Cycle 273 OCM FINISHING FLOOR (#167 / #1-02-1)

ISO programming

G273

Application

With Cycle 273 OCM FINISHING FLOOR, you can program finishing with the finishing allowance for the floor programmed in Cycle 271.

Requirements

Before programming the call of Cycle 273, you need to program further cycles:

  • CONTOUR DEF / SEL CONTOUR, alternatively Cycle 14 CONTOUR
  • Cycle 271 OCM CONTOUR DATA
  • Cycle 272 OCM ROUGHING, if applicable

Cycle run

  1. The tool uses positioning logic to move to the starting point
  2. Positioning logic in OCM cycles

  3. The tool then moves in the tool axis at the feed rate Q385
  4. The tool smoothly approaches the plane to be machined (on a vertically tangential arc) if there is sufficient room. If there is not enough room, the control moves the tool to depth vertically
  5. The tool mills off the material remaining from rough-out (finishing allowance)
  6. Finally, the tool moves with Q253 F PRE-POSITIONING to Q200 SET-UP CLEARANCE and then at FMAX to Q260 CLEARANCE HEIGHT

Notes

 
Notice
Caution: Danger to the tool and workpiece!
The cycle does not include the corner radius R2 in the calculation of the milling paths. Even if you use a small overlap factor, residual material may be left over on the contour floor. The residual material can cause damage to the workpiece and the tool during subsequent machining operations!
  1. Run a simulation to verify the machining sequence and the contour
  2. Use tools without a corner radius R2 where possible
  • This cycle can be executed only in the FUNCTION MODE MILL machining mode.
  • The control automatically calculates the starting point for finishing. The starting point depends on the available space in the contour.
  • For finishing with Cycle 273, the tool always works in climb milling mode.
  • This cycle monitors the defined usable length LU of the tool. If the LU value is less than the DEPTH Q201, the control will display an error message.

Note on programming

  • If you use an overlap factor greater than 1, residual material may be left over. Check the contour using the program verification graphics and slightly change the overlap factor, if necessary. This allows another distribution of cuts, which often provides the desired results.

Cycle parameters

Help graphic

Parameter

Q370 Path overlap factor?

Q370 x tool radius = lateral infeed k. The overlap is considered to be the maximum overlap. The overlap can be reduced in order to prevent material from remaining at the corners.

Input: 0.0001...1.9999 or PREDEF

Q385 Finishing feed rate?

Traversing speed of the tool in mm/min for floor finishing

Input: 0...99999.999 or FAUTO, FU, FZ

Q568 Factor for plunging feed rate?

Factor by which the control reduces the feed rate Q385 for downfeed into the material.

Input: 0.1...1

Q253 Feed rate for pre-positioning?

Traversing speed of the tool in mm/min for approaching the starting position. This feed rate will be used below the coordinate surface, but outside the defined material.

Input: 0...99999.9999 or FMAX, FAUTO, PREDEF

Q200 Set-up clearance?

Distance between lower edge of tool and workpiece surface. This value has an incremental effect.

Input: 0...99999.9999 or PREDEF

Q438 or QS438 Number/name of rough-out tool?

Number or name of the tool that was used by the control to rough out the contour pocket. You can transfer the coarse roughing tool directly from the tool table via the action bar. In addition, you can enter the tool name via the Name in the action bar. The control automatically inserts the closing quotation mark when you exit the input field.

-1: The control assumes that the tool last used is the rough-out tool (default behavior).

Input: –1...+32767.9 or max. 255 characters

Q595 Strategy (0/1)? (optional)

Machining strategy for finishing

0: Equidistant strategy = constant distances between paths

1: Strategy with constant contact angle

Input: 0, 1

Q577 Factor for appr./dept. radius? (optional)

Factor by which the approach or departure radius will be multiplied. Q577 is multiplied by the tool radius. This results in an approach and departure radius.

Input: 0.15...0.99

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

Example

11 CYCL DEF 273 OCM FINISHING FLOOR ~

Q370=+1

;TOOL PATH OVERLAP ~

Q385=+500

;FINISHING FEED RATE ~

Q568=+0.3

;PLUNGING FACTOR ~

Q253=+750

;F PRE-POSITIONING ~

Q200=+2

;SET-UP CLEARANCE ~

Q438=-1

;ROUGH-OUT TOOL ~

Q595=+1

;STRATEGY ~

Q577=+0.2

;APPROACH RADIUS FACTOR