Preparing for Plastic
Routing - Part 2
As companies make the transition
from the routing of wood or aluminum to the machining of plastics, there are
a number of preliminary procedures and considerations that can help ease the
conversion and ensure a smooth transition. Periphery factors in the routing
of wood and aluminum can become some of the most significant aspects of plastics
machining. Good planning and preparation can help ease these factors and the
costs associated with the startup of a new machining process.
This article is the second
of a two part series that discusses the need to have active preparation when
making the transition from wood routing to plastic routing. Part 1 discussed
the CNC router and its associated hardware. Part 2 will discuss tooling and
material selection as well as programming considerations.
Depending on the customer’s
requirements, fabricators may have leeway in specifying exactly what material
they will have to rout. This is an important option and should be taken advantage
of whenever feasible in order to reduce machining headaches down the road.
Some plastic sheet manufacturers
produce variations of their common sheet goods that are marketed as having improved
machining characteristics. By all means, try these. They typically produce better
chips, do not melt or scar as much and can sometimes reduce the problems associated
with chips wrapping on the cutters during plunging operations.
Various grades of the same
type of sheet can exhibit tremendously different routing characteristics. UV
protectants can inhibit good chip formation, fillers can cause premature cutter
wear, and different sheet colors can affect the quality of the edge finish.
Some grades may even be listed as co-polymers. These co-polymers may be listed
as a single sheet type but frequently contain a second plastic in the formulation.
It is better to test cut new grades before estimating tooling costs and routing
times because of these issues.
to verify with sheet manufacturers is if the material exhibits different machinability
going in the extrusion direction or across it. This can be thought of as cutting
with the grain or cross-grain. Most plastics do not react differently in regards
to extrusion direction, but the few that do have caused some fabricators many
Tooling selection should
be considered early during the preparation process. While it will be nearly
impossible to gage tool life (and therefore costs) if it is a new process and/or
material, tooling selection may greatly impact cycle times, fixturing costs,
programming needs, and material waste. Across the major tooling manufactures
in the U.S. today, there are over 90 style of dedicated plastic tooling with
700-800 tools to choose from. Narrowing your choices down to 1 or 2 tools or
styles of tools from a particular manufacturer can help you determine material
removal rates, chip extraction direction, and the best diameters for your applications.
This can factor in heavily when later trying to design fixtures and determine
optimum cycle times.
The very first consideration
during programming is cut direction. For almost every plastic used by fabricators,
conventional cutting will yield a superior edge versus climb cutting. The exceptions
are typically composites or combined materials. While conventional cutting is
very often the norm in routing (as opposed to climb cutting during milling),
nesting software that seeks to increase raw material yield and cycle time by
reducing the number of cuts per plastic sheet can force tooling into a climb
cut configuration. If this style of software is used by fabricators, test cuts
should be made to determine whether or not the climb cut edge finish is acceptable.
If it is not, raw material usage and cycle times need to be re-evaluated.
Another programming consideration
is plunging. Many soft plastics can exhibit severe chip wrap on the cutter after
repeated plunges. Many hard plastics can craze or "spiderweb" depending
on tool geometry, plunge speeds, spindle speeds and fixture support.
The most reliable method
for solving chip wrap is ramped cutter entry. This prevents the chips from forming
in a continuous curl and will work 100% of the time. Ramped entry requires special
attention to the location of entry holes and the location of nearby cut paths.
Other methods of solution involve pre-drilling of entry areas and specially
designed router bit point geometries.
Similar to soft plastics,
poor plunge finishes on hard plastics can be solved through a variety of methods.
Ramped entry will once again yield consistent finishes but is not the only method.
Craze-resistant grades of many popular plastics are available and can withstand
the plunge pressures of standard router bits. Solid fixturing with support directly
underneath the entry point can also improve the consistency of plunging operations.
Special point geometry on cutting tools is typically the last resort in these
types of materials. The best thing to remember when cutting holes in hard and
soft plastics is that router bits are for making traversing cuts and drills
are for making repetitive holes. The geometry of drills is far superior to that
of router bits for plunging and they should be used whenever possible.
A final programming consideration
should be to part fixtures. High quality, rigid fixturing methods are essential
to maintaining premium edge finishes and there are programming methods that
can enhance the adhesion power of various hold-down methods. In three axis routing,
a common method of increasing holding power is to leave the paper masking on
sheet goods and to rout through the plastic, but not the bottom masking sheet.
This ensures that the vacuum is not lost and provides extra vertical and lateral
grip on small pieces. Routing in this method requires extremely flat spoilboards
and may require frequent surfacing of the spoilboards to maintain their surface
dimensions depending on humidity and temperature variations.
Five axis routing programs
can benefit from higher spindle speeds that reduce the size of the chips being
formed and consequently can reduce the force being applied against the fixtures.
Multi-flute tools can also be used to achieve this benefit, but they are susceptible
to increased instances of melt and accelerated cutter wear.
The order of operations
in the CNC router program should also be examined for areas of improvements.
Small cuts and pockets should be made first to utilize the vacuum area under
scrap material. By making large part cut-outs last, scrap material can be fixtured
the same as finished material and assist in part hold down. Multiple depth cuts,
skin cutting or tabbing can also be utilized during programming to improve part
hold-down, edge finishes, and feed rates.
Advanced planning in the
areas discussed in this article and the last article - Materials, Tooling, Programming,
Runout, Collets, Vacuum, Dust Collection, Coolant - can help prevent some of
the common missteps that are associated with startups of new jobs or processes.
Addressing these issues can ensure that the tools, equipment, and programs are
ready for use when the job begins and that the run costs are inline with the