Acu-Rite CNC 3500i User Manual

7 Programming: Canned Cycles, sub-programs



The Mill Cycle is intended for contour milling operations. Tool 
diameter compensation, Z Pecking, Finish Stock, RoughFeed, and 
FinishFeed are supported. The cycle rapids to the XY start point 
(compensated, if ToolComp "D" parameter is used) rapid to the start 
height and then feed to the ZDepth (Z) or DepthCut (B) using the 
ZFeed (I). Subsequent milling blocks are then executed using the 
ToolComp (D) parameter and Feed specified. The feedrate can be 
changed in the blocks that are being milled. Tool diameter 
compensation cannot be changed from within the cycle. The cycle 
is terminated with the EndMill (G176) block; at which point, it rapids 
up to the StartHgt (H) and rapids to the X and Y location specified. If 
X and Y are not specified the tool remains in the current position. 
Activate a tool prior to Mill Cycle so the CNC knows the 
tool diameter.

If the "D" parameter is used for tool diameter 
compensation, the lines of code in the mill cycle must start 
with an uncompensated ramp-on move and end with an 
uncompensated ramp-off move as the first and last lines 
in the mill cycle are not automatically compensated by the 
cycle.

XStart

X

X coordinate of the start of the contour. If 
no coordinate is provided, default is set to 
the present position. (Uncompensated)

YStart

Y

Y coordinate of the start of the contour. If 
no coordinate is provided, default is set to 
present position. (Uncompensated). Move 
XStart and YStart below ZDepth.

StartHgt

H

Absolute Z position to which the CNC 
rapids before feeding into the workpiece. 
(Required)

ZDepth

Z

The absolute depth of the finished pocket. 
(Required)

DepthCut

B

Z-axis increment used for each pass.

ToolComp

D

Tool Compensation. Use Left or Right only. 
All other are no compensation.
Compensation LEFT
Compensation RIGHT

ZFeed

I

Z-axis feedrate (plunging feedrate).

Rough 
Feed

J

XY axes roughing feedrate. Defaults to last 
programmed feedrate.