Official GSK Agents in South Africa
Tel: +27 11 626 2720, [email protected]
Chapter 3 G Commands
133
Ⅰ
Programming
mode.
5) The drilling of G83, G87 command should be set as linear axis. (G83 drilling axis is
regarded as the 2
nd
axis, G87 treats as the 1
st
one).
6) When the in-feed amount Q of each time is 0, perform the common drilling cycle. The
drillingmachining will directly feed to the botton of a hole, and then moves to the start
position at the rapid traverse rate.
3.23 Thread Cutting Commands
GSK980TDi CNC system can machine many kinds of thread cutting, including metric/inch single,
multi threads, thread with variable lead and tapping cycle. Length and angle of thread run-out can be
changed, multiple cycle thread is machined by single sided to protect tool and improve smooth finish
of its surface. Thread cutting includes: continuous thread cutting G32, thread cutting with variable
lead G34, Z thread cutting G33, Thread cutting cycle G92, Multiple thread cutting cycle G76.
The machine used for thread cutting must be installed with spindle encoder whose pulses are set
by No.070m. Drive ratio between spindle and encoder is set by No.110 and No.111. X or Z traverses
to start machine after the system receives spindle signal per rev in thread cutting, and so one thread
is machined by multiple roughing, finishing without changing spindle speed.
The system can machine many kinds of thread cutting, such as thread cutting without tool
retraction groove. There is a big error in the thread pitch because there are the acceleration and the
deceleration at the starting and ending of X and Z thread cutting, and so there is length of thread
lead-in and distance of tool retraction at the actual starting and ending of thread cutting.
X, Z traverse speeds are defined by spindle speed instead of cutting feedrate override in thread
cutting when the pitch is defined. The spindle override control is valid in thread cutting. When the
spindle speed is changed, there is error in pitch caused by X and Z acceleration/deceleration, and so
the spindle speed cannot be changed and the spindle cannot be stopped in thread cutting, which will
cause tool and workpiece to be damaged.
3.23.1 Thread Cutting with Constant Lead G32
Command format:
G32 X(U)_ Z(W)_ F(I)_ J_ K_ Q_
Command function:
The path of tool traversing is a straight line from starting point to end point as
Fig.3-82; the longer moving distance from starting point to end point(X in radius value) is
called as the long axis and another is called as the short axis. In course of motion, the long
axis traverses one lead when the spindle rotates one revolution, and the short axis and
the long axis execute the linear interpolation. Form one spiral grooving with variable lead
on the surface of workpiece to realize thread cutting with constant lead. Metric pitch and
inch pitch are defined respectively by F, I. Metric or inch straight, taper, end face thread
and continuous multi-section thread can by machined in G32.
Command specifications:
G32 is modal;
Pitch is defined to moving distance when the spindle rotates one rev(X in radius);
Execute the straight thread cutting when X coordinates of starting point and end point are the
same one(not input X or U);
Execute the end face thread cutting when X coordinates of starting point and end point are the
same one(not input Z or W);
Execute the cutting taper thread when X and Z coordinates of starting point and end point are
