G171 Circular Profile Cycle
Anilam G171 Circular Profile Cycle cleans up the inside or outside profile of an existing circle.
G171 Xn Yn Hn Dn Zn An Rn Bn Sn In Jn Kn Pn
|X||X coordinate of the center. Default: present position. Optional.|
|Y||Y coordinate of the center. Default: present position. Optional.|
|H||Z absolute starting (rapid) height (must be 0.1 inch or 2 mm above surface to be cut into). Executed in rapid. Required.|
|D||Finished diameter of circle. If you enter a negative value, both the direction of cut and the starting and endpoints reverse. Required.|
|Z||Absolute depth of the finished profile. Required.|
|A||Setting for cutting on the inside of the profile (In) or the outside (Out). Selection required. 0=In, 1=Out.|
|R||Ramp distance used for each pass. Optional.|
|B||Z-axis increment used for each pass. Optional.|
|S||Amount of stock left by the machine before the finish pass. Default: 0. Enter a negative value to leave the stock without making a finish pass. Optional.|
|I||Z-axis feedrate. Optional.|
|J||Rough-pass feedrate. Optional.|
|K||Finish-pass feedrate. Optional.|
When executed, the CNC rapids to Ramp#1 starting position, rapids to H (StartHgt), then feeds to the depth of the first cut.
The machine feeds into the profile along Ramp #1, cuts the circle to the specified D (Diameter) then ramps away from the work along Ramp #2.
When cutting an outside profile, the tool ramps into the work along Ramp #1 and away from the work along Ramp #2 as illustrated in Figure
The Circular Profile Cycle automatically compensates for tool diameter. Activate the correct tool diameter before the G171 block.
If you enter a Depth Cut = B (Z Max.cut), the CNC executes the number of passes required to get from the H (Z Start Hgt.) to Z (Z Depth), cutting to the Depth Cut = B (Z Max.cut) on each pass.
When you enter an S (Finish Stock) value, the CNC leaves the specified stock on the profile and depth for a finish pass. The CNC finishes to the entered diameter on the finish pass. Enter a negative S (Finish Stock) to leave the finish stock without making a finish pass.
If you do not enter a J (Rough Feed) or K (Finish Feed) value, the CNC executes feed moves at the current feedrate. J controls feedrate of the roughing cycle. K controls the feedrate of the finishing cycle.