As
a machining operation, the process of machining grooves is typically performed
on a CNC lathe. A general purpose program required to make only the simplest of
grooves is very straightforward – it includes only two small operations of the
grooving tool - the
plunge-in
as the first motion
,
then
rapid
out
as the second toolpath
motion. Grooves of this type are rather rare and seldom done on CNC lathes, as
their cost would be too high as compared with alternate methods of production
(such as manual machining). The majority of grooves that need to be programmed
belong to the category of
precision
- or at least
semi-precision
- grooves. When planning a program for grooving
operations, you have to consider the best selection out of many methods
available. Once the groove machining selection is known, the rest of the
programming process is rather simple.
Various
tooling catalogues offer a multitude of grooving tools suitable for CNC lathe
work. The two basic considerations regarding the tooling selection for grooving
are:
Of
course, other features are also important, such as selecting the proper insert
grade, insert coating, corner radius, chipbreaker, etc. Still, the width and
the depth of grooving tool are the most important features for programming. For
certain type of grooves, additional tooling considerations will also be very
important, such as the radial clearance for face grooves.
Cutting Width
In
an engineering drawing, the width of a square groove is typically given either
as the actual width (wall-to-wall distance) or the absolute dimension to both
walls. A combination of the two methods is also quite common. At the very
least, groove width determines the grooving width insert. For precision groove
machining, the insert selection is very important - the basic rule is that the
insert width should always be smaller than the groove width. This will require
more than one plunge, but the groove quality will improve. In order to minimize
the number of plunge cuts, select the widest grooving tool suitable for the
job.
Cutting Depth
Any
selection of grooving tool must also take into consideration the groove depth,
as specified in the drawing. Catalogues specifications for grooving tools
determine the maximum depth allowed for the selected tool. It is not unusual to
increase
the cutting depth by modifying the insert,
usually by grinding off a small portion, providing the coating and the insert
width are not compromised.
Groove Location
Groove
location - or
position
- is normally measured as being
relative to a particular face or a shoulder. The drawing designation has a very
important impact on the selection of the grooving tool command point. As
illustrated on the previous page, groove location can be defined in the drawing
by
either
the Z1 position
or
the Z2 position
but not both
. For the objective of this subject, the
dimensions are from the front face of the part, but could be defined from any
other location. If both Z1 and Z2 are given, they also define the width of the
groove.
Many
grooves are classified as
precision
grooves rather than utility
grooves, typically defined by adding tolerances to the groove dimensions. More
details on grooving tolerances are described in the subject of
precision grooves
. Selection of the tool command point is important
not only for the actual setup at the CNC machine, but also for the programming
method.
Setting the Command Point
For
programming purposes, the grooving tool should be treated with the same practical
approach as any other tool in terms of the command point selection -
how it benefits the CNC operator
. As for all cutting tools, the command point of
grooving inserts is the
reference
point of such tool, relative to
part zero. This is the point that follows the XYZ (mill) or XZ (lathe)
coordinates in the part program. Precision grooving programs typically require
that the programmed command point is changed within the program, often combined
with a change of offset.
Square Inserts
A
command point for a typical square grooving insert used on CNC lathes is typically
programmed either to the
left
or the
right
bottom corner of the insert, as viewed by the
CNC operator. The same method applies for other square grooves, such as inserts
with
specified
corner radiuses, also with a flat section at the
bottom.
Note that all square inserts have
some
corner radius, but not always
specifically defined.
Round Inserts
Many
round inserts fit into the same tool holder as their square counterparts and
are set the same way. Round inserts have no flat section at the bottom and are
often used for recess grooving in shaft work, to increase the torque strength.
In many cases, programming technique uses a simple
'plunge and retract'
method, without any contouring.
Although
square inserts are often used for minor groove profiling (tapered walls, for
example), round inserts have much larger field of applications for various
groove contours.
