specialty tools available in the market
today. There are products that can be used to provide a radiused edge on parts
(Figure 4), to rout a finished edge and apply a top chamfer at the same time
(Figure 5), or to create a smooth bottom surface during pocketing without the
swirling effects of standard router bit points (Figure 6). These cutters either
solve problems that have been recurrent in the industry or allow fabricators
to eliminate tool change cycle times and/or utilize machines without tool changers.
Selecting the right cutting
parameters and cutting methods is extremely important when edge finish is the
primary driving factor of an operation. Every material and cutter combination
has a "sweet spot" in the cutting parameters and slight deviations
in any direction can cause an unacceptable decrease in surface finish quality.
Feeds and speeds are typically
the best known variables as far as cutting parameters and they are extremely
sensitive to minor variations. Unlike many other commonly routed materials,
plastics, and particularly acrylics, have an extremely narrow chip load range
that can be used to produce an optimal finish. (see Figure 7). Each cutter (based
on configuration and diameter) will have a different optimum chip load for each
material type. As a rule of thumb, the following feed rates are good starting
points if the goal is optimum edge finish. A constant spindle speed of 18,000RPM
and a depth of cut equal to the cutter diameter is assumed.
- 1/8" Diameter Tooling:
- ¼" Diameter Tooling: 100-200ipm
- 3/8" Diameter Tooling: 125ipm to 250ipm
- ½" Diameter Tooling: 150ipm to 300ipm
As long as the router bit
is not having stability problems and the workpiece is well fixtured, most of
these feedrates can be increased by simply increasing the spindle RPM. With
the newer generation spindles typically having maximum speeds of 21,000 to 24,0000
RPM, most of these feed rates will have plenty of room for improvement. The
only consideration to remember is that, unlike other materials, increased spindle
speeds must be accompanied by an increase in feed rate to remain within that
"sweet spot" on the chipload. Excessive spindle speeds will typically
melt the plastic or cause a wiping or smearing action on the finished edge that
reduces the quality of the surface finish.
After feeds and speeds
have been dialed in (usually through manufacture recommendations, as trial-and-error
is a time and material intensive process), the next step is to choose the cutting
method. Both conventional and climb cutting have their place, but here is the
rule of thumb: Larger diameters almost always perform better in a conventional
cut mode. Smaller diameters are entirely material dependent and must be tested
to determine the best method.
Other programming parameters
that should be considered are finish passes, entry points, and depths of cut.
Typically smaller diameters are the only tools that require finish passes for
optimum edge finishes. There is usually only a marginal gain in finish quality
for acrylics when 3/8" and ½" tooling is used in a two pass system.
The biggest problem that seems to surface in the industry regarding finish passes
is the amount of material to remove. Many CNC operators and/or programmers have
previous experience in the metal working industry and that can be a detriment
when attempting to use similar cutting parameters in acrylic. A typical finish
pass in ferrous and non-ferrous metals can be as little as .004"-.005".
When this amount of material is remove in acrylic, it frequently will compress
and cause the cutter to actually skip across the surface. This is due mainly
to the high rake angles employed in plastic tooling and the aggressiveness of
their cutting action. Without at least .015"-.030" of material to
remove, most acrylic router bits will not have enough material to bite into
and will actually show a deteriorated finished edge over the initial roughing
Entry points can also be
a troublesome issue during programming. While most acrylics do not exhibit the
chip wrap problem prevalent in other softer plastics, their tendency to craze
can sometimes inhibit their ability to be machined at high speeds during cutter
entry. The most common method is to slow the feed rates down to compensate for
this problem, but a ramped entry can work equally well and will not show the
entry melt that is associated with direct plunging by router bits. Another issue
on cutter entry is that because router bits do not have a centering point similar
to drills (this is to allow flat bottom cutting), they will have a tendency
to "walk" during the plunge. The visible result is a larger entry
point then the routed channel that will follow. The result is somewhat similar
to what a keyhole slot looks like with a large diameter hole followed by a smaller
slot width. Once again ramped entry can reduce this effect, but it is easier
to enter the cut by plunging into a scrap area and moving to the final cut path
in a lateral direction.
As a final parameter to
be considered, depths of cut are critical to ensuring consistent edge finishes
and non-broken tooling. A good rule of thumb is a maximum of twice the cutter
diameter per depth of cut. A favorite programming method is to use multiple
depths of cut when cutter breakage is an issue and the to take a final clean-up
pass of .015" for the entire material thickness. (see Figure 8) This gives
a premium edge finish while preventing broken tools in the smaller diameters.
It is a common concern that taking finish passes in small parts will cause the
parts to move once they have been cut away from the scrap, particularly in intricate
parts like letters. The best solution is to use the multiple depth pass/single
finish pass method described above, but to not cut through the paper masking
on the bottom side of parts. This allows the vacuum to continue holding the
parts, while the .015" finish pass will not typically tear the parts off
of the masking.
While much of the information
presented above was in the form of Rules of Thumb, it is essential that only
the proper cutting tools and cutting parameters be used when machining acrylics.
The information presented here is a broad overview of information regarding
routing of acrylics. The best source of detailed information is typically the
tooling manufacturers recommendations either through published sources or their
Technical Services department.