Programming
Thread Milling
Milling
is a great way to create a thread.
Recall from last month’s column, we discussed advantages of
thread milling. Some
people might be concerned with programming issues when thread
milling. Well let’s
look at a sample. The
following program is designed to thread mill a 2.625 x 14 TPI
internal thread using a 1.00” diameter multiple flute cutter with
3/4” flute length.
The
plan is to position the cutter to the lowest point of the thread and
feed out of the part. Our
program calls for the tool to use a 45º ramp-in move, complete a
360º rotation within the part and then finish with a 45º ramp-out
move.
For
this program we are using the center of the threaded hole as the
datum. At this point,
the coordinates are X0, Y0. The
first thing to calculate is the cutter start point called the
“pivot” point. This can be calculated as follows.
Pivot
point =(part diameter - cutter diameter) ÷ 2
Pivot
point =(2.5” - 1.0”) ÷ 2 = 0.750”
The
cutter begins to cut the thread when the cutter is in this position
(X0.750, Y0).
Although
this is the point at which the tool begins cutting the thread, we
must get the cutter to this point with a helical ramp-in move.
Use
a point 45º from the datum point, midway between the X-axis and
Y-axis zero line. This is half the value of the pivot point in both
X&Y and represents the ramp-in start position. This is 0.75 ÷ 2
= 0.375.
There
are two advantage of this 45º start-point.
First, the X and Y start and finish values are half the pivot
point value. Second, we can easily calculate the amount of Z-axis
movement required.
Calculate
the Z-axis moves based on the required circular movement.
The Z-axis move for a full 360º rotation is the pitch.
pitch = 1/14 = 0.0714”
We
selected a 45º ramp-in move, so we can see that the Z-axis distance
for this move will be 45º/360º x 0.0714 = 0.0089. |
Let’s
see how these values are used in the program.
In this example the Z-axis start point is Z-0.500 and the
milling method is climb milling.
Program
example
N10
T1
M 6
Tool change
N20
S1293 M
03
Spindle on
N30
G0 G90 X 0.0000 Y 0.0000 M08
Datum point
N40
G43 H01 Z0.1000
Rapid above part
N50
G1 Z- 0.50
F50. Feed to
depth
N60
G1 X 0.375 Y-.375 F9. G41 D01
Ramp in start position
G code for climb mill
N70
G3 X.75 Y.000 R.375 Z-
.4911 F 5.
Ramp in to pivot point
N80
G3 X .75 Y.000 I- .75 Z- .4196
Circle mill
N90
G3 X.375 Y.375 I-.375 Z-.4107
Ramp out
N100
G0 X.0000 Y.0000
G 40
Return to
datum cancel comp.
N110
G0
Z1.000
Retract from part
In
block N50 we feed to full depth and then move to the starting point
for the ramp-in position. Remember that this is half the pivot point
value.
The
ramp-in move is a helical interpolation move with the X and Y axis
moving incrementally 0.375 and Z moving 0.0089 upwards.
Look
at line N70 and note that the ending Z absolute position is 0.0089
less than the starting point in block N50.
Block
N80 cuts a 360º circular move using a negative I value. During this
helical move the absolute Z value reduces by 0.0714.
Block
N90 is the ramp-out position and again uses a 45º move in the X and
Y axis with an incremental move of 0.0089.
I’m
sure there are many thread milling methods out there.
We hope this methods is easy follow and helpful in further
understanding thread milling.
|
