This
is the simplest of all machining methods that is used in groove programming.
The section title essentially defines the whole operation. The type of groove
that belongs to this category is a rough groove, for example, one that will be
completed later. Also in the same category may belong some utility grooves that
are nothing more than open clearances. Edge burrs may or may not matter in such
cases, but the general approach to programming such grooves is not precision
oriented.
In
the following example, the simplest groove possible is programmed
(any prior machining is assumed to
have been completed)
. Note that
there is no effort in the program to control groove tolerances and/or its
surface finish, sharp corners or burrs included. This is a typical utility
groove that is often machined on manual lathes, because its much cheaper than
using a CNC lathe.
The
groove is 5 mm wide (
_
0.20") and 3 mm deep (
_
0.12"),
as the drawing shows. The command point for the selected tool is set at its
lower left corner, and the program will use T02 for the example:
…
N11 T0100
N12 G96 S150 M03
N13 G00 X28.0 Z-11.0 T0202 M08
N14 G01 X20.0 F0.15
N15 G00 X28.0
N16 X100.0 Z200.0 T0200
N17 M01
…
A
program with the same result can also use a special cycle G75, used for cutting
along the X-axis.
G75 Cycle
Fanuc
lathe controls offer a cycle listed under the multiple repetitive cycles
section in the manuals. This cycle is designed for grooves that require an
interrupted cut, for example, those machined in tough materials, deep grooves,
or in any other type of machining where the chip breaking will improve the
machining process. G75 cycle can also be used for cutting multiple grooves that
share the same characteristics.
There
are two formats for the cycle, depending on the control unit. For 10/11/15
Fanuc controls, use the one-block format:
G75 X.. Z.. I.. K.. D.. F..
where
…
X = Final groove diameter
Z = Z-position of the groove (last groove for multiple
grooves)
I = Depth of each cut (positive value)
K = Distance between grooves (positive value) - for multiple
grooves only
D = Relief amount at the end of cut
F = Cutting feedrate in selected units
Spindle
speed can also be programmed in the same block.
A
two-block format is used for 0/16/18/20/21 Fanuc controls:
G75 R..
G75 X.. Z.. P.. Q.. R.. F..
where …
R = Clearance for each cut (return amount) (first block)
X = Final groove diameter
Z = Z-position of the groove (last groove for multiple
grooves)
P = Depth of each cut (positive value)
Q = Distance between grooves (positive value) - for multiple
grooves only
R = Relief amount at the end of cut (second block)
F = Cutting feedrate in selected units
The
program on the previous page can be modified to use G75 cycle, even for a
single groove:
…
N11 T0100
N12 G96 S150 M03
N13 G00 X28.0 Z-11.0 T0202 M08
N14 G75 X20.0 I1.0 F0.15
(EACH CUT WILL BE 1 MM DEEP)
N15 G00 X100.0 Z200.0 T0200
N16 M01
…
For
a two-block format, the program will change only slightly:
…
N11 T0100
N12 G96 S150 M03
N13 G00 X28.0 Z-11.0 T0202 M08
N14 G75 R0.25
N15 G75 X20.0 P1.0 R0.25 F0.15
(EACH CUT WILL BE 1 MM DEEP)
N16 G00 X100.0 Z200.0 T0200
N17 M01
…
As
these examples represent a single groove, note that in either program, there is
no Z-location and there is no distance between grooves.
The
main difference between the two formats is that the relief amount for each cut
can only be programmed in the two-block format. In the one-block format, this
amount is set by a system parameter. Both formats support programming of the
relief at the bottom of the groove.
The
majority of programming CNC grooving operations falls into the category of
precision groove
. Although the term 'precision groove' may be
interpreted in different ways, the common denominator of CNC programs developed
for precision grooves is the focus on maintaining the precise
groove location
and
groove
width
. This requirement is
defined in the drawing by using various tolerances.
A
typical precision groove requires good planning of the actual machining. The
first requirement is the selection of a grooving insert, particularly its
width. The width of grooving insert must always be
smaller
than the groove width, which means more tool
motions than a simple plunge-retract method.
Once
the suitable insert has been selected, the machining method has to be carefully
planned. The technique can be itemized into steps. Once the steps are
finalized, they can be transferred into the program itself. The steps suggested
in this section apply to a groove that can be machined with only one roughing
cut. For wider grooves, the technique is very similar, and an example will be
provided later in this section. Command point of the grooving tool is set to
the left for the following procedure.
