HEIDENHAIN CNC Pilot 4290 - Manual (Page 158)

4 DIN PLUS 146
Thread cycle G36
G36 cuts axial/radial threads using driven or stationary tools.
Depending on X/Z, G36 decides whether a radial or axial thread will be
machined.
Move to the starting point before G36. G36 returns to the starting
position after having cut the thread.
Parameters
X:
Diameter – end point for axial holes
Z: Length – end point for radial holes
F: Feed per revolution - thread pitch
Q: Number of spindle - default: 0 (main spindle)
B: Run-in length for synchronizing spindle and feed drive (see G33 )
H: Reference direction for thread pitch – default: 0
■ H=0: Feed rate on the Z axis
■ H=1: Feed rate on the X axis
■ H=2: Feed rate on the Y axis
■ H=3: Contour feed rate
S: Retraction speed (higher speed for the retraction) – default:
Same speed as for tapping
Types of taps:
■ Stationary tap: Spindle and feed drives are
synchronized.
■ Driven tap: Driven tool (auxiliary spindle) and feed
drive are synchronized.
■ ”Cycle stop” becomes effective at the
end of a thread cut.
■ Feed rate override is not in effect.
■ Do not use spindle override!
■ Use a floating tap holder if the driven
tool is not controlled, e.g. by a ROD
encoder.
4.9 Dr
illing Cy
cles