HEIDENHAIN CNC Pilot 4290 Pilot User Manual

Page 74

Thr

ead cy

cle gr

oup

Thread cycle G31

G31 machines threads defined with G24-Geo, G34-Geo or G37-Geo.
G31 also machines successions of threads and multiple threads.

Chamfer length, overrun length: If you do not program ”B, P”,the
CNC PILOT will automatically determine the lengths from adjacent
undercuts or axis-parallel recesses. If no undercut/recess exists, the
chamfer and overrun lengths from Machining Parameter 7 will be used.

Parameters
NS:

Block number (from the finished part description containing the
basic block G1-Geo for thread contour definition)

Maximum approach - Maximum infeed distance

B, P: Chamfer length, overrun length
D:

Cutting direction (reference: defined direction for basic element)
– default: 0;

■

D=0: same direction

■

D=1: opposite direction

Type of feed – default: 0;

■

V=0: constant cross section for all cuts

■

V=1: constant feed

■

V=2: with distribution of remaining cut – if the division thread

depth/feed provides a remainder, the first feed is reduced. The
last cut is divided into four partial cuts: 1/2, 1/4, 1/8 and 1/8.

■

V=3: without remaining cut division – feed is calculated from

pitch and speed

Type of offset – default: 0

■

H=0: no offset

■

H=1: offset to the left

■

H=2: offset to the right

■

H=3: offset alternating left and right

Number of air cuts after the last cut – default: 0

Starting angle – default: 0

• ”Feed rate stop” becomes effective only

at the end of a thread cut.

• Feed rate override is not effective.
• Do not use the spindle override if the

feedforward is switched off!

Danger of collision!
An excessive overrun length P can cause
collision. You can check the overrun length in
the simulation.