Machining Procedure
MOTION 01 From a tool change position, move the tool to a
Z-position, where the middle of the insert width matches the vertical
centerline of the groove
MOTION 02 In X-axis, move the tool close to the part diameter
(1 mm or 0.020" per side suggested) *** START POSITION OF THE GROOVING
TOOL ***
MOTION 03 Feed the tool into the material, leaving a very
small amount at the groove bottom (0.125 mm or 0.005" per side suggested)
MOTION 04 In rapid mode, retract to the same diameter where
the previous cut started from
MOTION 05 Still in rapid mode, use an incremental motion to
the start of the
left
groove chamfer (or
radius)
MOTION 06 In feedrate mode, cut the chamfer to size
MOTION 07 Continue the cut on the
left
wall of the groove, to the groove bottom -
leave the same amount of material at the bottom, as in Motion 03
MOTION 08 In rapid mode, retract to the start position (as
established in Motion 01 and 02)
MOTION 09 Still in rapid mode, use an incremental motion to
the start of the
right
groove chamfer (or
radius)
MOTION 10 In feedrate mode, cut the chamfer to size
MOTION 11 Continue the cut on the
right
wall of the groove, to the groove bottom
(final diameter)
MOTION 12 Sweep the bottom of the groove, so the left corner
of the insert touches the left groove wall
MOTION 13 In rapid mode, retract to the start position (as
established in Motion 01 and 02)
When
described in such a step-by-step method, the process may seem a bit
complicated. The best approach to take is to follow each step on its own,
rather than all steps together.
Note
-
if properly calculated, the incremental
Motion 05
and
Motion 09
will have identical increments, although in the
opposite directions. Programming these motions in incremental mode makes the
programming much easier. This method allows a change of the command point from
the left corner to the right corner (and vice versa), with only the simplest of
calculations.
The
groove shown at right is a typical groove suitable for the above described
programming procedure.
If
no tolerances are given or only the location tolerance is specified, a single
offset in the program is sufficient. It will control the groove
location
relative to the front face, but it will
not
control the groove width. If groove width is to
be controlled as well, an additional wear offset for the same tool must be
programmed.
Programming Procedure
Once
the machining procedure has been established, it can be applied to the part
program. The programming procedure will follow all steps described above.
Always study the drawing first! For the example, a 4 mm wide grooving tool will
be used, with the command point set to its left corner. On the previous page is
a drawing that shows a tolerance on the groove location, but not on its width.
There will be only
one
wear offset required by the
part program.
Now,
the
machining
procedure can be converted to the
programming
procedure:
MOTION 01 G00 Z-10.5 T0202 M08
MOTION 02 X28.0
*** START POSITION OF THE GROOVING TOOL ***
MOTION 03 G01 X20.25 F0.15
MOTION 04 G00 X28.0
MOTION 05 W-1.9
MOTION 06 G01 U-2.8 W1.4 F0.1
MOTION 07 X20.25 F0.15
MOTION 08 G00 X28.0 Z-10.5 (START)
MOTION 09 W1.9
MOTION 10 G01 U-2.8 W-1.4 F0.1
MOTION 11 X20.0 F0.15
MOTION 12 Z-11.0
MOTION 13 G00 X28.0 Z-10.5 (START)
Actual
program segment can now be developed:
…
N21 T0200
N22 G96 S120 M03
N23 G00 Z-10.5 T0202 M08 (MOTION 01)
N24 X28.0 (MOTION 02)
N25 G01 X20.25 F0.15 (MOTION 03)
N26 G00 X28.0 (MOTION 04)
N27 W-1.9 (MOTION 05)
N28 G01 U-2.8 W1.4 F0.1 (MOTION 06)
N29 X20.25 F0.15 (MOTION 07)
N30 G00 X28.0 Z-10.5 (MOTION 08)
N31 W1.9 (MOTION 09)
N32 G01 U-2.8 W-1.4 F0.1 (MOTION 10)
N33 X20.0 F0.15 (MOTION 11)
N34 Z-11.0 (MOTION 12)
N35 G00 X28.0 Z-10.5 (MOTION 13)
N36 X100.0 Z200.00 T0200
N37 M01
…
This
detailed example represents a typical programming method for most
semi-precision and precision grooves machined on CNC lathes. Once you
understand the programming technique used, it will be much easier to adapt it
to any groove.