Cycle 27 CYLINDER SURFACE (#8 / #1-01-1)

ISO programming

G127

Application

 
Machine

Refer to your machine manual.

This function must be enabled and adapted by the machine manufacturer.

This cycle enables you to program a contour in two dimensions and then transfer it onto a cylindrical surface. Use Cycle 28 to mill guide slots on the cylinder.

Describe the contour in a subprogram that you program with Cycle 14 CONTOUR.

In the subprogram you always describe the contour with the coordinates X and Y, regardless of which rotary axes exist on your machine. This means that the contour description is independent of your machine configuration. The path functions L, CHF, CR, RND and CT are available.

The coordinate data of the unrolled cylinder surface (X coordinates), which define the position of the rotary table, can be entered as desired either in degrees or in mm (or inches) (Q17).

Cycle sequence

  1. The control positions the tool above the cutter infeed point, taking the finishing allowance for side into account
  2. At the first plunging depth, the tool mills along the programmed contour at the milling feed rate Q12.
  3. At the end of the contour, the control returns the tool to set-up clearance and returns to the infeed point
  4. Steps 1 to 3 are repeated until the programmed milling depth Q1 is reached.
  5. Subsequently, the tool retracts in the tool axis to the clearance height.
 
Tip

The cylinder must be set up centered on the rotary table. Set the preset to the center of the rotary table.

Notes

  • This cycle can be executed only in the FUNCTION MODE MILL machining mode.
  • The memory capacity for programming an SL cycle is limited. You can program up to 16384 contour elements in one SL cycle.
  • This cycle requires a center-cut end mill (ISO 1641).
  • The spindle axis must be perpendicular to the rotary table axis when the cycle is called. If this is not the case, the control will generate an error message. Switching of the kinematics may be required.
  • This cycle can also be used in a tilted working plane.
 
Tip

The machining time can increase if the contour consists of many non-tangential contour elements.

Notes on programming

  • In the first NC block of the contour program, always program both cylinder surface coordinates.
  • The algebraic sign for the DEPTH cycle parameter determines the working direction. If you program DEPTH=0, the cycle will not be executed.
  • The set-up clearance must be greater than the tool radius.
  • If you use local QL Q parameters in a contour subprogram, you must also assign or calculate these in the contour subprogram.

Cycle parameters

Help graphic

Parameter

Q1 Milling depth?

Distance between cylindrical surface and contour floor. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q3 Finishing allowance for side?

Finishing allowance in the plane of the unrolled cylindrical surface. This allowance is effective in the direction of the radius compensation. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q6 Set-up clearance?

Distance between the tool face and the cylindrical surface. This value has an incremental effect.

Input: –99999.9999...+99999.9999 or PREDEF

Q10 Plunging depth?

Tool infeed per cut. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q11 Feed rate for plunging?

Traversing feed rate in the spindle axis

Input: 0...99999.9999 or FAUTO, FU, FZ

Q12 Feed rate for roughing?

Traversing feed rate in the working plane

Input: 0...99999.9999 or FAUTO, FU, FZ

Q16 Cylinder radius?

Radius of the cylinder on which the contour will be machined.

Input: 0...99999.9999

Q17 Dimension type? deg=0 MM/INCH=1

Program the rotary axis coordinates in degrees or mm (inches) in the subprogram.

Input: 0, 1

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 27 CYLINDER SURFACE ~

Q1=-20

;MILLING DEPTH ~

Q3=+0

;ALLOWANCE FOR SIDE ~

Q6=+0

;SET-UP CLEARANCE ~

Q10=-5

;PLUNGING DEPTH ~

Q11=+150

;FEED RATE FOR PLNGNG ~

Q12=+500

;FEED RATE F. ROUGHNG ~

Q16=+0

;RADIUS ~

Q17=+0

;TYPE OF DIMENSION