Info, Links, and Questions Answered for Star Swiss-Type Lathe Programming and Machining
Updated Friday, February 02, 2001
This page contains links and information for the programming of Star Swiss-Type CNC Lathes. No particular warranty of compatibility or usefulness of the information given below, or any other liability, is inferred or implied by Star CNC Machine Tool Corp. This information is provided as a reference only.
Collet Sleeve Pin Macro
32mm Ejector Pin Macro
Drill Pecking Macro
How Do I
Single-Point Long Threads?
The single-pointing of long threads on a
Swiss-Type lathe (or any lathe, for that matter!) can be
very tough sometimes. Sometimes it is even impossible!
Anything that comes out of the back of the bushing of a
Swiss-Type Lathe when retracted to present a threading
tool, is "long".
Die heads, even if you could fit them in the machine (clearance
being a problem typical of Swiss-Type machines), work OK
on larger threads, but with small threads and high
diameter/length ratios, twisting and breaking of the
blank may occur. Rolling heads are less of a problem in
this regard, but still pose clearance problems.
Moving the single-point tool away from the guide bushing,
by whatever means, is necessary, to overcome the problems
encountered when retracting the prepared diameter into
the guide bushing support. There is an adapter or special
tool holder available for every Star machine that will
accomplish this. If necessary, have the guide bushing
made with lands as long as possible (extend them
backwards as long as possible, and even forward into the
machine if necessary and possible), and have a bushing
insert pressed into the back (non-slotted portion) of the
guide bushing that is honed the same size as the guide
bushing bore.
A progressive turning/threading method works well in some
cases, and may be the best choice if you are machining a
typical 60-degree V-thread with standard tolerances.
There is some programming involved, and if the thread
wall is thin and the crest is sharp, as with some
threads, the blend mark will be seen.
Single-pointing with a secondary support from the
opposite side works in some cases, when the machine is
capable of doing this. Using a "half-round"
support with the proper radius, or using a support milled
with a square corner to the part (providing 2 points of
support rather than trying for a full surface contact),
has been successful. BUT, again, if the thread wall is
thin and the crest is sharp, deformity of the crests from
the pressure of the deflection of the thread OD against
the secondary support will occur.
When single-point threading into or from a secondary
support bushing of any shape, care for the thread
shoulder, if any, must be taken, and very precise control
of the blank diameter is usually required.
How do I
Manually Program Tool Nose Radius Compensation?
Compensation for X (diametrical) axis
Nose Radius Compensation = 2(nose radius -(nose radius (TAN
(45 - angle / 2 ))))
To find the X axis compensation value:
1. Divide the programmed move angle by 2.
2. Subtract the answer #1 from 45.
3. Find the tangent (TAN) of the answer #2.
4. Multiply the answer #3 by the tool nose radius.
5. Subtract the answer #4 from the tool nose radius.
6. Multiply the answer #5 by 2.
The answer of #6 is the compensation value for the X axis.
Compensation for Z (radial) axis
Nose Radius Compensation = nose radius-(nose radius(TAN (
angle / 2)))
To find the Z axis compensation value:
1. Divide the programmed move angle by 2.
2. Find the tangent (TAN) of the answer #1.
3. Multiply the answer #2 by the tool nose radius.
4. Subtract the answer #3 from the tool nose radius.
The answer #4 is the compensation value for the Z axis.
Cautions With
the G50 Command
If, after having processed a G50 work coordinate shift,
one stops the process, say by RESET or by switching out
of Memory mode, and then one wishes to restart the
process, it is CRITICAL that the work shift not be
duplicated. Zero Return the axis to cancel the shift, or
be sure to restart the process at a place in the program
AFTER the G50 statement which has already been processed,
and BEFORE any subsequent G50 statement.
Otherwise, the coordinates may be shifted again (on top
of) by a G50 command in the program, and the very real
possibility of an accident is presented. To get around
this problem, use offsets, either wear or geometry,
instead of the G50 coordinate shift. This will sometimes
make the machine do a "herky-jerk" movement
when the offset is cancelled, but that can be programmed
around by commanding an incremental move on the same line
as the offset cancel code with a move distance equal to
the offset. The major benefit of using offsets rather
than the G50 command is eliminating a potential accident
due to operator error with G50s.
Another way to use offsets for coordinate shifts while
still retaining direct program control of the shift value
and avoiding large wear offsets is to use the G10 (optional)
function to rewrite the offset after each tool call:
T100
G10 P1 W1.0 <------ Shift amount - This command will
add 1.0 to the Z value in offset #1.
Roll Thread or
Cut Thread?
Use roll taps whenever possible! They last a long time,
make very consistent threads as long as the hole size
doesn't vary too much, there are no chips, and best of
all, they are much stronger than taps with flutes -
very important with small thread sizes. Additionally,
formed threads are stronger than cut threads.
The only drawback is the threads look a little funny,
compared to cut threads. The crests (minor diameter) are
"rolled over", sometimes looking like the
thread was tapped twice and cross-threaded. Some end-users,
particularly in the medical industry, do not like this
appearance and will not accept the parts.
Formula for
calculating feed rates when machining with the C axis, as
with Cylindrical Interpolation
Nobody said this was easy, so follow me...
You must (surely you do!) know at least [D], [Z], [C],
AND [P] OR [F].
P = PROGRAMMED FEED IN DEGREES PER MINUTE
F = DESIRED FEED IN INCHES PER MINUTE
L = ASSUMED MOVE DISTANCE IN INCHES
A = ACTUAL MOVE DISTANCE IN INCHES
Z = LONGITUDINAL MOVE DISTANCE IN INCHES
C = ORIENTATION MOVE DISTANCE IN DECIMAL DEGREES
D = PREPARED DIAMETER IN INCHES
First, solve for the following:
L = SQRT [ [ Z SQUARED] + [ C SQUARED] ]
A = SQRT [ [ Z SQUARED ] + [ C / [ 360 * [ D * 3.14159 ]
] ] SQUARED ] ]
Using the values calculated above, below is the formula
for calculating the feed rates:
To find [P] the PROGRAMMED FEED IN DEGREES PER MINUTE
when [F] the DESIRED FEED IN INCHES PER MINUTE is known:
P = [ L / A] * F
To find [F] the actual FEED IN INCHES PER MINUTE when [P]
the PROGRAMMED FEED IN DEGREES PER MINUTE is known:
F = [ L / A] / P
Any time the [D], [Z], or [C] values change [P] must be
recalculated in order to maintain [F]. ;-)
Formula for
finding the helix angle of a thread (as used in thread
milling - those in the know, know.)
P = Thread lead ( 1 / threads per inch = lead)
M = inch minor diameter of thread
H = decimal helix angle
H = ARCTAN [ P / [ M * 3.14159 ] ]
Formula for
calculating degrees of rotation during Cylindrical
Interpolation
H = Programmed move distance in degrees
C = Inch distance of desired move around the circumfrence
of the cylinder
D = Turned inch diameter
H = [ [ C * 360 ] / [ D * 3.14159 ] ]
Return to Star Tech Center, Ohio, Main Page
