Cycle 29 CYL SURFACE RIDGE (#8 / #1-01-1)

ISO programming

G129

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 ridge in two dimensions and then transfer it onto a cylindrical surface. With this cycle, the control adjusts the tool so that, with radius compensation active, the walls of the slot are always parallel. Program the center path of the ridge together with the tool radius compensation. With the radius compensation you specify whether the control cuts the ridge with climb milling or up-cut milling.

At the ends of the ridge, the control will always add a semi-circle whose radius corresponds to half the ridge width.

Cycle sequence

  1. The control positions the tool above the starting point of machining. The control calculates the starting point from the ridge width and the tool diameter. It is located next to the first point defined in the contour subprogram, offset by half the ridge width and the tool diameter. The radius compensation determines whether machining begins to the left (1, RL = climb milling) or to the right of the ridge (2, RR = up-cut milling).
  2. After the control has positioned the tool to the first plunging depth, the tool moves on a circular arc at the milling feed rate Q12 tangentially to the ridge wall. A finishing allowance programmed for the side is taken into account.
  3. At the first plunging depth, the tool mills along the programmed ridge wall at the milling feed rate Q12 until the ridge is completed.
  4. The tool then departs the ridge wall on a tangential path and returns to the starting point of machining.
  5. Steps 2 to 4 are repeated until the programmed milling depth Q1 is reached.
  6. Finally, 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

 
Machine

This cycle performs an inclined machining operation. To run this cycle, the first machine axis below the machine table must be a rotary axis. In addition, it must be possible to position the tool perpendicular to the cylinder surface.

 
Notice
Danger of collision!
If the spindle is not switched on when the cycle is called a collision may occur.
  1. By setting the displaySpindleErr machine parameter (no. 201002) to on/off, you can define whether the control displays an error message or not in case the spindle is not switched on.
  • This cycle can be executed only in the FUNCTION MODE MILL machining mode.
  • 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.

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 on the ridge wall. The finishing allowance increases the ridge width by twice the entered value. 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

Q20 Ridge width?

Width of the ridge to be machined

Input: –99999.9999...+99999.9999

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 29 CYL SURFACE RIDGE ~

Q1=-20

;MILLING DEPTH ~

Q3=+0

;ALLOWANCE FOR SIDE ~

Q6=+2

;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 ~

Q20=+0

;RIDGE WIDTH